Autodesk Fusion 360 (Year 2025 + 2026) - Complete Beginners Guide

1. Course Introduction: Hi, everyone. My name is Chris and welcome to the Autodesk Fusion 360, year 2025 Complete Beginner's Guide. A bit of background to myself. I'm an automotive engineer with over 15 years of experience in design, and I've been specializing in military automotive applications since 2018. During my career, I've been working with different CAD programs and have found Fusion 360 to be the perfect choice for those wanting to learn three D mechanical design and especially for prototyping or three D printing projects. This beginner friendly course is designed to guide you step by step in three D mechanical design with Autodesk Fusion. By the end of this course, you will have the skills to use Autodesk Fusion for personal projects, three D printing applications, academic work, and professional engineering tasks. This course is divided into ten sections. Each one is organized in a logical order to build your skills and modeling techniques in this powerful CAD software. As we progress, you will learn how to navigate fusions, user friendly interfaces, create complex sketches and components, build three D assembly models, and produce detailed two D engineering drawings to industry standards. This course also features assignments and practice exercises. These will enable you to apply the skills and techniques that you will learn to generate complex level cad parts and assemblies. So whether you're an aspiring engineer, a professional working in the industry or a hobbyist exploring three D printing, this course is designed for you. So, let's dive into the world of three D mechanical design. This course consists of ten sections which are structured in an order that provides a progressive learning experience, enabling you to enhance your understanding of three D mechanical design in fusion software. By the end of this course, you'll have the skills and knowledge necessary to create a wide range of parts and assemblies at an intermediate level. So let's explore each of these ten sections. In the first section of this course, I will detail the contents of each section, which is this lecture now, and then I will walk you through step by step how to download fusion via the Autodesk website, and we'll take a look at the various licensing requirements and also the available options for acquiring a free license. Once you have fusion downloaded and installed, we'll move on to the second section, setting up your workspace. Here, we will study fusions user interface and the design environment. We will also cover how to create and navigate projects. And as a part of this process, we will create a dedicated project for this course and its contents. We'll then learn how we can change the settings within fusion to switch between metric and imperial units, I millimeters and inches. And finally, in this section, we'll learn how to adjust the grid settings and change the environment background. Now that we have our workspace setup, we'll move on to the third section and begin two D sketching. This is a fundamental topic when learning three D design infusion. And here we'll learn about the fundamental sketch tools, including the line tools, rectangle tools, hex tools, slot tools, circle tools, arc tools, and many more. Following this, we will explore the sketch modification tools that allow for precise adjustments within our sketches. Then move on to patterning sketches. We'll learn how we can implement linear patterns, circular patterns, and sketch mirroring techniques. Now we'll also give you a detailed overview of sketch constraints and how they can be used to accurately define geometry based on specific requirements. We will then cover dimensions and controls before moving on to three assignments. Now, these are designed to give you the opportunity to apply the tools and techniques covered in this section. These assignments will test your knowledge of sketching for mechanical design. And should you have any questions during these, please don't hesitate to send me a message. Section four is where we will begin three D modeling. We'll start off with the extrude tool and learn how to add and remove material based on the profiles created from our two D sketches. We'll then take a look at the revolve modeling tool and understand its application based on part geometry and features. Then we'll study the sweep tool and identify when and where to use it effectively based on the parts design requirements. We'll then learn how to add engraved or embossed texts such as logos, brands, part numbers or similar features. Moving on, we'll study shell and whole features and how to apply threaded features, including both male and female threads. We'll then study how we can assign materials to parts and customize their appearance for a more realistic representation. And of course, we'll study the rendering environment built into fusion as well. You will then be provided with three D modeling assignments. Each assignment involves creating a three D model based on defined dimensions at the start of each lecture. These exercises are designed to test your ability to apply the tools and techniques learned in this section. Now I'll also demonstrate a technique for modeling each one of these exercises. If you have any questions during these assignments, please do send me a message. In Section five, we focus on creating assemblies by combining individual three D model parts. We'll start with modeling each component of a pulley assembly, and I will guide you step by step through the process of designing these parts with predefined dimensions. Once the individual parts are modeled, we will then place and learn how to position each part. After the parts are placed, we will study how to use the joint command and assign the various types of rigid and revolute joints to build the complete assembly. Todos fusion is provided with a complete content library. So we'll take a look at the vast collection of premade standardized parts and learn how we can insert them into our assemblies to streamline our workflow. Then we'll learn how to create cross sectional views to visualize and analyze parts that may otherwise be difficult to see within an assembly. Also, we'll learn how to toggle and adjust the visibility and transparency of individual parts or subassemblies to improve clarity and focus during assembly design. We'll then explore how we can pattern parts within assembly files, focusing on both linear and circular pans. Finally, we'll cover how to edit existing assemblies, including modifying joints, repositioning parts, and making necessary adjustments to achieve the desired results. Section six is a project where we will create a generic design of workbench, as we can see here. We'll use various sketch techniques to incorporate the dog holes on the worktop and offset rigid joints to position the braces and aprons. All the dimensions are pre calculated and we'll go step by step in creating each component and building the entire assembly. Section seven is another project focused on modeling and creating an STL file of a three D printed phone stand. If you are using a multicolor three D printer, I have included a technique to generate separate bodies and faces to assign the correct filament colors. Otherwise, this can be printed using a single filament printer in one piece. We'll also model in a generic smartphone which can be three D printed. This is more for sketching and modeling practice, but I feel it's a good exercise to expand upon your sketching and modeling skills. In Section eight, we'll be creating two de engineering drawings. We will begin by learning how to create drawing files, linked to parts or assemblies, and how we can customize them, such as adding new sheets and defining title block attributes. I've also included lectra specifically on creating your own title block where you will be able to create your own tailored to your company, your clients, or your academic requirements. Using the Pulley assembly modeled in a three D modeling section, we will insert a base view, project additional views from it, and also create section views. The process will also cover how to switch between first and third angle projections within two D drawings. For each view, whether base or projected, we will learn how to adjust the associated styles, add labels, and include essential information. Following this, we will learn how to insert dimensions and modify drawing preferences. Once the dimensions are added, I will demonstrate how to apply linear and angular tolerances. For assembly sheets, we will also cover how to add a pas list and use identification balloons to correlate parts within the pars list and any related details. And finally, I've included a complete example of generating a two D drawing for the Pulley assembly modeled earlier. In Section nine, it will explore some additional content, not necessarily required for previous assignments, but useful for understanding some further capabilities within fusion. We'll start with an example of modeling springs and spirals using the coil command, and after that, we'll take a look at loft modeling, which allows us to create complex geometries and faces. And next, we'll learn how to split bodies within apart. And finally, I'll provide a 30 minute overview of auto Des fusion. I created this for American students in 2024, and I feel that it's a good sort of getting started summary. In Section ten, this includes plenty of practice modeling exercises, and it's a good summary of all the tools and techniques learned within this course. All the dimensions for each exercise are provided, so feel free to have a go at modeling these yourselves, and I will also be providing a complete demonstration on how we can model each one of these parts or assemblies. Overall, this course provides a clear and logical overview and structure for learning auto sfusion for professional purposes. Upon completion, you will reach an intermediate level. You will be capable of sketching, modeling, assembling, and creating two D engineering drawings to professional standards. If you have any questions, please feel free to contact me, and I wish you all the best in your future endeavors in CAD design. So I look forward to seeing you in the course. Thank you. 2. Downloading Autodesk Fusion: In this lecture, we'll learn how to download Fusion 360. So for this, we'll be working on the Autodesk website, and we will take a look at options for free licenses, Fusion limited, educational licenses, free 30 day trials offered by Autodesk, and also the subscription plans available. So to do this from your desktop, if you open up your browser, but today I'm working in Chrome, in the search bar, if we enter Autodesk, and then click Search, you should then see the very first option. It's autodesk.com. But this is the American site. It should be exactly the same, either in Europe or elsewhere in the world. Once the link has opened, we want to come up to the very top where we've got products, pick the drop down there, and then immediately Autodesk will be promoting their packages. So a package for CAD design here, including various softwares, package for architecture, instruction, media entertainment and so forth. You'll also see on the right, got to start a trial, download your software, what you need to be already in possession of a license for and various other options. But for now, we ought to come down to view all products and take a look in depth at the options available for autodesk fusion. So let's click once the page opens, if you scroll down, you'll see all the various Autodesk softwares starting off with AutoCad, AutoCad Lite, Fusion, which we'll be focusing on today. They've got packages in here as well. Autodesk inventor, RDS Max, and so forth. But as I say, today, we're going to be focusing on autodction, and immediately they're trying to promote their subscription plans. We're not so much interested in that for now. Let's take a look at all the options. Let's select Fusion, LetclickO. And now we're starting to see more of the available options to us. So immediately at the start here, we have the option to download a free trial, and then down here again, they're promoting their subscription options. Let's go on download a free trial, Left Click ones. And then within the free trials, there are three options. Now, number one is a free 30 day trial, and that's the full package for all features and all functionality. And I would recommend downloading this package if you are investigating fusion, if your company is interested in fusion, or you're thinking about pursuing cad design with fusion. The next option we've got is what I call fusion LT, Fusion Light fusion Limited. This is really for hobbyists. So this is a free license, okay, free access to fusion. However, it does have limited functionality. It is more intended for hobbyist users. I've never used the limited version of fusion, and I wouldn't really recommend it because we don't want to be running into any limitations when we need to use perhaps certain tools or features or methodologies when we're working in CAD. Then the last option available here, and this is another free license type, this is for educational use. So if you are a registered student at an educational institution, you can have free access to a full, complete license for full features, full functionalities for students, and also educators as well. So if you are teaching engineering or such or you're teaching at an educational institution, you can unlock educational access here. I do believe you need to provide some sort of documentation or proof that you are a registered personnel at such an institute, and then once approved, you will have access to the full license. So in terms of downloading fusion and acquiring an appropriate license, it depends on where you stand currently. I would always recommend starting the free trial, whereas if you're a student or an educator, jump straight into an education license, or if you are working for a business and you're intending to use CAT software for the purposes of business development, it will be worth looking into a subscription plan. And if we come down to the three plans here, I would definitely recommend the one year annual license. So right now it is a discount of $476 per year, which equates to about $40 per month. So depending on your circumstances, you can select the appropriate, either a license or you can select the free trial. So if we select, start a free 30 day trial. So from here, you can enter your email address, register an account, and then once that's complete, you can come up to products, come across to download your software, and then from there, you need to sign in, and you'll be able to download Fusion 360 under that appropriate license. Okay, I hope that all makes sense. Any issues, please send me a message. Aside from that, I will see you in the next lecture. 3. Workspace Introduction: In this section, we'll learn how to set up our workspace. We'll start by studying Fusion's three D environment, its various tabs and toolbar locations, and how we can create new projects. I recommend creating a new project specifically for this course, and we'll keep all of our example models and assignments in a single location that's easy to navigate. In addition, we'll learn how we can switch between metric and Imperial measurement units, I E millimeters and inches and also adjust the modeling environment settings such as the grid and the background colors. So let's set up our workspace. 4. User Interface: In this lecture, we will open fusion and review the key components of the user interface, including the three D environment, display tools, browser, tabs and tools, and last but not least the ViewCube. So once we've opened up fusion, as we can see here, straight away, we are presented with the modeling environment. So in the very center, we have the three D environment, and this is where we will be sketching, re modeling, and creating our assemblies. It is the main focus of modeling in fusion. At the bottom, we have a panel of display tools and viewing tools such as pan, orbit, Zoom, et cetera, and we'll be covering each one of these and their keyboard or mouse shortcuts throughout this course. The left hand side, we have the browser. Now, this organizes all of our design elements, such as parts, document settings, and the default axis and planes, and we'll be sure to be using these throughout the course also. At the top are the tabs. So the two main that we will be using within this course are called solid and sketch, which are essentially three D modeling and two D sketching respectively. And under each tab is a series of tools relating to that tab title. And on the right hand side, just up in the corner, we have the view cube, and this is a really useful tool that helps us to orbit and orientate parts or assembly for better viewing angles, and we'll be for sure using that a lot throughout this course, also. So that is a quick overview of the key elements of the user interface. Throughout this course, we will be learning more about each one and how they are utilized to allow us to design and create as we need. The more that we use fusion, the more that we will become more fluent in the software. Now let's move on to the next lecture and create our very own first project. 5. Create Your First Project: In this lecture, we will create our first project. And I would always recommend creating a new project for different projects that you're working on, as this will keep each related part file together alongside any related assemblies and drawing files. So this will give you the quick and easy access to everything in one area. So to create our new project, we're going to come up to the top left where we have the nine squares here, which is our data panel, Left Quick that once. And you'll see on my screen here that I've got a number of projects that I've already created. So I've got my automotive, my fusion course project, general applications, military personnel, et cetera. All of these projects are stored within the Cloud, and that's one unique thing about fusion compared to traditional CAD programs is that every file you work on is cloud based, whereas programs like Autodesk Inventor or Solid Works would keep files either locally or stored within some sort of vault. I really like that about fusion, especially if you're working globally or you want to share files around the world. It's really fantastic for that. It's also quite safe and secure. You've got that backup there online. So to create our new project, let's come up here. Let's select new project. And then you can name this how you like. So for me, I call it Fusion Course Project. So I've obviously already created this, and I've got all my content within there. So feel free to call that Fusion course project or how you like. And then once it's created, if you double click on that project, it should be completely empty with inside. And as you work your way through this course, you can add each of the files and assemblies, examples, exercises that we work on. A few options we have here when it comes to the interface, so we can open on the web. So if we select this, it's essentially exactly the same, but on the web, and there are a few more options available on there as well. It's very rare that I use that. But if you prefer to navigate through your files online, then you can open on the web here. And you've also got the COG app here as well, which enables you to sort. So last updated name, also view differently as well. So it was a grid or a list. I typically view as list and I sort by name, but feel free to adjust those how you like. And that is how we create a project, and I would advise you to zap all the files within this course within that single project, and we'll be referencing them throughout this course. Thanks for watching, and I'll see you in the next lecture. 6. 2026 Updates Design Files: Hi, everyone, Chris, here. I hope that you're enjoying the course so far. I created and published this course at the beginning of 2025. And since then, there have been a number of updates that Autodesk have introduced for fusion software. One of those updates I undercover in this lecture. It's a very small change, and it has almost no impact for the remainder of this course, but it's still relevant, and I think that it's something we should discuss. Let's take a look. Starting from Fusion's 2026 updates, when we open fusion, we can see this window up here, which asks us what do you want to design. And here we must select the appropriate design file based on what we are creating. Most important and commonly used design files are the first three, part design, assembly design, and hybrid design. So in this lecture, I will explain what these three are and when we should use them. Let's start with part design. This design type is used for designing individual parts. For example, we would use a part design to model this base plate or this bracket or this bolt. For assembly design, this design type is used when we combine parts together to form an assembly. For example, we can insert all of the above part designs and position them accordingly to form an assembly, like we can see here where we have the base plate, the bracket, and in this case, I've added two bolts. Then we have hybrid design. Now, this is the original fusion file type. So before 2026, this was the only file type available. In hybrid design, you can model individual parts and form assemblies all within the same file. So at this point, you might be asking, can we use hybrid designs for every part and assembly? And the answer is yes, you can. It gives us most flexibility and control for efficient modeling. However, for intermediate or advanced users, it can give some limitations when it comes to editing individual parts or salssembies. I won't go into too much detail at this point on the course. For the remainder of this course, I will be using the fusion default file type, which is hybrid design for every lecture. So what should you use? My recommendations are if you are new to fusion CAD modeling, then choose hybrid design for every lecture throughout this course. This gives you the most flexibility when designing parts and assemblies and as the design type that I have used in this entire course for every part and assembly that I will create. However, if you are coming from a solid works inventor or other CAD background, I recommend choosing part design for individual parts and assembly design for assembly files. Now, this is the traditional bottom up approach that's used for complex assemblies and project management. So if you're coming from a solid works or inventor background, it will be a lot easier for you to transition to fusion if you are already accustomed with this workflow. Now, if we go back to the design type box, you'll notice there are other design files such as drawing. Now, this is intended for two D engineering drawings. This course features an entire section on drawings, which is Section eight, so I'll explain this design file there. And next, we have electronics design and the electronics library. Now, these are very bespoke design modeling environments for circuit board and component design. We'll put those aside for now as we're primarily focused on two D and three D mechanical design. Once you have selected either hybrid part or assembly as the design, just double check the options on the right hand side. Make sure to select standard as the default file type. And for the unit system, I will be using millimeters and grams for every lecture, but feel free to change as you prefer. I hope that makes sense, but if you have any questions, please don't hesitate to comment either on this video or you can send me a direct message. In later sections on this course, I will revisit these design file types, and you will understand more about CAT model structuring and workflow. So I'll see you in the next lecture. Thank you. 7. Design Files Switching Between them: In this lecture, I will show you how the user interface changes when we are using part design, assembly design, and hybrid design. I'll then show you how to tell which design type we are using and how we can switch between the file types if we've selected the wrong one. So let's open up fusion, and for example, let's go with a hybrid design. Make sure our unit system here and when to use Metric, in this case, millimeters and grams to create new. So from here, if we come over to the left hand side, you'll see here, we've got the browser, and then under the document settings, it identifies here hybrid design. Now, let's say that perhaps in the future, you want to change that. So we click on the Convert icon there, and then over here, we have this toolbox that pops up, and under design type, it states hybrid, we can change that. So we could jump into part, for example. Now, before I demonstrate this, I just want us to take a look at the tool bar at the top here. So in all of my lectures in this course, I'm using the hybrid design, so the tool bar will look the same as this. But watch how this changes. Let's select Let's go on assembly and click Convert. Now, the tool bar here looks very different, and these tools are all related to forming assemblies. If we then change that, let's go on to part design, click Convert. You'll see here that all the tools are in relation to designing individual parts. So it's just one thing to keep in mind and to appreciate when you're selecting the design type. But for me, I'm going to stay on the hybrid as I've done in this course, click Convert and use this tool bar, which features all of the tools required for individual part design and for assembly design as well. Okay, I hope that's all clear, and I'll see you in the next lecture. 8. Setting Units, Grid Settings & Environment: In this lecture, we will learn how to switch between units. So I mean metric and imperial, commonly millimeters and inches. So we will learn how to do this in our individual designs and also how to switch units for permanent use. So by this, I mean in the user settings. So once we've opened up a new design like here, we can tell what units we're working in by coming over to the browser. And under the browser, we've got one folder here, which is document settings. If we hit the drop down next to that, it'll then detail to us what units that we're currently working in. So currently I'm working in millimeters. And if we want to change this, we can just simply left click on change active units, and our tour boox pops up. We can select here centimeters, meters, inches, out foot. So I'm going to stay in millimeters for the time being. So this is how we change units for an individual design. I'll only be applicable for this design here and not for any others. But if we want to make a permanent change, all future designs to be in a specific type of units, we can come up to the top right under where our profile icon is, if we left click on that and then hit preferences, they have many tools pop up here that you should be studying on the general settings here, so you can change to the language and so forth. We won't go through all of these, but we will be covering quite a few throughout this course. But in terms of units, we come down to the bottom, and we have the default units. So under here if we come under design, which is what we're going to be working on in this course. And here we have the option to set the default units for new designs. And again, I've got these in millimeters, but you can switch between these as you like. For example, if I change to inches and select apply, okay. Then start a new design by just selecting the new design button up here. So we're in our new design now, and if we come over to the document settings, hit the drop down. You'll then see that we're working in inches. Okay? So I'm going to switch that back to millimeters, come on the default units design, that back and mill apply, okay? Close down that design, start a new one, and just make sure that's in millimeters as begin to see here. So those are the two methods for switching units. Let's now take a look at our environment, and you see here that we have this grid. Now, many students have asked me previously how they can turn off the grid. The grid is there as a reference point, and it's good to help with three D visualization. I understand that it can be quite distracting. So in terms of turning this off when we are in design mode, we come down to our display tools down here where we have grids and snaps. Just hit the drop down there, and we've got this option here to turn off the layout grid. And then we can continue design in just a plain environment, like so. Another option we have here as well is grid settings. So if I turn the grid back on, then go to grid settings, we've got a toolbox pop up here, we've got the option here to have the grid as being adaptive or fixed. For me, personally, if you keep the grid on, I would recommend keeping it adaptive. So what this does is it adapts according to how far you zooming out or zooming. It depends on the scale on which you're modeling. If you're modeling something very large, it will adapt accordingly. Otherwise, if we have it as fixed, we can actually fix the major grid spacing. So in this case, if I change that to 500 mil, you can then see the grid has changed to 500 mil spacing and the minus subdivisions. If I change that to let's say two, I'm going to press Okay. I'll then need to zoom out so that we can see the scale of the grid now. So we have 250 mil going on half a meter and in the other direction. Recommend for me personally, grid settings, I usually keep the grid on, and I recommend keeping it on adaptive, pressing okay. And then, regardless of the scale we're modeling, the grid will adapt accordingly as we can see that I'm zooming in now. Just a reference, by the way, I'm using the mouse wheel to zoom in and zoom out. The way you see me panning around, I'm using the middle mouse button. We'll cover all those details in a later lecture alongside a few keyboard shortcuts. Now let's take a look at the environment and some of the display settings. So if we come down to the panel at the bottom and then under display settings, hit the drop down there. And first, let's take a look at environment. So right now, I'm in photo booth. You see it's a white background. I'll give an example here. Let's select gray room. And there we're working in a gray background. Let's try one more. It's going to tranquility blue. We've got that nice blue background there. I typically work in photo booth, but it's completely up to you. What your preference? I like to have the white background for me personally. Also the display settings, we've got some visual styles. So to better demonstrate this, I'm actually going to open an existing part. So this is a fastener that I've drawn previously. Going to use this as an example to show you about the visual styles. So the default is shaded with visible edges, okay? So we can see the edges there are highlighted in black. We've got options here to change the visual style. So you may want to just have it shaded with hidden edges, okay? So shaded part, and then we can see the hidden edges. Another option there is just shaded, so that's where the edges are not so visible. We've also got the option for wire frame, and also wireframe with hidden edges and with visible edges, okay? Like, so the visual style that I prefer to model in is shaded with visible edges only. So I think that's sort of visually the most easy to read parts and assemblies in. And the last setting I want to show you whilst we've got this part open are the view ports. So if we hit the drop down here and go on multiple viewports, we can then see we've got our sort of ISO view at the top right here, and we've got our front view, top view, and side view. And this can be really useful if we're communicating with clients or working with other team members, other engineers, other students, et cetera. So another option there in which we can work with our parts. And even within each viewport, we can edit them. So, for example, if I jump over to we're now looking at the top view, okay, I can move this around and make any edits or show any visuals, likewise, for the others. If we want to leave the viewports, we just hit the drop down again, and then just go on single view. Then we're back to our original part in a single view. Okay, I hope that all makes sense in this lecture. And again, if you have any questions, please send me a message. Aside from that, I will see you in the next lecture. 9. Sketching Intro: In this section, we will learn all the fundamental elements of sketching. Sketching is essential to three D modeling, and Fusion provides many sketch tools that enable us to construct high quality sketches to then later three D model. We'll start by understanding all of these sketch creation tools, their location on the toolbars and their keyboard shortcuts. We'll then study the sketch modification tools, pattern tools, and very importantly, sketch constraints. The end of this section, there are three sketching assignments for you to test your knowledge and capability to sketch infusion. All the tools required to model these sketches are taught within the following lectures. So I look forward to seeing how you get on with these assignments. Each lecture in this section is presented step by step, and I will walk you through how we can use these sketch tools for common practices. I'll be giving a range of examples throughout the lectures, which I recommend you follow along with me and take the opportunity to practice these tools and familiarize yourself with what they are used for. In the following sections of this course, I'll be regularly using the tools covered in this section, and so will you. Regarding the design file types, which one should you use? Again, if you're new to fusion, I recommend within this section for every lecture to use hybrid design. So that's the same as me. I'm going to be using millimeters and grams. And then for those of you who have worked previously with Solid Works or inventor and want to follow the same workflow as in those CAD programs, I would recommend going for the part design selecting standard, and then you're according units here. So let's start sketching. 10. Sketching Planes, Lines & Dimensions: In this lecture, we will create our first sketch, and we're going to be using the line tool. We'll start by understanding which default plane we should start our sketch on and then we'll create a basic sketch using the line tool and apply both linear and angular dimensions to fully constrain it. And then finally, we'll finish the sketch by saving it within our project folder. So now we've got Fusion Open. Let's come up to the top where our tabs are, come under solid, and the very first option there is to create a sketch. Left click that once, and now we're presented with 32 dimensional planes, which we need to choose one of them to do our sketch on. So this one here is the X Z plane. This one here is the Y Z plane, and this one here is the XY plane. A lot of students have asked me previously, which plane should I do my sketch on? Now, there's not necessarily a right or wrong answer here. It depends on the orientation of the part. Example, if I'm modeling this part here, let's say it's some sort of bracket base plate, in this orientation, I would model it on the XY plane. So when I apply this to my assembly, it will automatically be in the correct orientation. Whereas if I were to model the same part, but in this orientation, I would be modeling that on the X z plane. And likewise, if I were to model the same part in this orientation, I would model that on the Y Z plane. We'll learn more about default planes as we progress throughout this course and create more parts, and you'll become more familiar and accustomed to choosing the more appropriate plane to draw on. But for the purposes of this lecture, we're going to start with the XY plane. So let's left click on that once, and now you'll see we're looking perpendicularly to that two dimensional environment. And if we look up to the top where our tabs are, have a new tab there, which is sketch. And underneath this tab, we have many tools in relation to sketching. For example, we have the creation tools, modification tools, automate, which relates to fusion, applying automatic dimensions and constraints. We've then got the constraints, configure inspection tools, ability to insert parts or images, various selection tools, and the option to finish the sketch. So within this section of the course, we'll be covering all of the core tools available here, including many that are in the drop downs as well. So we're not just limited to what's available here. We've also got additional tools here which perhaps might not be as regular used. Let's start off with a line tool then. We'll come under our creation tools, and you'll see the first option there is line next to it, two point rectangle, then to diameter circle, spline tool, mirror and dimension or various other tools in there. So the line tool is the very first one. It's the most commonly used tool, the shortcut for that is L on the keyboard. So if I come over to the workspace and I hit L on the keyboard, you can then see the line tool is selected and I'm now using the line tool in this environment. At the very center here where the two axis cross. So that's the X and the Y axis. This is called the origin, and that is 0.000 on the X, Y, and Z axis, and it's typically where we start sketching. I'm going to start my line sketch from the origin. I'm going to left click once, and I'm going to drag out my line. Immediately here, we can see we have two parameters which we can control. Number one is a dimension and the other one is an angle. So we can choose either to add in a dimension at an angle or we can just left click anywhere in the environment. So if I just left click here, for example, we have now this blue line in place. I'm going to hit Escape on the keyboard, on this line, I'm going to hit Delete, and then I'm going to hit L on the keyboard and redo that. Let's start from the origin, come across, and now let's input a dimension. Let's go for 50 millimeters. I'm going to type in 50 on the keyboard. And then if we move the mouse around, you'll see that that dimension is locked in place. So we have a line that's 50 mill in length, that linear dimension there, that is the angle that we still need to input and control exactly where this line is going to be. So that angle is in relation to the X axis, and how we control that is by hitting tab on the keyboard, and now you can see it's highlighted, and we can insert an angular dimension there. So in this case, I'm going to type in 45 degrees. Then I'm going to hit Enter on the keyboard. Now we have this fixed line in place 50 mil in length, 45 degrees from the X axis. Now notice as well that the color is black, and the two endpoints are black circles as well. So what that color indicates is that this entity is now fully constrained. It's not possible to change its angle or dimension. It cannot be moved. Now we can change these if we want simply by double clicking. So 50. If I change that to, let's say 75 and the angle double click, let's say 30, they can change it like so. We can then press Control Z on the keyboard if we want to go and now we're back to our 50 mill linear and 45 degree angle line. Let's continue sketching then. I go to hit L on the keyboard again, go back to the line tool. I'm going to bring the mouse over and snap on to the end of our line here with that blue box up here. I'm going to drag to the right hand side, and you'll see we're snapping to the grid. If you want to turn off grid snaps, come down to the grid and snaps, then you can turn off snap to grid. But for me, I'm going to keep that on throughout this course. I'm going to come across, and I'm just going to drop the line. Let's just say somewhere here, bring this line down again, left click once. Across here. Left click. And now I want to finish off my sketch and generate a closed profile so to do this. I'm just going to simply left click once at the origin again. And now you can see we've got this shaded blue area, which is our closed profile. I notice that we're still in the line tool. There are different ways to exit the line tool. We can hit exit on the keyboard or we can right click and press Okay, and now we've left the line tool, we're free to use any other tools. So now we've created a basic sketch. If we then look at the color of these lines, we can see this one is black. This one is black. The other two lines here are both blue, and that indicates that they can move. Okay? So we can move this line like on the X axis and this one on the y axis. We want to constrain those in place. But to do that, we want to apply dimensions. Let's come over and do our create tools again and let's select sketch dimension or shortcut D on the keyboard. So if I hit D, and then going to select this line here, click once, bring that dimension out. Left click again. I'll apply a dimension there. Four, 50 millimeters, press enter. See where we are there. So this line has now turned black, and it's not possible to move. I hold down the left mouse button. Can't move that line. This one is still moving on the X axis. There's control here would be the length of this line. So I'm going to hit D on the keyboard again. I'm going to put an in dimension on this line, bring that down, add a dimension there of 80 millimeters press enter. Okay, I'm going to press exit and leave the dimension tool. And now we have a fully constrained sketch. Okay. All our lines, all the endpoints are black in color. We have our closed profile there. That's looking good. One more thing I want to show you, as well, I let's go for the shortcut L on the keyboard, I'm just going to start anywhere in the environment. Left click once, and I can continue drawing like so. Left click again. And then I'm going to left click one more time, let's say here. Let's say that I want to end the sketch there. Mag, I don't want to generate closed profile. Options we have here is to press exit on the keyboard, right click, select Okay. Or another option is to just left click once on this green tick here, we're telling fusion that we want to finish the sketch. And now we're no longer drawing lines from the endpoint here to escape on the keyboard and we've completed that sketch there. If we ever want to remove any entities, quite simply, we can left click, press delete on the keyboard. We can also select them as well. If we hold down the left mouse button and drag across a line, we need to make sure that the entire line is encapsulated within the square. We can then hit Delete on the keyboard. And then another option as well, if we left click and drag up like this, notice that it's a different colored square. So this one here is kind of orange with a purple border. One here is yellow with a dash border. What this means is that any entity that comes into contact with this area will be selected. If I let go now, you'll see we've selected that line. But if I do the same thing and drag across like this and let go, I've not selected it. It's a really useful tool when we're working with fusion. Just drag across like this. Maybe I have selected it, hit the lead on the keyboard, and now we're left just with our sketch there. So now we've completed our first sketch. Let's go ahead and save that. We come up to the top left. We're going to hit Save. Now we've got the option to give it a name. So, in this case, I'll just say first sketch, and then location, we just want to make sure the correct project is selected. So our fusion course project, save. And let's go into our nine squares up here. Then you'll see our first sketch has just appeared here. I've also got the bracket in there that I threw into this lecture earlier. But yeah, you should just have the first sketch on its own in that project. Okay, so that's the basics of the line tool and adding dimensions and having fully constrained parts. We're going to move on in the next couple of lectures and go through the remainder of the creation tools, then we'll do modifications, constraints, and so on. So I'll see you in the next lecture. 11. Sketching Rectangle Tools: In this lecture, we will learn how and where to use the three types of rectangle tools. So these are the two point rectangle, three point rectangle, and the center point rectangle. So to demonstrate this, I will work in a new design. But if you want to work from the previous file where we did the line tool, if you've got that open, great, if it's not open, no worries. Come up to the show data panel. Make sure you go to home and then select the according project. In this case, Fusion course project. And you should have the file that we called first sketch there, right click and select open. But for me, I'm going to work in a new design for this one. So let's come up through the top left. Again, under solid. Let's hit Create sketch. And for this, we could choose any plane, but I'm going to go with the XY plane in this case. And let's go up through our Create tools, and then you can see there we've got the two point rectangle, which is the shortcut R on the keyboard. Now, if we hit the drop down, and then we come under rectangle here, you see there are three options here. The two point rectangle, which is the standard. That's the most commonly used type of rectangle, the three point rectangle, which I very rarely use, only in some instances. And then we've got the center rectangle. And that's a fairly commonly used tool as well. So we've got the shortcut R on the keyboard. And then if we look on the right hand side, we've got the sketch palette, so I'm just going to bring that to center now. In terms of feature options, we can actually pre select which type of rectangle we want, 2.3 point or center. So just by hitting R on the keyboard, we can then just quickly choose there as opposed to going to create rectangle and then choosing the appropriate one there. So put the palette over there for now. So again, I'm going to start from the origin. Going to pan across by holding down the middle mouse button. And I'm going to start at zero, 00. That's the origin. I'm going to bring the mouse out. And as we can see here, we're forming a rectangle. And again, just like the line tool, we've got parameter options, which we can input. For this particular case, I'm going to put in 80 millimeters, and let's do that by 40 and height press Enter, and there we have our complete profile there, a rectangle that features all black lines, that's fully constrained. Notice these symbols that will pop up here. Now, these indicate constraints, which we'll be covering in a later lecture, but just to give you a bit of a heads up, this symbol here represents a horizontal constraint. Now, this symbol is tied to this line. So this line is indefinitely horizontal, so we cannot change the angle, cannot make it vertical, or that is horizontal and likewise, the same with this one. So that's one of the powerful features behind using the two point rectangle tool. Likewise, for the vertical lines, you'll see this symbol here, same symbol, but just in a different orientation. So it being vertical here indicates a vertical constraint on this line, and the same is also apparent on this line as well. It's a fantastic tool, and it's much quicker than drawing out a rectangle with the line tool and then perhaps having to add individual dimensions and constraints on top of that. So it's a quick way to show rectangular geometry. I go to pan across now, and I want to demonstrate the next rectangle tool. Let's go for the three point. So I'm going to press R on the keyboard, then under my sketch palette, I'm just going to click three point rectangle, throw that back over there. I only click once. So not the origin this time. We're just going to go sammer on the Xaxis. So it's called three point because we do three clicks? We identify three locations for this rectangle to form. So we got the starting point, which I've clicked already. Now I need to do one more left click, which I'm just going to do anywhere. Let's say here. I need to do one more click now. And if I draw the mouse out, I then need to define the height. So in the first two clicks, I defined the angle and also the length, and then in the third click, I define the height. I'm just going to put that in its 50 mil for now. Again, I very rarely use the three point rectangle. It's only in certain cases, but you may find yourself using this more and more regularly, depending on the geometries that you're regularly drawing. Now notice again here that this rectangle is completely blue. All edges and all the corners are all blue. That means we can move it anywhere. So if I hold down the left mouse button at this point, for example, I can move it. And also, we don't have a dimension on this line. I got to go ahead and add that press D on the keyboard, select this line, put a length in there of 110. Then if I try that again, so the dimensions are fixed, but in this case, I'm able to move that around, and that will be so until we anchor down one of these corner points here. So that's the three point rectangle. Now I'm going to press R on the keyboard one last time, and we're going to take a look at the center rectangle. This is quite a commonly used rectangle where we only need to identify two points to define the rectangle. So the very first being the center. In this case, I'll just select on the x axis there. And my second point then will define both the length and the height. So I've got control of that corner point there, or I can input dimensions. So in this case, let's go over 150 p. Let's go 80. Then I can also control the position of this rectangle using the center of the rectangle. I can hold down the left mouse button, and I can move that around to say, wherever it would need to be. And we see here as well that it's also input a number of constraints. So this type of constraint here is called the parallel constraint. So this is parallel to this line here. And likewise, with these two vertical lines, then down here, we've got one more constraint which is perpendicular. So we've got that 90 degree angle there. I like to use the centerpoint rectangle whenever I'm mirroring entities because I've got the center point of it identified already, so I can do any mirror lines down the center or across the horizontal, we'll be doing that in a later lecture. But those are the three rectangle tools. Again, the most common is the two point rectangle, it sits right up here, and it's the first selection when we hit R on the keyboard. Next most popular would be the centerpoint rectangle, and then the third only for special cases, we see the three point rectangle. So we'll be using rectangles in the later examples, and I will see you in the next lecture. 12. Sketching Circle Tools: In this lecture, we will learn about the functions of the five types of circle tours and I'll demonstrate each one of these. So these are the center diameter circle. We've then got the two point circle, three point circle, and then we've got the two tangent and the three tangent circle, as well. So I've opened up fusion. I've started a new part, and as you can see here, I've input some geometries already. That's going to help me to demonstrate the functions behind each of these circle tools. So let's come up to our creation tools, to the drop down the circle. We see that the shortcut for the center domed circle is C. So let's go ahead and hit C on the keyboard. Now, just like the rectangle tool, our toolbox pops up and offers us the different variations of circle tool. I'm going to put that toll aside for now. Let's go ahead and use the center diameter circle. So this is the most commonly used type of circle. So to demonstrate this, I use the square that I've drawn in here. And the very first click that we define is the center point of that circle. And as we bring the mouse out, we can start to see the circumference form. We have the option at this point to enter a diameter into the parameters box or we can snap onto existing geometry. For example, I've drawn this square in place. I could snap on to the midpoint of this horizontal line, or I could even snap on to the corner point of the square if I left click there. So if I left click there, we've then got our circle in position. The next tool we're going to take a look at is the two point circle. So if we come over to our box and select the two point circle, just zoom out pan over a bit, the two point circle, the very first point we define is a place on the circumference of the circle. If I left click at the end point of this line here, that's one position of my circumference, and then you'll see the next click wherever that may be. Will be the other circumference. So that will define the diameter. So in this case, I could snap onto existing geometries, or I could just input a diameter. In this case, I'm just going to snap on to the midpoint of this line here, or left click there, and there we have two point circle. So the next we have the three point circle. So principles exactly the same as the two point, except on this occasion, we're actually identifying three points on the circumference. To demonstrate this, if I select, let's say, the endpoint of this line here as one position or my circumference, another point as the endpoint of this line, and then I just need to define one more point, which will be the last point of my circle, identifying those three points there, and I'll choose the midpoint of this horizontal line, and there we have our complete circle. The next tool to demonstrate is the two point tangent circle. So very straightforward to use. This is just where we need to identify two points to which our circle will be tangential too. So to demonstrate this, I'm just going to use this V here. I'm just going to select these two lines. I'll select the first line, so the circle must be tangential to this line. I'm going to select the second line here, as we can see our circles formed. And we now have the option to move the circle. However, wherever we move it, we are constrained by the tangential constraints to the two lines that we identified previously. Here, we can identify a radius or we can just click wherever it needs to be. For example, I just let go there. And now we see that we have these tangential constraint symbols pop up, identifying that this circle is tangential to this line, the circle is tangential to this line here. And that leads me on to the last tool, so I hit C on the keyboard once again, and then we'll move on to the three tangent circle. So same principles as the two point, except here, we just identify three points. So I'm going to identify the three entities here. F one, two, and my third entity is going to be this one here. And we've got this preview coming into play, and we can see the position of the circle. So I'll select that entity there. And again, we've got these three tangential symbols pop up here, identifying the according constraints. So that's a quick overview of the five circle tools. The main ones that we use when modeling are the center diameter circle and definitely the two tangential circle, as well. We rarely use the others, but they do come into play, depending on what geometry we're working on. I hope that all makes sense. And if you have any questions, please send me a message, but aside from that, I'll see you in the next lecture and we'll do some more of the creation tools. 13. Sketching Arc Tools: In this lecture, we'll learn about the three different types of arc tools and how or when to use them. So the three tools are the three point arc, the center point arc, and the tangent arc. I've started a new design in fusion, and as you see, I've already input some sketches, and I'm going to use these to aid me in demonstrating how these tools work. So first of all, let's come up to the top. We're in sketch mode. Let's come under Create. Come under Ark. There we have the three tools available to us there. Now notice there is not a shortcut for any of the arc tools. If you want to add a shortcut, you can do so by left clicking on the three dots here and then going change keyboard shortcut. Then you can put any shortcut that you want in here and then press, Okay. The first tool we'll start with is the three point arc. If I select this, and again, we've got our sketch palette which is docked on the right, and there we have the center point, the three point and the tangent. I'm going to put that back over to the right hand side. Let's start with this three point arc then. So here we need to define three points. The first is the starting point. We'll go left click once here, and then we need to place the end point of the arc. Okay? So we've got our endpoint in place. And then when we move the mouse now, we'll then see the arc beginning to form. Typically here we would snap onto an existing geometry or perhaps an ideal location on the grid. We bring the arc in like this. We can see that the arc becomes tangential to the two lines, the horizontal and the vertical. So it essentially forms a fillt. But in this case, I'm just going to explode that slightly. I'll bring it up to this point here, and there we have our three point arc. So three points, the start, the end, and then the final sapping position. Let's now take a look at the center point arc. I'm going to come over to the palette and select the center point arc. This is very straightforward to use. So the very first click that we do is the location of the center of this arc. We're putting in the center point, which in this case, I'm going to use this sketch. I'm going to select the center of my cross there. And then the second click identifies the beginning of the arc. Let's say I want my arc to start in this position here, left click once, and then you'll see that as we move the mouse around, the radius is fixed as per the distance which we have defined here. And as we bring the arc around, we can then either snap on or put in an appropriate angle. So I'm going to snap on too, yep. There we go. And there's a three point center. Ah, let's do that one more time, then, let's select the center. Bring that out slightly for a snap out. Here. Then we can draw that around. And yeah, perhaps we can end it in roughly the same location, like so. And that's how we use the center point arc tool. And the last arc tool I want to demonstrate is the tangent arc. Now, this is really useful for when we want that tangential constraint at the start of the arc. I I demonstrate this by starting our arc here, so we're coming off of a curve, we start our arc here. And as we move the mouse, we can see that wherever we bring that endpoint of the arc, it will always be tangential at the starting point with this arc here. Let's say my ending point is here, Snap on there, got our arc in place, and we see that it's input a tangential constraint there. We've got a tangential joint between this arc and the one that we created. Now, one thing to keep in mind here with the tangent arc is that it will only be tangent with the initial geometry and not with the final geometry. So as we see here, this joint here is not tangential, let's say, with this vertical line here or the horizontal line. So just something that we need to understand when we're using the tangential arc. And I want to show you one quick tip as well, which is actually under the line tool. So let's say, for example, I draw a line, I'm just going to snap onto the grid, go 40 mil. And now I'm still on the line tool, right? But from here, I can actually draw an arc. By coming to the endpoint of this first line here and holding down the left mouse button. And with the left mouse button held down, if I draw out what should be a line, it actually becomes an arc. That's a really handy tool for when we're doing a lot of sketching and we're in need of tangential arcs coming off of existing entities. We can just quite simply hold down the left mouse button and continue to draw arcs like so. Okay, so those are the three arc tools very straightforward to use. The most commonly used one is a three point arc, but equally the center point arc and the tangential arc are quite commonly used, depending on what geometries that you're working with. It will be for sure using these tools throughout the remainder of this course. And I'll see you in the next lecture. 14. Sketching Slots: In this lecture, we'll learn about the various types of slot tools and how we can use them. So there are five variations of the slot tool. These are the center to center slot, the overall slot, the center point slot, three point arc slot, and the center point arc slot. So let's take a look at each one of these. So if we come over to fusion, I've opened up a new design. I'm already in sketch mode to come up to the create up here and come under the slot. And we'll see here that we've got the five slot tools available. Now, just like the arc tools, there are no pre installed shortcuts to these slot tools. If you do want to add them, hit the three dots and add a keyboard shortcut here. So let's start with the center to center slot. Let me demonstrate this one. So the very first click defines the center point of one of the arcs. I'm going to start that at the origin, and I'm going to come across say 50 mil in this case, and I'm going to left click again. And the second click defines the center point of the other arc. And so if I now move my mouse out, you're going then see we need to apply a with. But if I apply a WIC there, let's say, ten mil, can enter that in a keyboard, or I could click to Snap on the grid's Enter. We've then got our slot form. So the first click, as I said, that was the center point of this arc. Second click was the center point of this arc, and the third click or input dimension determines the width of the slot. So a nice and easy tool to use. And in my experience, it is the most commonly used slot tool. Let's go back onto these tools then, let's go for the overall slot. To demonstrate this, let me go below and I'll select this position here being the very first point and this position here being the second point. Now, if I open this up now, and again, I'm going to put in ten mil, press Enter, you'll see the difference here. So the very first click defines the outer quadrant of this arc, and the second point defines the outer quadrant here of this arc, then our third click defines the width. Okay? So first one, we're going center to center. Then we're going overall, and now we're going to take a look at the center point slot. The center point slot tool demonstrate this. I'm going to choose our first click here. So this is the center of the slot. I'm going to drag that out to this point here. So 25 mil from the center to the center point of one arc. And then if I expand that out, you'll see our slot form. Again, I'll input ten mil enter our first clicks the very center of the slot. Second click center point of this arc, and then third click determines the width. And essentially what's on the right hand side has mirrored onto the left. So center center point width. Then we've got the three point arc slot, create, three point arc. Very first click defines where we're going to start our arc. So let's say here. Second point defines where it's going to end. And the third point, we're going to add in this arc. Let's go for this position here. And once we've clicked our third point and we expand our mouse, we can then form a with around the arc that we've created. Again, let's go for ten mil press Enter. So this is the arc here that we drew in. We do 1.2 point and then define the radius and then moving the mouse out, we've then defined the width of this slot, or rather I input it as ten on the keyboard. And then last but not least, we have the center point arc slot. Select that center point arc slot. I'm actually going to reference it from the center point of this arc here. So if I do my first click here, I then need to define where my arc will start. So let's go for this position here, and then going to draw in my arc. Let's come up to here. And then I need to input my width, let's say, ten mil. So this is just a variation of the three point arc slot. Was a three point, we define 1.2 0.3 point, and the center point arc, we actually determine the center point of this arc and then the starting and the finishing point. I'd like to give one example of where this can be used in some geometry I've drawn just over here. We'll come to my tools again, slot. Select the center point arc slot. I'm going to define the center point of my arc, in this case, it is here, and I'm going to define my first point of the arc being this geometry here. I'm going to bring the arc around and snap on to this point here, expand my slot. I'm going to input a radius, sorry, a slot width of let's go for ten mil. Press ok. That's an example of where this tool would be commonly used. It's really snapping on to existing geometries. Okay, so fairly straightforward for the Actors. As I say, the most commonly used one is the center to center slot. But they all come into use. It all depends on what we're modeling, what we're working with. Any questions, please send them to me, but aside from that, I'll see you in the next lecture. 15. Sketching Polygons: In this lecture, we'll take a look at the three polygon tools and understand where we should be using them. So these tools are the circumscribed polygon, the inscribed polygon, and the edged polygon. So jumping into fusion, I've opened up a new design, come up to the top, create a sketch. In this case, it doesn't matter which plane. I'm going to go for the XY plane. And if we come under Create, then we've got our polygon options here, circumscribed, inscribed, and edge. Let's start off with the circumscribed polygon. I'm going to model this over here. So first of all, we need to find the center of our polygon. So that's the very first click. Then as we bring the mouse out, we can see the polygon begin to form. And there are two parameters which we control here. Number one is the distance from the center of the polygon to the midpoint of one of the edges. I'm going to put in a distance here. Let's go for 50 millimeters. I'm going to hit tap on the keyboard, and the other parameter is the number of edges. So the default is six. I'm going to go, in this case for eight. Then finally, I can adjust the mouse to change the angle. I'm quite happy with that. It's our left click once. And there we have our complete profile, eight sided polygon, 50 mil from the center to the midpoint of this edge. Let's do that one more time and take a closer look at the preview. So we can already see the preview of the polygon here and we see this circle inside. And so the polygon is on the exterior of that circle and hence it is circumscribed. In that every edge of our polygon is tangential to that circle. I'm going to now change and move on to the inscribed polygon. Take a look at this. Our left click, once again, that's starting the center point. And then as I bring the polygon out, we can now see that the circle is on the outside, and every corner or joining point of our polygon is then in contact with the circle and the edges are no longer tangential. In this case, again, we have two parameters to define. I'm going to go ahead again with 50 millimeters. Press tap on the keyboard. I'll also change that to an eight sided polygon, press enter, and then we can clearly see the difference between the two. So one is measuring a distance from the center point to the midpoint of this edge. One is measuring a distance from the center point of the polygon to one of the edges or joining points. That leads us on to the final of the polygon tools, which is the edge polygon. Roll over here. So in the edge polygon, the first click defines the starting point of one of the edges, and the second point will define the ending point of that edge. So I'm going to actually put in a distance here. Let's do it 40 millimeters, and we've also got the option to control the angle. If we hit tab on the keyboard, I'll put in an angle of 30 degrees. I'll press Enter, and then we can see a preview of the polygon appearing. And depending on which side of the line the mouse cursor is, it will determine where oligon is, whether it's this side or this side. We're going to also control here another parameter, which is the number of edges. I'm going to increase that to eight again. Let's enter on the keyboard, and there we have our parameters in place there. Now, we can modify these parameters. Let's put this down to. Let's go for 25 and I'll change that to 15 degrees. Let's change this 125. We can boost this up to 75 as an example. And the only parameter that we cannot later control once the polygon is in place is the number of sides. Once we have defined an eight sided polygon or six sided, et cetera, that is then fixed. And so if we did want to change the number of sides, we would have to select the leap and then start again. And so that is a summary of the polygons. The most commonly used one is the circumscribed polygon. But again, situationally, you might be a need to use either of the other two. And I will see you in the next lecture. 16. Fillets & Chamfers: In this lecture, we'll study the Fillet and Shamfa sketch tools in different ways that we can apply them. So we'll start with the filet tool, and then we'll move on to the three different types of Shafer tools, which are the equal distance Shamfa, the distance and angle Shamfa and the two distance Shamfa. So jumping into fusion, come under the create sketch, select any plane here. Just going to go ahead with the ex plane and over here. And to demonstrate this, I'm going to draw in a two point rectangle. Start at one point here, and I'll add in a horizontal dimension 150, press tab on the keyboard, vertical dimension 100. So let's say that we wanted to add fillets to each of these corners. We come up to the top, and actually, we're going to come under the modified tools. You'll see fillets available here. We've also got the icon here that we can choose as well. No shortcut assigned, so feel free to add a shortcut if you'd like. So let's select fillet. So from here, we need to either define a corner point. For example, I could select this corner here, we've got that red preview in place, identifying where the fillet will be. Or we can do is actually select the vertical line here and then this horizontal line to give us that fillet between the two. So I'm going to go ahead and do it the quick way, which is just a single click right in the corner there, and then I've given the parameter of the fillet, so I need to define the fillet radius. In this case, it's given me the default 20. I'm going to go ahead and add 25 mil, and then press Enter on the keyboard. And then you'll see going to hide the constraints. There we see the dimension there. Move that up here. And again, we can change that. Double left click. Let's go for 18 mill. Okay. Let's do the same principle on this corner, but using a slightly different method. Select fillet, and then we select the horizontal and then select the vertical, then we can input our dimension there. Let's go to 25. And let's say that we wanted to add multiple fillets of the same dimension. You can do that by again, choosing the Fillet tool or select this corner here. We won't input a parameter just yet. Let's say we want that to be ten mil and this one here. Okay, so now we've got both of those selected. Now we can enter the parameter. So in this case, let's go for ten mil, let's enter, and you'll see both of these are ten mil. And this fillet here is controlled by this dimension here. If I move this dimension, I'll put it there for now. If I then change that dimension to let's say 25, we'll see that both of these fillets have increased to 25 milad. I'm gonna put that back. Let's go for five mil. They go got five mill there, five mill there, 25 and 18. And so it's a very straightforward tool to use, it's very quick, very effective. It's used often in sketching, although we can also apply filllets within three dimensional mode as well. So that's after we extrude a profile. We can apply filllets after that, or if we're in sketch mode, we can apply them before. There is a slight difference between the two, and we're going to cover that when we move on to the three D modeling section. So that's it for the filllets. Now let me demonstrate to you SHAMFAs. Again, I'm going to draw in a two point rectangle, do the same dimensions. Let's go 150 by 100. And from here we come under modify, and then we've got SHAPAt three options here. Got some nice previews that appear. For example, under equal distance Shanfa, you can see there that the ShanfA in this case, is 20 by 20. It's a 20 mill vertical, 20 mill horizontal. We've got the distance and angle, and that's where we put a distance on either, in this case, the horizontal or we can do the vertical, and then the angle would be applied, and that would determine the distance on the opposite, whether it's the horizontal or vertical. And then we've got the two distant Shafer. So this is where we have essentially a non equal distant chamfer. Let's go ahead and apply some of these. Let's go for the equal distance chamfer first. And again, we can just select the corner point or we can select the two lines. Going to select the corner point for now. Let's go with a 20 mil Shafer, press enter, see if we've got 20 mil on the horizontal and 20 on the vertical. We look at these dimensions, got 20 here, and then we've got FX 20. Now, FX is a function, so it's referring to something. We hover the mouse over there, it's referring to this dimension here, which is D eight. If we double click here, it just says it's referring to D eight. So if I go ahead and change dimension D eight, and I enter there, let's go for 15. We can then see that we've changed the horizontal by 15, and then the function has read off of that dimension. Now they're both 15, and that remains as an equal distance chamfer. Come over to this corner then. Go ahead and demonstrate the distance and angle Shaf. Now, one note when we're using this tool where we want to define the distance, we need to select that line first. For example, if we want to control the distance on the horizontal here, we choose this line on the vertical, we choose this line first. But let's go ahead and let's go with the distance on the horizontal, and then we're going to chooe a second line, which is the vertical and start to see the Shaf form. So for the linear distance here, let's go for 40. Then for the angle, we can control it with this wheel or we've got the parameter box there. I'm going to input an angle for 20 degrees, press Enter, there we see our parameters. Our dimensions have appeared there. And again, we can adjust these. So change that to 30, can change that too. Let's go for 15. That is the distance and angle ShafA and last, we'll go for the two distance ShafA. So here we're going to select two lines or a corner point. Let's go for the corner point. Then first of all, we need to enter in the highlighted arrow. So in this case, the horizontal. Let's go for 50 mil there. And then let's select this arrow here and let's go for, say, 15 mil. Press Enter. Now we've got those two linear distances there. Then you can change any of these dimensions, so you can adjust them accordingly if you need to do so later. So that is a summary of the fillet and the hamper tours very straightforward to use, and we'll definitely be using these in future lectures. And so I'll see you in the next lecture. 17. Text Tools: In this lecture, we'll learn how to add text to art sketches, which can then later be used to either iboss or engrave. And I've got two examples here. So if we look at the blue text down here, this is Imboss text that we see it protrudes out from this face, ortho scusion. And then the example I've got up here is an engraving. I've engraved my text here, AtoEcusion. So let's learn how we can apply text to art sketches. So under a new design, come up to the top. I'll let create sketch. You can choose any one of the default planes. In this case, I'm going to choose the X z plane. If we come up to the top left under our creation tools, we then have the tool here text. And if we left click on that once, you'll see a toolbox pops up. And we have two options. Number one is text, which is just a text box, essentially, and the other is text on a path. And I'll demonstrate both of these to you. But this is where we have some predefined geometry, and our text will conform to the path of that geometry. So let's start with the text or the text box, as I call it. We left click once anywhere in the environment, bring out our text box. Left click again. We then see we have some sample text in place already. We've got our toolbox here where we can control a number of variables about this text. I'm going to change this to Autodesk fusion. And then moving down, we've got various fonts that we can work with. I change this. Let's go for aerial, whether it's bold, italic, then we've got the option to change. Well, it says height, but this is essentially the size. So if we change this to, let's say, 15, you see much larger, go to leave that it's eight for the time being. And in terms of character spacing, this determines the spacing between each one of the letters. If I increase that to go for 20, okay? We can then see we've got some quite large spacing between those letters. Leave that as zero default for now. We've also got the option to flip as well. Where required, we can flip on the vertical, like so, or on the horizontal, like so. And then relating to the textbox itself, we have various options for alignment. So we can align that to the left if we want that to be on the top here, you can adjust these how you need. It's very straightforward. We've also got the option here as well to change the angle. Hold down the left mouse button. We can adjust that or you can manually input an angle that you need. Go ahead with zero. So let's look at text now on a path. But to demonstrate this, I'm going to draw in a centerpoint arc. I'll start the center point of my arc here. Let's go and start the arc here, bring that around, like so. Let's come up to the create tools. Select text. Then in here, we just want to make sure that we've got text on path selected. And then, first of all, we need to define the path which the text needs to be on. I'm going to select my arc in this case, and then our range of options pops up again. I type in Autodesk inventor. Okay. And we can make any of the same adjustments that we covered with the text in a box. But here we need to flip the text. I'm going to flip on the vertical. That's correct. We've also got the option as well to input the text on the other side of our geometry as well. So to do this, we come under placement, and then we could put, in this case, above the path. And so we've got the text below the arc or we can have it above. We've also got the option here as well to fit to path. So fusion here will take into account the length of this arc, and it will adjust the text spacing so it fits from one point to the other. And this can be quite useful when we have a defined area in which we want our text to cover. So if I hit the checkbox here, we'll then see it spaced out accordingly to cover the entire of that path. And again, at the bottom, we've got the options for aligning. So we're going align it to the left of the path, either center or to the right. And so that's it for the text. It's very straightforward, and we'll be using this more in the three D modeling section where we will begin to engrave and emboss three D part or see you in the next lecture. 18. Sketch Modification Tools: So far in this course, we've covered the fillet and the various hamper tools. Now, they all come under the modification tools. And in this lecture, I want to study the remainder of the modification tools. These are offset, trim, extend, break, and scale and move. So let's start off with the offset tool. Now I've drawn in some existing sketches to help me demonstrate this. We'll come up to the top, come under modify, and let's go straight to offset, which is O on the keyboard. Let's press offset. Our toolbox pops up, and here Fusion is asking us to identify what curves that we want to offset. We've got the option as well for chain selection, which I'll show on the square afterwards, and then we've got two sides flip and match topology. So let's first of all, select a curve. In this case, I'm going to choose the circle here. From here, we can either use the arrows or we can input a distance to offset. But if I left click, if I hold down the left mouse button and drag, we can then choose to offset that how we like, or we can input an exact distance. But let's say, in this case, we're going to go for 25 we also have the option to do a two sided offset. So that's offsetting exterior and interior. So if I select this, well then see if we're offsetting the circle, 25 mil exterior and 25 mil interior. If I click Okay, we can then see we have those two dimensions in place there. So this is our original circle. The outer offset is by 25 mil, so we can change that by double clicking Gentha 30, and the inner one, we can change that to, let's say, minus ten. Okay? And there we have our two created offset circles. I'll show one more example of that using the flip tool, if I press O on the keyboard, select my curve, and I input an offset of, let's say, 25, unchecked two sides. And now we're offsetting exterior. But if we flip that, it will then flip to interior, and essentially, it'll just put a minus in between the value. But if we change that to a positive, it will then go on the exterior. We'll click Okay with it, and then we'll move over to the square. I'm going to press O on the keyboard, bring up the offset tool, and here, I need to select my curves. Now, in terms of selection, we can either have chain selection turned on or off. Let's turn chain selection off and select this top horizontal line here. I can now offset that line, the exterior of the square or interior. But if I click Chain selection, it will chain select all of the curves or entities which are in contact with the one that we selected, which is a nice shortcut. I'm going to enter an offset value there of let's say ten mil. Let's do two sided, as well and press Okay. And there we have art to offset squares by ten mil from our original. Let's move on now to the trim tool. We'll come up to modify. We've got our trim tool here. That's the shortcut T on the keyboard, of a press and in trim mode. And the trim tool is very straightforward. It will essentially trim an entity where it intersects with another. So, for example, we can see a preview here. This purple line will be trimmed away fusion will recognize where that line intersects with the circle and then trim accordingly. If I place the mouse cursor over this line here, it will trim from this intersection of the circle to this intersection of the circle. So let me click this line here. We can see that's been trimmed. This one here, choose this side, and this one down here, choose this side, and we can even do the same to the circle as well. So if I hover the mouse over this part of the circle, it will recognize this intersection point with this line and this intersection point with this line. If I select that arc there, we can then remove that likewise, on the other side, even do the same up here and so forth. It's a really handy tool when we're sketching. Next up, let's take a look at the extent tool. Again, a very simple tool to use. Come under the modification tools, and there we have extend. And this will just extend a curve until it intersects with another one. So, for example, as I hover my mouse over this line here, we'll see this red preview appear, and it will extend this line all up until the intersection to this circle. If I left click there, that line is then extended like so. Likewise, on this vertical line here, just hover the mouse over, and it will extend that line all the way up until contact with this one, like so. So again, very straightforward and a very practical tool for when we're doing sketching. Now let's move on to the next tool, which is break. So one of the modification tools, we come down to break, select that. And break just simply breaks an entity where it is in contact and conflicts with another. For example, I have a circle here and I've got a line running through it. If I hover the mouse over the circle, like so we can see these two red crosses appear down here. What this will do is this will break up this circle at those two points. By left click on that circle and leave the brake tool, press a scape on the keyboard, and then I go to select the circle. I can no longer select the entirety of the circle. I can only select this arc. And likewise, if I then select this side of the circle, I can only select this arc, but it's broken up circle into two arcs there. But notice that the line remains intact. If we want to change that, we can come under break, and then we can just click on the line like so, press exit on the keyboard, and then when we move the mouse over this line, you'll see it's then broken up from this one and this one is now independent, and so is this one here. That's the principle behind the break tool. And now we'll move on to the scale tool. So let's come under the modification tools, then we'll come down to sketch scale. This is very straightforward to use. We have a toolbox pop up in which point we need to select the entities we want to scale and then the point of the scale. So in terms of entities, we can either select individual ones or hold down the left mouse button and just drag across. In this case, I'm going to select the polygon and the circle. And then the point at which we're going to scale from. In this case, I'm going to choose the very center of the circle there and the scale, we can then define the factor here. So let's say, for example, let's scale that by two, and then press Enter. We've now scaled our components by a scale factor of two. And then the last of the modification tools is scale MV. That has a shortcut of M on the keyboard. So let's select that, and then our toolbox pops up. And the first thing we have to do is to select what it is that we either want to move or copy. So for this example, I'm going to select the polygon and the circle, then we can see here that we have a pivot in place. And if we move that pivot, let's say, over here, our entire selection will move with that. We can also choose to rotate as well. Another option is the square here. We hold down the left mouse button. We've got free movement over everything that's selected. And in terms of the rotation, if you do want to adjust the position of the pivot, so that was an automatic position, we can come across to our toolbar and under set pivot, we select this, and then we define the new place of the pivot. So in this case, I'm going to select the center of the circle. And then when we're done with that, we can click Done, and now we can then move from that pivot or rotate from that pivot point. If you want to fine tune movement of anything you've selected, you can use the distances here. For example, if I enter 25 on the X, 25 on the Y, and the z would just move it forward and backwards. So we'll leave that at zero and compress Okay. Press Control Z to stop that, press M to go back into the move tool, re select everything. And then we've got the various options to rotate this sketch around all three of the axes, X Y and Z. At the very bottom, we've got the option to create a copy. If we select that, and then I go to move this sketch over here and then let go. That's okay. We can now see that we've copied that sketch and positioned it over here. Press M on the keyboard back into the move and copy tool, and now I want to demonstrate the point to point move type. So we need to just select two points here. One is the original of the entities that we select, and then one is the target point to which that will move too. So if I now select all these entities here, polygon and Circle, but the original point, I'm going to click here as an example, and a target point, I move over here. I'm going to select this to be my target point, and we'll see that all of my selection has moved over according to our two points, the origin and the target. Press okay? Okay, a press control Z I want to show you a shortcut to moving any sketches. So if I drag select across the polygon and the circle, I hold down the left mouse button, I then have the free movement of those that I've selected, and it doesn't just have to be the center point of the circle, can also be any point like so. Okay, so that is the fundamentals of the modification tools. And definitely in future lectures, when we start three D modeling and I start doing a number of examples and you have assignments, you will find these tools of great use. And so I'll see you in the next lecture. 19. Sketch Pattern Tools: In this lecture, we will study the various pattern tools, including the rectangular patterns, single jewel and symmetric, the circular pattern, and the mirror tool. So in fusion, I've done some sketches to help me demonstrate these. Now, first of all, we're going to start with a rectangular pattern on a single axis. So right here, I've got a rectangle with a circle, and let's say, for example, we want to pattern this circle alongside this axis here. So let's come under our creation tools. Let's come under rectangular pattern. Our toolbox pops up. We need to identify the object to pattern, in this case, and choose the circle. Then we have a lot more tools available. So first of all, we need to define a direction or directions. So for now, we'll focus on single axis, so I'm just going to select one axis. Now here we can choose any pre existing geometry. For example, I could select this line here if I wanted to pattern in this direction or the vertical line here in the vertical direction, and I can choose construction lines as well. So in this case, I'm going to select this line here. And then I've got the option to change between the distribution type. So I've got extent and spacing. I'm going to stick with extent for now, and I'll show you spacing a bit later. Moving down to the boxes, we have quantity here, so I'm going to select I want to have a total of four of these circles. And in terms of their distance, now this relates to distribution. So the extent of my pattern, in this case, I've calculated it to be 250 mil. And as we can see now, we have the original circle, the second circle, third and the fourth. So four circles total, and the extent distance is 250 mil. That is the distance from the center point of this circle up to the center point of this circle here. The next up, we've got the direction. So I'm just patterning in one direction here, but we can also pattern symmetrically, which would lead to more circles appearing on this side, which we don't want, and I will demonstrate an example of where symmetric panning is useful later. And then you'll see we've got another quantity distance and direction. So these three here only relate to a second axis. So we've only selected one direction. So essentially, we don't need those three for this particular example. I'm quite happy with my four circles at 250 mil extent. And then if I press Okay, we can then see those circles now form. And we can edit these anytime by double left clicking on this symbol here, which is the rectangular pattern symbol. So if I double left click, you can see our toolbox pops up again and we can make any according changes from there. Now one useful tool within this is suppression. So if I tick this box, we can then see that we have these check boxes appear in the patterned circles. And then if I select this one here, for example, and let's go for this one, as well, and presso, we can then see that those instances of our pattern are now suppressed. I press Control Z on the keyboard, bring them back. Double Left click on this symbol, and then we've got our toolbox available again. Another way to do this as well, so I'm going to hit Control Z to come up to create rectangular pattern, select my object. Now, in terms of direction, so we've talked about selecting individual entities. But in this case, what we can also do is use the arrows. This is a really useful, handy quick tool that we can use. So in this case, I'm patterning a quantity of three, but if I go for four, and then we can adjust the arrow accordingly as to where we want them. So if I click Okay there, looking good. Let's move on now to the rectangular pattern Jual acts. I'm going to use this sketch to help me show this. Let's come up to our creation tools again, go on a rectangular pattern. Again, we're going to select our object, in this case, this circle, and under direction or directions, select, and now we're going to select two directions. Let's go for this horizontal line and this vertical line. So we're going to pattern in this direction and also vertically as well. And for this, I'm going to drag my toolbox down so you can use the scroll bar on the side if you need. Keep the distribution as extent and go for a quantity of four. Then distance, let's go for the same 250. So we're patterning like we did for the single axis. And then under the quantity distance and direction, this is for the vertical. So let's go for a quantity of three, and I've already pre calculated this as a distance of 100 and that's an extent reference distance. Then we can see we've panned in both axis. And if we click Okay, that's looking good. Then again, double click. In this case, yeah, we want to suppress anyone. Let's say we want to suppress these two. Let's go for three, press Okay. And then we've removed those instances, and we can put them back. So again, go in the suppression. We can just left click to bring them back. That's okay, like so. And that is the rectangular pattern for dual axis. Let's now move on to symmetric patterning. I'm going to use this sketch up here to help me. Let's say that we want this circle pattern in both directions horizontally and vertically. Let's come under create. Let's choose our rectangular pattern tool and object, select the circle. And under direction, let's click on this horizontal line and this vertical line, keep the distribution as extent. And then under quantity, let's stick with three, and I do a distance here. So this is pre calculated 100, and then I'm going to change the direction of this. Right now, the distance between this center point and this centerpoint is 100 mil, and I've got my three circles there. But if I change the direction to symmetric, you can then see I've got my three circles, and they are both patterned by 100 mil. So center point to center point, 100 mil, and center point to this center 0.100 mil. I'm going to repeat that for the other direction as well, which is the vertical, keep the quantity three, and then I'm going to put a distance here of 50 mil. And again, I'm going to change that direction to symmetric. So patterning symmetrically both above and below. Okay. And that's a case where the symmetric pattern can be very useful. So now we've covered the rectangular pan tool. Let's now move on to the circular pan tool. But to demonstrate this, I'm going to use this sketch down here. Let's say, in this case, we wanted this circle to be patterned around this axis here. Come under the create tools, select circular pattern, very simply, just like the rectangular tool, we select our object. So I'm going to drag around this circle here. And then in terms of the center point, I'm going to select the center point of this circle here like this one. And put a quantity there. Let's go for eight. And then we've got different options for distribution. So full distribution is essentially patting around 360 degrees. We could change that to partial distribution. So in this case, we're patterning over 180 degrees. We could change that to say two, two, five and so forth. We've then got the option to symmetric pattern. So if I got a symmetric, and I'll type in, let's say, 180, and I'll go for a quantity of five. We can then see that this is our original circle, and we're patterning symmetrically. So I've got an additional two circles on this side, so counterclockwise, and then clockwise, two circles on this side over 180 degrees. And again, we can change that we go to 270, like so or if I change that to 90, they can all be so bunched up together like that if I put that back on full, let's go for a quantity of eight. And again, just to show you the same suppression ability is available by clicking here, and then we can just left click on any instances that we don't want to have. Click Okay. And again, if we want to edit any of this, we can double Left click on the circular pattern tool and then make any changes from there. So I go in my suppression. Take these back and press Okay. And that is the circular pattern tool, so a very simple tool to use. And the last tool I want to show you is the mirror tool. So that's the tool just up here. And we can also find that under the creation tools just above circular pattern here. But to demonstrate this, I'm going to be using this sketch here. Let's say, in this case, that we had these two circles here, and we wanted to mirror them over to this side. You see, I've got this construction line that's in the center, and that's snapped onto the midpoint of this horizontal line and the midpoint of this horizontal line. Let's go ahead and use the mirror tool with our tool mox. We need to select our objects. In this case, I choose one and two. And then under mirror line, click Select. And in this case, I'm going to choose the mirror line here, my pre drawn construction line, and we see the two previews appear on the other side, and if I click Okay, we've then mirrored across those circles. It's a really straightforward tool to use a really good for efficient sketching. That is a summary of the pattern tools. So we've done the rectangular patterns, looking at single axis, dual axis, and also symmetric. We've covered the circular pattern tool, and we've also covered the mirror tool as well. These tools are really handy when it comes to sketching and can be used fairly regularly depending on what we're working with. And we'll be for sure using these throughout the remainder of this course. I'll see you in the next lecture. 20. Dimensions & Constraints: In this lecture, we will study the dimension and the constraint tools. So constraints are essentially applied rules to geometries that cannot be broken. They restrict how these geometries can move or change relative to each other. Overall, they help us to ensure that our sketch maintains certain relationships when being modified, which allows us to design with precision while maintaining fully constrained sketches. So in this lecture, I will demonstrate applications for both linear and angular tolerances and then each of the common constraints. We will be using these on many occasions when sketching in this course, and particularly during the examples that I give, the assignments for you, and also the projects that we work on together. So let's jump into fusion and start off with the linear and angular dimensions. So the shortcut for this is D on the keyboard. And then if we come up here, we've got sketched dimension, or if we hit Create, we've got sketched dimension just down here. I typically use the shortcut, D on the keyboard. Now let's take a look at this line here. So this line is sitting at an angle from this one, which isn't yet defined. Therefore, it's free to roam in terms of angle, and if we see there, it's free to change its length. If we want to constrain this, we can use the dimension tool. So I'm going to select this line to dimension, and then I've got two options from here. Number one, I can state its linear length like so, or I can define a length from the endpoint of the line just here to the origin. And so how I change between the two is just by dragging the mouse up. So if I drag the mouse closer to the line, it will recognize that I want to input a flat linear dimension, whereas if I drag the mouse up, it's then referencing from the endpoint to the origin. So let's say, for example, I want to input a dimension of 100 mil, just a linear length of that line. Let's enter Okay. I've come out the dimension tool. Now we've applied a dimension to it, but as we can see the line is still blue, and that's because we haven't defined an angle or given this a constraint yet. So in this case, I'm going to apply an angle. So an angular dimension very simply, we click one line, click another, and then we see the angular dimension forms. I'm going to drop that there and give that an angle of 30 degrees. Press Enter on the keyboard. As we can see now, all of the geometries here are black in color, so they are fully constrained, so nothing can move. I cannot change the angle of this line or change the length of this line without coming into the dimension itself. So if I double click, hit 45, or if I double click here, hit 50, that's the only way we can change it. I hate control Z on the keyboard to revert back. Another example I'll give is dimensioning between two points. For example, we have the center point of this circle, going to left click here once and the center point of this circle. We just here, left click again, and then we can just define that dimension there. So let's say 100. Now that's fully constrained. And again, once that dimension is in place, quite simply double click and we can alter it as we need. So that's the dimension to very straightforward and very commonly used. Let's move on now to constraints. So the first constraint we're going to be working with is the vertical and horizontal constraints. So to help me demonstrate this, I have two lines here. You can see neither of them are either vertical or horizontal, we can make some changes here. So if we come up to the top where our constraints are, we can see the shortcut for this is just here, horizontal vertical, or we can select the drop down, and it's available for us here. So we'll left click that once. Now we are in the vertical horizontal constraint. We can then left click, for example, on this line here, and it will apply that constraint to this line. And we'll see the symbol form here. Now, this is the vertical constraint symbol, which indicates that this line is constrained vertically like we've just done. And I'm going to do the same for this line, like so. And I'm going to exit that tool by right clicking and then selecting Okay. And we can see now that both of these lines have that constraint in place there. Now, if we have a line, for example, let's say, at this angle, and we use the vertical horizontal constraint, in this instance, this line here will become horizontal. So if I left click, we then see the horizontal constraint, and the reason for that depends on the angle. If the line is closer to a vertical position, it will be assigned the vertical constraint, whereas if it's closer to the horizontal position, it will be assigned the horizontal constraint. Just move this out the way, and then I'll show you another example of where the horizontal constraint can be useful. If I select the vertical horizontal constraint here and I select this endpoint here, and then this one, we'll notice that this endpoint is now horizontal with this one here. And if we hover our mouse, let me just bring these closer. If we hover our mouse over this constraint, we'll see that this one is also highlighted and vice versa, and that indicates that that relationship is in there between these two points here. They are constrained horizontally. So this line here is now fully constrained, and the only movement we have in this line here is from side to side. We cannot change its angle because of this constraint, and we cannot move it up and down because of this constraint here. So the only thing left to do here is to press D on the keyboard and give a dimension between these two, let's say 40. Now this line and its endpoints are in black color, and this sketch here is fully constrained. Let's move on now to the coincident constraint. So a coincident constraint is when two points are made coincident with each other. For example, let's have a look at this circle here and this line here. Let's come up and select the coincident constraint, which is just here or on the drop down, the second one and here as an example, I'm going to select the center point of this circle, and then I'm going to choose the midpoint of this line. Now I could choose the endpoints as well. But for now, I just go with the midpoint, and we can see here this symbol is the coincident constraint symbol, identifying that the two points here are coincident. So we can remove any constraint that we have applied. For example, if I right click on this one and I select delete and I try and move my circle, we can see that that constraint is no longer in place and to put it back centerpoint to midpoint. Another example I give is these two lines here. So when I've drawn these two lines, notice here that they are automatically inserted with, in this case, a horizontal constraint, and in this case, a vertical constraint. So if I just select the line to and I begin to draw a line vertically, we can see in blue there, just below the mouse, that fusion will automatically apply that vertical constraint. And likewise, if I apply horizontal constraint, we can see the symbol appear there. And that's really helpful when it comes to quick sketching. So let's select the coincident constraint once again. And in this case, I'm going to select this point and this point here. And we'll see that they are now joined, and if we zoom in, hover the mouse over the corner, we can see that constraint there. Let's now take a look at the tangent constraint. In the center here, I have a circle and then three lines surrounding it. Let's say that we wanted this line to be tangential to the circle, like so. First of all, I'm going to apply a coincident constraint between the endpoint of this line, and then I'm going to select the circle here. And then for tangency, just going to select tangent here or in the dropdown, it's the third one down and select the entire line and the circle. We'll now see that tangent constraint has put in place, and we've got our line there. Press control z. I'll show you a Nullar example with this line here. So again, tangent constraint, select this line, select this circle. And now those two have this tangential relationship. So with this line, it can still move up and down, and it will always maintain that relationship with the circle. I'll give one more demonstration with this line here, so tangent, this line to this circle. And again, lines can be at any angle. But for example, this angle is not lined, so if I move it around, you will see that it will always follow that tangency. Then if I go ahead and apply a horizontal constraint to this line here, we can move it side to side like so, and then if I apply a coincident constraint between this point here and the circle, it's now fixed in place. And likewise, I do the same for the vertical line. Let's go for this point and the circle. Let's do the 30 mill length line as well, endpoint to line, tangency, line, circle. Now we have those three tangent constraints in place. It's a very simple tool to use. We use this very regularly when we're working with arcs or circles. Next, let's take a look at the equal constraint. So I'm going to demonstrate this on this line here and this one here. An equal constraint ensures that two geometries are exactly the same, either in length or it could be a radius or a diameter. So the equal constraint is just up here or on the constraints, fourth one down. I'm going to select this line here, which is dimensioned at 30 mill and then select this one here. And now that relationships in place. If I measure this line, we can see that it's 30 in length following this one. And now that that relationship is in place, if I change this dimension, let's say, change to 50, you'll see that this dimension will change also. Here we have 50 mil and 50 mil. And likewise, if I do the same for, let's say, this line and this line, although there's not a dimension in place, they will still have this equal constraint here. And if I go ahead and then apply a dimension here, let's go for 40 mil. I'll see they are both 40 mil in height. I'll demonstrate the same using some circles. So if I draw a circle out, let's say 40 mil, I draw another circle out, but don't place the dimension. Choose the equal constraint and select them in any order. So I select these two here. This one will jump up to the same diameter, and then we can change that. I'll say 75. And now we have 275 diameter circles. Next up, we have the parallel constraint. So put simply, this constraint ensure that two lines are parallel to one another. It's located just up here, and then the constraints, it's the fifth one down. So I'll select that tool. And to demonstrate this, I want to choose this line here, and I want that to have a parallel constraint with this line here. I I left click there, we can then see that we've got that parallel constraint in place there. Where I move this line, it will stay parallel with this one. And if I change this one's angle, we can see this angle will change also as they are kept with that parallel relationship. I'll demonstrate that again up here. So up here, we have a rectangle and a straight line. Going to use the parallel tool, select the line. And I'm going to use, for example, this edge here, then we can see that both of those are parallel to one another, and I cannot change the angle. So if I grab the endpoint of the line, not possible to change the angle. Next is the perpendicular constraint. So if I select the perpendicular constraint just up here, it's a sixth one down perpendicular, and I want to have a perpendicular constraint between this line and this line here, so that essentially forms a 90 degree angle between these two. If I left click this line and then left click this line, we'll see the constraint similar pier here, and we've got that 90 degree relationship. And likewise, I could repeat that for these two lines here and form the same relationship, one, two, and then we see the similar peer here as well. Another example is if we press L on the keyboard, so we're in a line tool, and then we snap on to this line here. So I'll left click once. If I draw a line vertically upwards, like so, and then left click again, come out of that line tool, we can see at the bottom here that fusion has automatically input the perpendicular constraint. It's recognized that this is coming off perpendicularly from this line. So again, it's quite useful for efficient sketching. Next, we have the fix unfix Constraint. So right now, within this sketch that I've drawn here, it is almost fully defined. There is only one piece of movement that this can do, so I hold on to a corner point. I can move this sketch around, but aside from that, I cannot alter any dimension of either the straight lines or the arc. Everything here is either fixed by the dimensions or by the constraints. So if I want to prevent this movement, we use the fix constraint. If I select this, I can then apply that at any point on this sketch, and it will then be fully constrained. So every line now is currently blue due to that freedom of movement. But if I apply a fixed constraint, let's say this corner point here, we'll see that every line now turns black and that this is fully constrained. So I cannot move this if I try and hold down the left mouse button. Everything there is fully constrained as a result of applying that fixed constraint. If we want to remove that fixed constraint, we need to right click on it and then come down here and select unfix. And then doing so, the sketch is blew again, and I have freedom to move it, where I could apply it in different location let's say there. So that's a really handy tool, and especially when perhaps we're not referencing sketches from the origin. Next is the midpoint constraint. So this is located by the triangle up here that identifies the midpoint. So with this constraint, if I then select, let's say this endpoint here. So this blue line, I want this endpoint to be constrained with the midpoint of this line, which is roughly around here. So now I've selected that endpoint. If I just click anywhere on this straight line, fusion will pick up where the midpoint is and it will form a constraint between the two. And we can see that relationship triangle just in place there. Another example I give is if we want the midpoint of this line here to be constrained to the midpoint of this line here, we can just select the two lines. So for example, our left click once here and then once again here, and we'll see that both those midpoints are now constrained together as represented by the triangle there. Another example I'll give is, let's say we have an example of a circle and a line. If we want the center point of this circle to be in contact with the midpoint of this line, it's going to select the center. It's going to click anywhere on this line, let's say here, and then we've got that constraint put in place, we've got our triangle appearing there. Next, we have the concentric constraint. So this is very straightforward. This is represented by the two circles here and it's also just down here below midpoint. So if I select this, and we want to have these two circles to be concentric with one another, I E, their center point axis is concentric. We can just quite simply left click on both of those circles. And as you'll see there, we've got the concentric constraint symbol showing up, and both of these circles have the same center point. That can also be applicable on an arc as well. So in this case, an arc on a circle, if I select the circle and then select the arc. So this here is the midpoint of the arc. So essentially, what will happen is the center point of the circle will be on the center point of the arc or left click on the arc, and then we can see that relationship put in place. And if I try and move these around, we can see they move together because they have the same center points exactly the same for the circles as well. Next is the colinear constraint. So let's say, for example, here, I want this line here to be colinear with this one, so it will be something like that. We could raise this one up, something like that. We can come up to the top when we've got colinear, can select that. And quite simply, we'll just select the two lines to have that relationship. We'll see the colinear constraint symbol just there. And then if I adjust, let's say, the height of this line here, so press D on the keyboard, add a dimension in, let's go for 50 mil. You will see that the relationship is maintained between the two. And likewise, if I adjust that to let's say 80, these two lines will always remain colinear with one another. Another example, I hit L on the keyboard, and I start at the midpoint of this line here. So left click once, I just bring that across, then I'll press L on the keyboard again, I draw in another line here. If I want these two to be collinear, I'll select the constraint. Now, this line here is perpendicular to this line as indicated by this constraint here. And it's also this endpoint of the line is snapped on to the midpoint of this line. Therefore, only this line can move to be colinear with this one. So if I select these two, we'll see this one jump down again to the midpoint of this position, and we're maintaining that colinear relationship between the two. And last but not least is the symmetry constraint. So quite simply, this just ensures that two entities are symmetric about a symmetry line. So in this case, this vertical line is going to act as the symmetry line, and we're going to add a symmetry constraint between these 2100 mill length lines. So that's located just up here. Click on symmetry. First of all, we need to define the very first sketch entity. So we'll select this one. And the second one, we'll select this one, and then our third click defines the symmetry line. In this case, I'll select the vertical line. What we'll see as the angle between the two is then the same by right click Okay. Now, if I adjust one of these lines, like the angle, like so, we'll see that based on its symmetry constraint about this line, that this angle will move as well. So let me D on the keyboard and dimension these two. Let's go for 45. We'll see both these angles are now 45, and if I adjust that, let's go for 15. Both of these are now 15, and these lines maintain this symmetry constraint just here. So that is a overview of the dimension and the constraints tools. Now, the constraint tools I gone through the most common ones, and we will be using these throughout the remainder of this course, especially when we move on to the projects, the examples, and the assignments, and you'll become more and more familiar with them. It does take some time, and in my experience, the more that you sketch, the more you become accustomed to constraints and how useful they are in forming precision engineered sketches. So I look forward to seeing you in the next lecture. 21. Construction Lines & Measurements: So far in this course, we've covered all of the fundamental sketch tools. So in this lecture, I will highlight some additional sketching techniques to support us in two D sketching. We will take a look at how to sketch construction lines and how they differ from generic lines. I'll introduce you to the measurement tool, show you how to switch between dimension diameters and radii, and we'll also take a look at the sketch palette. So construction lines, you might have seen this in previous lectures. These are construction lines here. They are dash lines, and they can be used as temporary reference lines to help position and align other entities within a sketch. So essentially, they act as guidelines that can be deleted once the primary design elements are placed. So I'll give an example of how these can be used. Let's come out of the create tool and a slot. I do a center to center slot. I just throw this in anywhere, give it any dimensions. And then I'm going to use my mirror tool, select these geometries, and the mirror line, I can select, let's say this line here. And so this is a good example of where construction lines are used. It's used as a reference line, in this case, to help us project a geometry by using the mirror pattern that's directly in the center of the two horizontal lines. So how do we input construction lines? Let's hit L on the keyboard? To put in construction lines, we need to ensure that the line type, so under the sketch palette, that this construction icon here is then highlighted, like so. And then any geometries that I draw will be construction lines like So also the same likewise goes if I use other tools. So if I use the circle creation tool, or if I use the rectangle tool. So it's important when we're finished with our construction lines to make sure that this is unchecked, like so. So how does that differ from generic lines? I'll show you the key difference here. So when I hover my mouse over this rectangle here, it's actually split into four rectangles. So these are four individual profiles. Whereas when we're using construction lines, the rectangle itself just acts as one profile. And this can be really handy when we later come to three D modeling. If we're using the extrusion tool, revolve tool, sweep tool, loft tool, et cetera, we are required to define profiles in which to three D model. And in this case, we would have four individual ones, whereas in this case, if we take out the slots, we just have one profile available. If you do it by accident, draw any construction lines and you wanted to make that a generic line. You can left click on it, and then under the sketch palette, we can just uncheck the construction there, move that back, and there we have a generic line. And as you see now, we have these two profiles available. Another really useful tool we can use when sketching is the inspection tool. And that's located just under the toolbar here, so we can just click there or under the drop down, it's the very first one. It's a shortcut I on the keyboard. If I hit I on the keyboard, they're going to take some measurements. So the toolbox pops up. We've got options here to select faces, edges, vertices. We've got bodies, which we'll be covering in the three D modeling section and also components. Under precision, I just leave that as the default, if you want to measure in secondary units as well, you can do so. Let's take a look at that in a bit. For now, I'm going to select this horizontal line, which is identified as selection one and then this vertical line, identified as selection two. Immediately, fusion will show us the angle between those two lines. If we look at our toolbox, we'll see that selection one, so the horizontal line has a length of 200 mil, and selection two, the vertical line is the length of 125. So let's take a look at secondary units then. Let's say we wanted to measure in imperial units, so inches. We now have a look at the length. It's shown in metric, and then in brackets afterwards, shown in inches. So 7.874 " is 200 mil. Let's give another example of that. I'm going to hit on the keyboard again. We're going to take a measurement this time from the center point of this circle to the corner point of this rectangle here. Now, if we look at our toolbox, we can see quite a bit more data there. So we've got this results section. So the true distance between the two is 71.589 millimeters. We've got that in inches as well. And then if we want to see the distances on the X, Y, and Z axis, we can select one of these. So, for example, if I select this one, we can see that on the Y, we've got 15 mil on the X is 70. And we can switch between the measurements being aligned to Section one or two. So, for example, I've got them as one here or as two there. Those figures that we see on the screen are then input here, so X, Y, and Z. Then we've got some more data down here. So selection one, which is the center point of this circle, its position relative to the origin is 300 mil on the Y zero and then on the Z 95. So we can see the two axis up here. We've got the X and then the Z there. And the same for selection two, X Y and Z. So referencing, again, from the origin zero, zero, zero on the XY and Z axis. So that's a very handy tool for quick measurements. We don't have to input dimensions. We can just do a quick check there on either distances or angles. And the last tool or rather technique that I want to show you in this lecture is how to switch between diameter and radius when we're dimensioning off circles. I'm going to hit C on the keyboard, I draw in a circle there. Let's go for 100 mil. So we've got our 100 mil diameter circle here. Now, this is currently displaying as a diameter, but we can change it to a radius. You simply right click on it and select toggle radius, and then you'll see it will become radius measuring 50 mil. A nice quick tip to finish this lecture, and I hope those tips are useful, and you'll be seeing me use these throughout the course. I look forward to seeing you in the next lecture. 22. Sketch Assignment 1: So far in this course, we've covered all of the fundamental creation modification and constraint tools. And so this lecture is your first sketching assignment. The assignment brief is to sketch this part using the tools learnt in this section. Now, there isn't necessarily a single correct methodology to draw this part. The most important thing is that the end result is consisting of all the dimension geometries and that they are all fully constrained. But I recommend pausing the lecture here and attempting this assignment. For the remainder of this lecture, I will complete this sketch using the tools that have been demonstrated so far. But please pause the video here and attempt this sketch, and I will see you shortly. Okay, welcome back, and hope you got along well with the sketch. And now I will model this part myself and talk you through the tools I will be using. So I will be going through this quite quickly, but I will be explaining each use of the tools as I go through them. I've opened up a new design, count to the top left. It creates sketch. The options are the three default planes. You can choose any one of these for this two D sketch. So let's go with the XY plane, then on the sketch grid. I'm going to start with the outer body. So for this, I use the two point rectangle, start at the origin, draw that out. We can see on the horizontal there, we have a dimension of 80 millimeters. It tab on the keyboard. We put a vertical dimension of 40 millimeters, enter on the keyboard. They want to add in my two center lines. So these are identifying at the center according to the midpoint of the verticals, and also the centers, according to the midpoint of the horizontals. I hit the line tool, then going to hit construction. I'm going to find the midpoint of this line as identified here. Left click once, drag that down and left click again onto the midpoint of this horizontal line. Same for the verticals, midpoint, come to midpoint, left click, looking good. Then off my construction lines. G to hit C on the keyboard and start drawing the circle from this center line here with a diameter of 15 mil. I'm going to press O on the keyboard for offset. Offset that circle. I use the parameter box over 2.5. It's okay. G to hit D on the keyboard, dimension from the center point to the vertical line. And that dimension as per the drawing is 20 mil press enter. And now we can see those circles are black in color and they are fully constrained. Now let's go ahead and add in this slot, one of the create tools and the slot. As for the dimensions provided, we have a dimension of 15 mil from the center point of both the arcs. So it's logical, in this case, to use the center to center slot. I'll select that. Make sure my slots on this center line here, draw that across, expand that out. I've got a slot w there of six mill plus enter. I want to use my dimension tool and dimension the center point of this arc to this vertical line. Add that dimension in 15 mil, enter. Then I'm just going to add one more dimension from the two center points. Is the 15 mil plus enter. Okay, everything's in black color looking good, turn off the constraints for now. Want to add in this arc down here over this creation tools arc. I'm going to use the in this case, I'll go for the center point arc. I know my center point is defined here. I know the first point is defined on this vertical line at a distance of the radius, which is 12.5 mil. Okay. Then click once, make sure it's snapping onto a vertical line, draw the arc around and then snap onto the horizontal line here, our arc in place. We can put this square geometry with a Shafer in here. But for this, I use the two point rectangle tool, start from this corner, drag across, and then put the dimensions, 12 mill on the horizontal, press tab on the keyboard, and got ten mill on the vertical, Enter. Now Shanfer on this corner here. Come under the modification tools. It's Shafer. We know the Shafer is four by four, so it's an equal distance Shafer. I'll select that tool. I select my corner point here into four on the keyboard, press Enter looking good. Now we're going to put in the arc up here so we know the center point of this arc is the intersection between the horizontal and the vertical center line. We coming of the creation tools and the arc on center point arc. Started here. Drag that across, make sure we're snapping to that horizontal line. We've got the rad of 12 mil. So we're going to left click once on that snap, draw that around and then left click again when we're in contact with this horizontal line. Now we just need to add the text on top. Under the creation tools, let's go on text. In this case, we don't want the text box, but rather the text on path. Now we need to identify the path. In this case, it's the arc. In terms of the text, we've got fusion 2025, might bump that size up a bit, and let's go for 2.5. Then we want to make sure the alignment is in the center, not that it's offset like so, and that's the correct orientation, horizontal, not vertical flip, looking good. It's okay. The last feature that we need to add now is just the three mill circles around all four of the corners to do this. It's C on the keyboard, but in the circle, three diameter, enter. I'm going to hit D on the keyboard and dimension the center point, the vertical line. That's five on the drawing, then center point to the horizontal is also five. And quite simply, I'm going to use the mirror tool to mirror this across to this location, this location, and this one. Mirror line, first of all, the object, select the circle, mirror line or select this center line here, press Okay. Let's use the mirror tool again. So I'm going to right click and select repeat mirror. Under my objects, I want to select this circle, this one. In terms of mirror line, we want our vertical center line here. Okay, looking good. Now I'm just going to tidy up these dimensions. Okay, so that is the sketch complete. I did go through that quite quickly, but hope you were able to follow along, okay. If you were able to do this yourself, yeah, big, well done. That's fantastic. And so following this, I look forward to seeing you in the next sketching assignment. I'll see you there. 23. Sketch Assignment 2: This lecture is your second sketching assignment. So the assignment brief is to sketch this part using the tools learnt in this section. And there are many ways in which we can complete this, but our only concern is the final result having all the dimensioned geometries and that they are all fully constrained. So for the remainder of this lecture, I will demonstrate how to create this sketch using the tools learnt so far. So at this point, please pause the video and attempt this sketch, and I will see you shortly. Okay, welcome back, and I hope you got along well with the sketch. So now I will model this part myself and talk you through the tools that I'll be using. So, let's first of all, come up to create sketch. We can select any plane. In this case, I'll choose the XY plane. I keep the sketch grid off for this sketch, and hit L on the keyboard and start with a line tough from the origin, come up vertical, enter the dimension there is 60 mill. Enter. I'm going to right click, select repeat line, start from the origin, and come across on the horizontal by 84. I'm going to left click, come up by 18. Again, left click, come across 18, vertical 24. And then we have an angled line. So I'm going to put this in anywhere for the time being and then come across 24. I'm going to hit Enter on the keyboard. I'm just going to tidy up these sketches quickly and turn off the constraints. So we know that this point here and this point are horizontally constrained, and we have a tangential arc coming from this line across. So let's go on the horizontal constraint, select the endpoint here and the endpoint here. Then come up to create an arc. I'm going to go ahead with the tangent arc. I'm going to start that from this endpoint here. So we've got our tangency with this vertical line. I'm going to come across and finish our arc there. I just need to add in a dimension, so hit D on the keyboard, and I'm going to give that a rad. In this case, it's 12 mil. That's looking good. Everything's black in color, all fully constrained. You need to add the text in on this line here. It's come under create and text. And again, we want this to be on text on path, and we'll select our path. Is this line here. Text, in this case is Fusion 25. We want to make sure that we've got the fit to path option selected there so that the text starts at the start of this line and finishes at the endpoint. That's okay. I'm now going to add in the polygon here to come under create polygon. For this, I'm going to use inscribed polygon because the dimension given eight mill is from the center point of the polygon to one of the outer points of the polygon. Left click here. I draw that out eight mill, press Enter. It's got six sides. And here I know that this point is horizontally constrained at this point. So I use the horizontal constraint, this point to this point. Now black in color, fully constrained. Ahead and have the circle down here, C on the keyboard, draw that circle, 12 mill, D on the keyboard and dimension from the center point to the horizontal line 12 mill, and then again, center point to the vertical. Let's go 12 mill as well. We've got the Shafer down here, so the various champa tools we can use. But we know that this Shafer has two different distances. So in this case, it's come under the modification tools. Shafer. We're going to two distance Shamfa Do this line here, this line here. So we're going to control this distance first. That is five mil and then I'm going to control this distance, which is ten mil, let's enter. That's all looking good, and then just one more feature to add, which is the rectangle. So let's come under the creation tools and the rectangle for this, we use a three point rectangle, draw this in. So it has a length of 16 mill. Okay, I'm just going to click once, and I'll adjust the angle later. Then we're going to add the height in, which is eight mill Iso. Now we know that this line here is parallel to this line. So I'm going to select the parallel constraint, select this line here and this one. Then I know also that there is a vertical constraint between this point and this point. Choose my vertical constraint, this point, this point. And then there's a distance between these two points as well. So I hit D on the keyboard, this point to this point, come across ten mil, enter, and I'm just going to tidy up these dimensions quickly. Okay, so all of our entities are black in color. Everything's fully constrained. That's looking good. I hope you were able to follow along, okay. And if you did this yourself, a big well done, that's fantastic. And if you have any questions, please don't hesitate to contact me, and I look forward to seeing you in the next assignment. 24. Sketch Assignment 3: This lecture is your third and final sketching assignment. The assignment brief is to sketch this part using the tools learned in this section. This may look quite intimidating with all the various arcs, curved slots, and tangencies. But if we break this down, it's not too difficult, and it makes a good use of a range of tools for complex geometries. We need to get a bit creative here and ensure that in our final result, we have all dimensioned geometries and that they are all fully constrained. For the remainder of this lecture, I'll demonstrate how to sketch this using the tools learned so far. So please pause the video here and attempt this sketch, and I will see you shortly. Okay, welcome back. And I hope you did well during this sketch. And so now I will model this part myself, and I'll talk you through the tools that I'm using. So I'm under a new design, go to create sketch. Gonna choose the XY plane. Gonna turn the sketch grid off. And I'm going to press C on the keyboard, start at the origin, and go to draw the circle on the arc on the right hand side. So the circles got a diameter of 30. Then the arc has a radius of 30. So to a circle diameter of 60, and later we can trim this to just leave the arc behind. Going to input another circle. So somewhere over here, 18 mil diameter, and that's referenced by the 100 mil dimension to the center point of these circles. So I'm going to hit D on the keyboard and dimension between these two center points at 100 mil. We can also see that these are horizontally constrained. So I'm going to use the horizontal constraint tool, center point to center point. And now our sketch is in black, fully constrained. It's looking good. I'm also going to add in some more circles. So there is an arc down here with a rad of 15. So I put a circle diameter 30. We've also got an arc up here of 60, so circle diameter 120. We know that both of these are tangential to this circle here. I'm going to use a tangential constraint tangent this circle to this one and this one to this one. Now, let's move over to the left side where we've got this slot. So to model this, we need to input these construction lines. So I hit L on the keyboard, make sure that construction is selected under the line type. I'm going to draw a line out from here, like so. Do exactly the same from here. This will be our ten degree line, and then the same up here, which will be our 100 degree line. So let me put these angles in, hit dimension on the keyboard, select these two lines, our construction lines, add in the ten degrees there, and then we've got 100 degrees between these two lines. So now that we've got our construction lines in place, we can draw this curved slot. They're coming to create slot tools, which is the center point arc slot. We know the center point is here, I'm going to bring that out by the radius of the slot, which is 60 mil. And then we want to snap onto our ten degree line and bring that curve. I'll make sure the construction's turned off. Bring that curve all the way around to our hundred degree line, and then we're going to bring that out, it's got a radius of ten the arc, so that'll be a slot width of 20 mil. We've then got an arc on the exterior of this. So I want to offset this, press O on the keyboard, select the slot. I'm going to bring that out by five mil as per the drawing. Good. We know the circles tangential to this arc, so we can put in a tangency between these two. And then moving down here, we've got this straight line that's tangent to this arc and tangent to this circle. Press L on the keyboard, and I'll start somewhere on this arc and finish somewhere on this circle. Then use the tangency constraint between this line and this circle and then this line and this circle and this arc here. So that's looking good. We just need to use the trim tool now and tidy this up and trim away this part of the arc, this one, this one, these guys, also this one and this one. I'm going to tidy up these dimensions here. So where we've got a diameter, I want that to change to a radius. I'm going to right click and select Toggle radius and do the same down here. And so that is our sketch complete, but we can see that it's not fully constrained because we still have a number of blue lines. So there are a few dimensions which we just need to confirm. That is the width of 20. I'm also going to put in the distance here, the offset of five. And we just need to put in the dimension as per the drawing between these two center points, just 15 mil. And then if we look at this curve here, we don't have the tangency between these two. So let's input that. And that is the complete sketch. Fully constrained, as per the drawing. Looking good. And if you were able to draw it yourselves, fantastic, even if it wasn't fully constrained. And that concludes the third assignment. So I will see you in the next lecture. 25. 3D Modelling Section Intro: In the previous section, we studied the key elements of sketching, and in this section, we'll take those tools with us and begin to form three D models. We'll start by understanding the fundamental three D modeling tools such as extrude, revolve and sweep modeling before moving on to three D modification and construction tools. We'll learn about each tool's location and their respective keyboard shortcuts where applicable. We'll also study how to assign materials and add appearances to parts, and finally, how to create high quality rendered images of our parts or assemblies. At the end of this section are a series of three D modeling assignments for you to test your knowledge and capability to three D model infusion. All the tools required to model these parts are taught within the following lectures. So I look forward to seeing how you get on with these assignments. Just like in the sketching section, each lecture in the three D modeling section is presented step by step. And I will walk you through and demonstrate how we can use these three D modeling tools to generate complex three D geometries. I'll be giving a range of examples throughout the lectures, which I would recommend you follow along with me and take the opportunity to practice these tools and familiarize yourself with what they are used for. In the following sections of this course, I will be regularly using the three D modeling tools covered in this section, and so will you. Regarding the design file types, if you're new to fusion, let's stay with the hybrid designs. Make sure you choose the right unit system. So me, I'm going to use millimeters and grams. And if you're coming from a CAD background, I recommend for this section to use part design and make sure that your type is standard. And then, yeah, you can choose the correct unit system there. So, let's start three D modeling. 26. 3D Modelling Introduction: In the previous section, we studied the key elements of sketching, and in this section, we'll take those tools with us and begin to form three D models. We'll start by understanding the fundamental three D modeling tools such as extrude, revolve and sweep modeling before moving on to three D modification and construction tools. We'll learn about each tool's location and their respective keyboard shortcuts where applicable. We'll also study how to assign materials and add appearances to parts, and finally, how to create high quality rendered images of our parts or assemblies. At the end of this section are a series of three D modeling assignments for you to test your knowledge and capability to three D model infusion. All the tools required to model these parts are taught within the following lectures. So I look forward to seeing how you get on with these assignments. Just like in the sketching section, each lecture in the three D modeling section is presented step by step. And I will walk you through and demonstrate how we can use these three D modeling tools to generate complex three D geometries. I'll be giving a range of examples throughout the lectures, which I would recommend you follow along with me and take the opportunity to practice these tools and familiarize yourself with what they are used for. In the following sections of this course, I'll be regularly using the three D modeling tools covered in this section, and so will you. So let's start three D modeling. 27. Extrude & Extrude Cut: In this lecture, we will study the extrude tool. This tool is one of the key three D modeling tools in fusion. It allows us to generate three D geometries by either adding material or by removing it, which we call extrude cut. To demonstrate this, we'll be modeling this part that we see here. It makes good use of the extrude and the extrude cut tool. So we'll start off by doing some sketching and then I'll introduce the various options, controls, and edits we have when using the extrude tool. So to model this part, we'll start off with a sketch and an extrusion of the base. We'll then form the cylindrical feature at the back like this. We'll then create the slot in the top using the extruded cut tool. We'll then add the boss around the slot, and then finally, we'll use extruded cut again to remove material from the base. This is a good part to demonstrate for this lecture, as it requires us to use the extre tool for both adding material and also removing material. So let's start by sketching the base. So I have up and up fusion in a new design. Let's come up to the top left, create sketch. We're going to do this on the XY plane. Let's start off with a line tools, hit L on the keyboard. We'll start at the origin. And then I'm going to draw this line out 60. And then from there, we've got a tangential arc coming down with a radius of 25 on the arc tools, like tangent arc. Start from this endpoint, bring that around. But in 25, okay. Then from there, back into the line tool, come across by 60, and then we have another arc here. So I'm going to continue to do that in the line tool. Just go to hold down the left mouse button and drag that up to the endpoint here. That's good. So this sketch is not yet fully defined. We've got the tangency between this line and this arc and the tangency here between this arc and this line. We do need another tangency between these two here. We don't need one at the origin because the arc snaps on to the origin, and that forms a coincident constraint. From here now, there is a through hole on the left hand side, that's a radius of ten. So it's C on the keyboard, from the center, then a diameter of 20. Then we've got a center to center slot over here. Let's go create. But in the slot, center to center, it starts from the center point of this arc and comes across. I'm just going to put the slot in there and then dimension that up afterwards. So center to center, we have 12 mill, and then the radius of the slot, we have six mill. So that's our first sketch complete. And we have three profiles here. We have this profile. We have this profile within the circle, and this profile within the slot. Let's come up to finish sketch on the top right. Let's go on the home view. So next to the View cube, just hit the home icon, and let's come over to solid, and we've got the option to extrude here. So this is the shortcut E on the keyboard. And our toolbox pops up. In terms of the type of extrusion, we have the default extrude or the general extrude, which is most common. And then we also have thin extrude, as well. So this is very similar to shelling apart, and we'll be looking at that later. But for now, we're going to focus on extrude. In terms of profiles, we'll need to select one of the three profiles. So we've got one, two, and three. We want to select this one here, so I'll left click there. In terms of the starting point for the extrusion, we want that to be on the profile plane. So that is the plane in which we drew the sketch on. Now, there are other options like offset that we can't offset an extrusion by a distance. For example, if I select offset, I put my offsets, let's go for 50 mil, and my extrusion distance, let's say, ten, we'll see here that the extrusion does not start on the plane. It's actually offset by 50 mil, and then we've got our ten mil extrusion. That's not exactly what we're looking for. But exit that. Let's go back to profile plane, select that profile again. And then we have another option here, which is direction. So in this case, we're just extruding in one direction where we see the arrow is, like so. But we have got the option as well for two sides. So this is where we can control the extrusion in one direction and then in another, as well. So we've got these side one and side two. But in this case, we're just going to go with the one side. There's also symmetric, as well. So symmetric would be equal distance both sides. We said, let's say, 20 mil be 20 mil in one direction and 20 mil in the other unless we change the measurement here to the whole length. Which case, it will be ten mil in one direction and ten mile in the other. So an overall extrusion of 20 mil. Let's change the direction back to one side. We've then got extent type, so distance is where we state a distance for it to extrude. So we manually input a figure there. We've got two object, so that's in the case where we can extrude to another body or a face or perhaps a plane that we've inserted. And then we've also got all, as well. So this is where fusion would recognize all of the bodies within the path of the extrusion and then extrude up to that point. We'll take a look at that later. Keep it on distance for now. And as per the drawing, we have a extrusion of tent mill and a zero degree taper. So if I change the taper, let's say to 25 degrees, and then I click on the front view, we can see there that it's tapering. So I scroll this way, we see that taper all the way around. And if we want it to taper in the other direction, we can just put a minus in front of it, and it will taper like so. We're not so much interested in taps for now. We'll keep that at zero. And the last option here is operation. So we've got join, cut, intersect, new body and component. So we want to leave our first extrusion as new body. And then for any further extrusions, we can then investigate whether they are to join onto an existing body to cut that body, which we'll be doing today or to intersect and so forth. So let's press Okay. Next up, let's do the circular feature on the left hand side with the through hole and the slot running through it. So to do this, we want to sketch on this face here and then extrude from that face. So to do this, we can either click on Create sketch and then select the face, or a shortcut is just to right click and then select Create sketch. Now we're looking at that face perpendicular. I'm going to choose the circle tool press C on the keyboard, and I want to snap on to the center point of this circle here and this arc. If we move the mouse here, fusion will recognize. We're trying to get to the center point, and we'll see that blue circle. Let's draw that out, and we can just bring that to the origin as that's 50 mil. That's the diameter of this circular extrusion. We'll click there once. Then nice and simple. We'll come to solid, select extrude. Then we're going to select our profile here. So we do have two profiles available, but this is the one we want. Left click on there. In terms of the toolbox, everything here is to be left as default, and under distance, we want to enter in 30 minus ten, which is 20. And now as we look at the operation, you'll see that fusion will no longer be generating a new body. Instead, it will create a join. So that will join essentially this body to this one, so we'll just have one body. If I click Okay for now, and then I come over to my browser on the left hand side, and next to bodies, so if I hit the drop down, you'll see we just have one body, and we can choose to hide that if we want. Now, if I come down to my timeline, and I right click on the extrusion and then select edit feature. So I'm going to edit this extrusion here. Got my toolbox again. If I select new body and then okay, come over to our bodies folder, and we see we've got two bodies there. We've got the new body, which is generated and body one, we can choose to hide either one of these or show them, it can be really useful when it comes to doing any presentation work or demonstrations and such. But for the purposes of this part, we only need a join in this case, so I'm going to edit feature, change that to join, press Okay, and then we want to implement this slot, which is on this face here. So I'm going to right click on that face, hit Create sketch. Now for this, I'm going to use the centerpoint rectangle under my creation tools, rectangle, centerpoint. And again, I want to snap on to the centerpoint of these two circles here. But now we can see that blue circle. It's left click once Snap on there, bring out our center point rectangle. I want to make sure this comes exterior of the 50 mil circle. We're going to enter in a length there of let's say 60 millimeters, press tab on the keyboard, and then the width of this slot is 12 mil. Press Enter by geometry and place there. Let's come up to solid, select extrude again. Then we just need to extrude these certain profiles which are this one here and this one here. Now, notice that the default in fusion is to add material. For example, with this arrow here, fusion is wanting to add material to this part, but actually, we want to remove material in the other direction. So if we move the mouse down, we'll then see this red highlighted area indicating that material is then being removed. And also, if we look at the toolbox, we can see that the operation is not a new body. It's not a join, but it's a cutting operation, essentially removing material. So we want to leave everything as default. So starting from the plane we drew on, only going in one direction, and we want this to be a distance extent type. So in this case, the slot depth is six mill, so type in minus six. A operation is cut, and that's correct, and press Okay. There we have our slot in place on the home view. That's looking good. The next thing we need to do is add the boss, which encapsulates the slot just here. So to do that, I want to sketch on this face here. So again, I'm going to right click, go create sketch. And here I'm going to use the offset tool because the entities of this slot are all present. So if I hit O on the keyboard, or you can go into Modify and then select offset, we can then select the slot entities. So from here, I want to offset in the other direction. So I'm going to hit the flip, and then I'm going to enter a distance there of minus. So we've got the ads 11 minus six. So that'll be minus five. That's okay. Then you see we've got this profile here. That's the one we want to extrude. I'm just going to hit E on the keyboard and then hover my mouse over till we see this profile selected, not this one, this one. And then we're going to extrude that by a distance of four mel as per the drawing and leave everything else as defaults, and we do on that to be a joint operation. So it just remains within the same body. Click Okay. And there we have the boss surrounding the slot. And let's add one more feature to this part so we can practice again with the extrude cut tool. And for this, we want to sketch on this face, and they're going to take off some material giving us a slot on the underside of this part. So let's right click create sketch. And for this, I'm going to use a line tool and draw in a construction line. So under my line type hit construction, when I come across to I see the midpoint snap. Left click once, take that down to the midpoint snap of this horizontal. That's good. And let's turn off construction, put the palette back. Come under my create tools rectangle. Let's go with the center rectangle. And this is why I drew the construction line in place so that I can hover down and identify the center point of that construction line, which identifies the middle of this part, and I can just drag that out like so. I need to make sure that my slot width is exterior of both of those. So I'm going to go for 125 mil. And then in terms of the width, let's go for 12 mill again. Just enter on the keyboard. Then let's come up to solid. Let's go on extrude, and let's select the according profile. So we've got one, two, three. So in this case, we don't want to add material, so we don't want material coming out like this. So we're going to go in the other direction, make sure the operation is cut, and in this case, we're going for -4 millimeters. Leave everything else as default, press okay. Then we have the slot on the underside of this part. And that is our completed part. So it's a good practice of the Extrude tool for both adding material and removing. And just before we finish this lecture, please do remember to save this part as we will be referencing it in a future lecture. I hope you're able to follow along, okay. And again, any issues with either the sketching or the three D modeling, please send me a message. But aside from that, I will see you in the next lecture. 28. The Viewcube: In previous lectures, I've referenced the view cube a number of times. So let's take a closer look at what this tool can do and how it can streamline our workflow. As a quick summary, the view cube is a three D navigation tool that helps us to orientate our part or assembly. And so it's mostly used in three D modeling, but it can also be used in two D sketching as well. Ultimately, it can allow us to view our part or assembly from different viewpoints, I E, the front view, top view, side view, et cetera. So let's take a look at how this works. So we've got the view cube up here on the top left, and to demonstrate this, I'm going to be using the part that we drew previously. If we come over to the View cube, we have the option to select one of the faces here. For example, as highlighted the front view. If I click on this, I'm now looking at the part from the front view. And as we bring our mouse over the view cube, you'll see we have these four arrows around the cube. If we click the arrow on the right, for example, we'll then be looking at the right view. And then once again, the back view, left, and back to front view. Likewise, on the top, we can see the top view, and if you go to the bottom, we see the bottom view. And in the top left here, we've got the home view. So if we click that, I use that very commonly. When I'm modeling, it really helps for efficient modeling. So let me go back on the front view then. I just wanted to show you these two arrows up here. So if we select this arrow here or left click, we'll see that the part rotates 90 degrees in that orientation, so clockwise. And likewise, if we do the same with the other arrow, it will go counterclockwise. I go back to the home view. And a few options I want to show you, as well. So we have a drop down here, and if we select that, the very first three options that we have are the types of view that we're seeing. For example, typically, when modeling, we work in orthographic. For me, that's preferred. But some people like to use perspective. So I've selected perspective, and as you can see, the part looks different. It looks more somewhat three dimensional and realistic. Can be a really useful tool if we need screenshots of our models or assemblies, we're showing these with clients. We're doing them in presentations. Perspective can be nice for that. We've also got the option for perspective with ortho faces. So that means that I'm going to click on that now. That means that we're looking at this part in perspective view. But if we look at a face, let's say the top view, so I'm going to click that in the ViewCube. We'll now be looking at that view orthographically. So when we say from an angle like this, it's perspective, but then when we look at a face, it's orthographic. Let me give an example of that. Let's look at the top view. So here is orthographic. But if I change just to perspective, you'll then see the difference there, and we see that kind of element of realism, how we would perceive it with the human eye. I'll go back to the home view again. A few more options we've got here. So we can set current views as home. So where I click on the home, this is currently the home view. But if we want the home view to be, let's say, this corner here, so we can select the corners as well, or the edges. I'll click this corner here. If I want this to be the home view, I can go to my drop down and I can set current view as home. And then we've got the option of a fixed distance or view. So a fixed distance is the distance it's at now. So if I zoom out a bit, so then I go to my options set current view. If I go fixed distance, we will always see the home view from this distance. But if we go fit to view, then we go to the home view, this is our new home view, and it will sort of come to the screen and fill the page. We can also reset the home view as well. So I I left click Reset home, then go to the home button. We'll see you now on the original home view. We can also do the same as well with setting current views. So in terms of front and top, let me click on the front face. So this is currently front face. Let's say we wanted this face to be the front. I can do is I can set current view as the front, and then we'll see on the View cube it's now titled front. We can also reset that as well so we can reset the front like so, back to the home view. Going to put orthographic back on. That's how I typically model and we can also do the same process as well with the top view. So if for whatever reason, just for an example, if we wanted this view to be the top, set current view as top, and then we see that in the view cube, then all we need to do is reset the front, and then the entire view cube will reset to the default and go back to the home view. So that's an overview of the view cube. We can also left click anywhere on the cube and orbit like so. So it's a really useful tool for when a part modeling or working with assemblies, then you'll be seeing me use this a lot throughout the upcoming lectures. Hope that's all clear, and I'll see you in the next lecture. 29. Revolve Modelling: In this lecture, we'll learn how and when to use the revolve three D modeling tool. To demonstrate where this tool is used, I've shown some examples here. So on the left hand side are models that would typically be modeled using the extrusion tool, whereas on the right hand side, we would use the revolve tool. So the revolve tool enables us to rotate a two D profile about an axis, thus generating complex geometries such as gears and rotary components. So in today's lecture, let's revolve model a rotary part. This is the sketch profile that we'll be working with, and then once we've complete that sketch, we'll then proceed to revolve this around one of the default axis. So jumping into fusion, let's go under Create sketch. And for this, we could choose any of the default planes, and then we'll select the according axis for us to revolve that around. In this case, I'm going to go with the Y Z plane. I'm going to start with the line tool, hit L on the keyboard, and I'm going to start above the origin. So if we move the mouse over the origin and then come up, we can see we've got that snapping line there available. Left click there once, then that's come across by 100. And then I want to dimension this line here from the origin at a distance of 15 mil. And so once our sketch is complete up here, we'll then be revolving around this axis here. Let's continue in the line tool. We'll go from this endpoint, come vertical 40. Come across 60. And then from here, we want to come down and snap onto the endpoint of our hundred mil line here. Let's also put in a constraint, so let's do a vertical constraint between the origin and this point here so that everything is then fully defined, everything's fully constrained, and we can see the red padlock there. That's good. I'm just going to tidy up these dimensions quickly. Then let's come up to finish the sketch. Let's go on the home view and have a look at that. So we see our profile there. That's only one profile available. Let's come up to solid, and then we're going to select the revolve tool. We left click that once. Our toolbox pops up. We need to define the profile. So fusion has automatically selected this profile for us because it's the only one available. Under axis, we need to choose one of the default axis. We've got three here, blue, which is the z, red is the X, and the green is the Y. So in this case, we want to revolve this profile around the Y axis, so I'll select that one. Or alternatively, we can actually select it from the Who exit that. Alternatively, we can actually select it under the origin folder here. So we've got the three axis here, so we could just click Y, like so. On the home view, I'm going to turn off the grid. Then under the options, the main option is the extent type. So typically, that should be on full, which is a 360 degree revolution. We've also got the option of partial, as well. But this is where let's say we can rotate it by an angle of 180 or if we want to flip the direction, put a minus in front of it, and then we'll just have that 180 revolution, or we could go, let's say, 270. Another option we have is to an object, so that's when it comes into contact or interferes with another object. And in this case, we don't have that, so we won't be doing that today. Let's go ahead with partial minus 270 in terms of direction, so we're just revolving in one direction, but we have got the option to go two sides. So if we go two sides, we have two angles here, need to be careful about the minus. So in this case, we're going minus 270. Let's go minus 135, and let's also go the other direction, so we can just bring the wheel around like so. Okay and that's also a negative. So negative 135 in both directions gives us this. And we've also got the option for symmetric, as well. So just like extrude, it will revolve in both directions. So if I type in, let's just go with 90. Okay, so that's essentially 90 degrees in each direction. I'm going to keep that as one side. Let's go partial. And let's do minus 270. And in terms of the operation, yeah, we want this to be in the new body, the first body in this design. Is it okay? And there we have revolve parts. So that is the basics. We want to start off with a sketch. Okay, and then we need axis to revolve that round. Now, in this case, I used one of the default axes, but it might be that you're working away from the default axis. In which case, you can input your own. So, for example, I can actually draw a line in, let's say, here. Then if I finish that sketch, I'm going to delete this feature down here in the timeline. So delete that revolve feature, we've still got our sketch there. We'll come under solid, hit Revolve, we'll select our profile here. Then under axis, I'm just going to select the line that I drew in here, and we can see it's the same shape, but instead of revolving around the Y axis here, we've now revolved around our own line, like Okay, so that's an overview of the revolve tool. It's used somewhat regularly, but it's good to appreciate so that when we do come across these complex geometries, we know that there is a more suitable tool as opposed to the extrusion tool, which would be quite tricky and time consuming for a part like this. And we'll be doing examples later in the course when we use the revolve tool as well. And so I'll see you in the next lecture. 30. Sweep Modelling: In this lecture, we'll learn how and when to use the sweep three D modeling tool. On the slide here, we can see three examples of whether sweep tool will be used. The sweep tool enables us to create complex geometries by sweeping two D sketch profiles along a predefined path. This is a great tool if we are modeling piping or cable conduits or similar geometries. So in this lecture, I will demonstrate the principles by modeling an RClip using the sketch path as defined here. Jump inofusionGt a new design here. Let's create sketch. And let's do this on the X zplane. Press L on the keyboard, start from the origin. We'll go to the left 68 mill. They're going to hit L on the keyboard again and draw in a tangential arc. So they're going to hold down the left mouse button and draw that arc around, and I'm going to finish it roughly around there. Green tick move this dimension out the way. Press D on the keyboard. Dimension this arc here that has a rod of 12.5 mil. From here, we've got a straight line coming down to a series of arcs and then an endpoint over here. I want to put in the center points of these arcs and then I can draw the arcs from there. To do this, I'm going to come under create. I'm going to enter a series of points. My first points going to be roughly here, second is there, third is there. Now, these are the center points of each of the arcs. So we've got the dimensions for where they are. Let's go ahead and put those in. First one has a horizontal distance from the center point of this arc at 24.5 mil. Second one center point of this arc is 36.3. And the third one is 53.2. We know these two points are horizontally constrained. I'll go on the horizontal vertical constraint. So like those two points, then we'll press D one more time on the keyboard, and we'll put a dimension in from here to the origin. So that height dimension there is 12.5. And then the height dimension to the origin from this point is 5.6. Now we've got three center points in of the arc. I'm going to use the circle tool. I'm going to start a circle from this point here. Let's got a rod of five mils, so diameter of ten. Repeat the process for the other two points. And then what we can do is we can trim off any of these circles that we don't need later just to leave us with the arc. Let's go ahead and put in this straight line then. That's coming down here. I want to make sure that we're using the tangential constraint line to arc. We've got that tangency there, same process here, line to circle. Now it's black in color. That's constrained. We've got our tangencies in place. Nice. Let's do the same then. So line tool, let's go to these two circles, and let's also put a line tool to these two circles, as well. Again, tangency constraint, line to circle, line to circle. Same process here. Okay, all in black color looking good. And you can now start to see the part of the circle that will be soon to trim off. We've got one more line, which is the line that just finishes off this sketch. I'm going to put that point up here. Going to use the vertical constraint between this point and this point, and then I'm going to use the tangency constraint between the line and the circle. Then want to make this horizontally constrained with this point here. Use a horizontal constraint, center point there. That's looking good. Okay, everything's black in color. Everything should be fully constrained by the sketches, yeah, that's right. But the red padlock there, that's looking good. Let's go ahead now and use the trim tool then and tidy this up, so we don't need this arc here, but we do want this one. If we trim, select there, we're left with our arc. Same process for these two here, and now we have our complete profile. Going to tidy up these dimensions a bit. So what are the diameters, let's right click on them, toggle to radius, all three. And I just tidy these guys up. Okay, so that's one sketch complete. What we're going to do is we're going to finish sketch there. That was our path. Let's go back on the home view. And now we're going to do another sketch, which is going to be our profile, which is going to begin here. Let's go and create sketch. And in this case, instead of drawing on the X z plane, we want to be drawing on the Y Z plane. I'll select the Y Z plane, zoom in, and now you'll see we're looking at a 90 degree angle to how we were looking before. And we're going to start off with a enter diameter circle from the origin, which if I rotate the model, we'll see is the beginning of our sketch path. We're going to put in a diameter there at five mil press Enter. And that's our profile, and quite simply, we're just going to sweep that along this path. Let's go and finish sketch. Go up to solid, let's go and create. Let's go and sweep. In terms of the sweep command, so first of all, we need to define out profile. So I'm going to select this one here, Left click once, and the path, select this box, and then we're going to select that path. So this one here. Now, we need to make sure that we have chain selection on. If I do that again without chain selection, it will only take one entity. For example, if I click this line here, it'll only be sweeping down here and not the entire path itself. They want to make sure chain selection is on, and it will chain the entire path together. Left click there. The distance, we want to keep that as one. So the distance defines how much of the path we actually extrude along. So if we choose a distance of one, it means the entire path is followed. However, if we reduce this, so if I say let's say at 0.5, it will only go half of the way along this profile. And we can also control the distance with this arrowhead here. I hold down the left mouse button. I can actually drag it along the path, and as I'm doing that, you'll see that the distance changes. So this particular position is 0.786, and if I go all the way to the end, I will end up just about one. So we can control that by manually dragging the profile along the path. I'm going to leave that as one for now the taper wangle. So we could put in a taper angle there actually 0.5. Okay, we can see that tapering out, and then if I put minus in front of that, we'll see that taper down. But for an clip, the thickness should be constant, in that case, we'll put zero, zero. For the twist angle, it won't be applicable for this part here because the profile that we're sweeping along the path is circular. I'm actually going to just jump over quickly to another part that I've done here where the profile is rectangular, like so. Add in a twist angle there. So if I put in, let's go 45 degrees, we'll see that where our profile has started in that orientation, by the time it reaches the end of the sweet path, it will have rotated by 45 degrees, so twisted by 45. If I change that to 180, it is now in the sort of upside down orientation at the end. So that is an example of where we perhaps would use the twist angle. So let's go back to the arch wip. Orientation leave us perpendicular, so that's perpendicular to the path itself. And operation. So just like when we use other modeling tools, we've got different options here. We've got to join to, let's say, an existing body, which in this case, we wouldn't choose. In this case, we would go with a new body. But we've also got the option here to cut, as well. So just like inextrude or the same with revolve, we can cut by following a path. And I want to show you an example on that on another part that I've done here. So I've drawn in a cylindrical block, and then at the top here, I've drawn in a profile, and I've done a sweep path around the perimeter of this cylinder. So let's go and create. Let's go and sweep. Then in terms of my profile, I'll select the one that I've drawn in here. Then in terms of path, we'll select the perimeter, like so. And then we've got the same details so we can adjust here. So we can include tapers and such. We can also control the two arrows here. So, for example, if I do these, we can then manually define sort of how much that we're actually cutting away at this. But in this case, I'm going to stick with a distance of one and one, and then we'll make sure we're under the cut operation, so we see in red to remove material. We click Okay. As an example of where the sweep tool can be used to remove material. If we go back to the arclip. Again, for this one, we're going to keep as a new body, so let's click Okay. And there we have our complete arclip. What we can do is change the visual style. So if we put shaded with visible edges, we can then we can see more of the geometry and intersection points between how we did the sketch. We're going to leave that as just shaded for now. So it's a really useful tool, and now you understand the principles behind it. We can assess based on what we need to model, if we need to use the sweep tool or the revolve tool or the extrude tool, which is what we've covered so far. Okay, so I will see you in the next lecture. 31. Engrave + Emboss: In this lecture, we'll study the Ibo Engrave tool. This is a three dimensional tool that we can use to incorporate text into a part. Examples of where this can be used is branding or adding part numbers, and it is especially useful for when we are designing plastic injection molds. So here are two examples we can see on the screen. The text on the very top is what we call Imboss text, though it's where it protrudes from a face. And just below that, the text there is what we call engraved text, which is engraved or carved into the face. So let's move over to Fusion now and see how these tools work. So I've pre drawn a cube, as we can see, it's 100 by 100 by 100. The very first thing we need to do is to add some text. So we need to start a two D sketch. So let's go for this face here. Let's right click and select Create sketch. Now we're looking perpendicular at that face. Let's now come up to create and we'll select text. So like we did in the two D sketching section, we have the option here to either input a text box or we can write text on a path. So it's up to you. In this case, let's actually go for a path. I want to draw in an arc to a three point arc. Just going to use the vertical constraint tool to position that in the center. There we go. That'll do for now. There we go. That will do for this example. Let's come back into our text tool then, and let's go for text on Path. I need to define the path, and then let's input our text. So let's go for It fusion 2025. I'm okay with the size of that. I want to make sure that's in the center of this arc. Let's press Okay. Let's go on the home view. You can see our two D sketch in there. Let's now go finish sketch. Let's come over to solid tab under the creation tools. So the three D tools, let's use the one here called IBOs. The toolbox pops up. We need to define the profile, so we just hover the mouse over the text. I'll highlight in blue. Left click that text. And in terms of the face we want to emboss from, we're going to select this face here. Okay, let's take a look at that preview. It's looking good. So that's embossing by a height, a depth rather of two mils so far, so feel free to change that. Let's go for's go for four, okay? So a bit exaggerated. And then we've got the option to choose the effect. So whether it's embossed or infusion, they call it debo, but the term that we use is engrave. So, for example, if I select that, we see that red highlight there indicating it's removing material, and we can see it being engraved or debossed into that face. For this example, let's go with Imboss. And then in terms of alignment, we can offset this. So if I go on the top view, rotate that. We can use our arrows here to offset this how we like. We can also change the angle. I'm going to leave everything there is the default, zero, tab, zero, tab, zero. That's okay. Then if we rotate that, so we can use the ViewCube, we can see that looks good. We've got our four mil inboss text there. Exactly the same process for engraved or DeBoss. Go right click on this face, create sketch. Go under our creation tools, hit text. I'm just going to go this time for the textbox. Okay, start finish. Into my text. Let's go fusion 2025. I need to flip that orientation, both vertical, horizontal, place that in the center. I turn the text on bold. That's Okay, I'm happy with that position. Let's finish the sketch there, go on the home view. We've got our text in place. Come under the creation tools, and again, in Boss In terms of profile, we'll select the text there, and in terms of face, we'll select this face here. So, in this case, we just need to debosset's go for minus two, in this case. Just look at the preview there. Yeah, that's looking good. It's what we wanted to do. I leave all my alignments to zero, preso. Looking nice there. So that is how we Ibos or debos or engrave text, it can be part numbers. It can be brands. It can be any form of information, like a label. And as I say, for plastic injection molding, this is particularly useful. So a very simple tool to help us there, and I'll see you in the next lecture. 32. Adding Planes: In this lecture, we will learn when and how to use all of the varieties of construction planes. These planes are temporary reference planes that are excellent at helping us to model perhaps complex elements or designs. Just like the default planes, so the X Y, the X Z, and the Y Z, these construction planes are used for sketching to then later three D model, and I'll show you some examples as we go through each one. So let's jump into fusion and you'll see here that I've drawn in four existing bodies. So I'm going to using these to help me demonstrate a use for each one of these construction planes. The construction planes are located just at the top here so that under the solid tap and then as we come across to the right hand side, we've got construct. And if we open this up, we've got our eight planes located up here. So we're going to go through each one of these today. Let's take a look at the offset plane to begin with. So this is nice and simple. It's left click on this once. We have a toolbox pop up. And then here we need to define either an existing plane. For example, we've got the default, the XY, the XE, or the Y z, so just locate it down here or we can select a face. I can select this face, this one, any of these faces here. And to demonstrate this, I'm going to choose this face here. We'll then see our construction plane appear. And we can use the arrow here to either move that up if we want to sketch some geometry here or we can move it in the opposite direction and actually go into existing bodies. So in this case, I'm going to go into this body, let's say about 25, okay, press Enter, and then we see the plane appear here. We look on the left hand side where the browser is, come down to the bottom, you'll see a new folder has appeared called construction. And within that, we've got our plane that we've added here. So this one is referred to as plain nine. And we can right click and rename that if you like. I'm going to leave it as plain nine for now. We can turn off the visibility by clicking the I there, turning it back on like so. So let me give an example of why we might put a plane inside an existing body. Let me right click on that, and we're going to create a sketch on this plane. I go to go for actually, I'm just going to go for a rectangle, press R on the keyboard. I'm drawing a rectangle here, let's say 50 by 25. Press Enter. Let's finish that sketch there then, and you'll see that sketch is located on the plane that we've added. So we see the sketch just there. Let's now go ahead on solid, and I'm going to make an extrusion there. I'm going to draw the arrow up. Fusion will recognize that as a cutting operation. So I'll leave that there for now, and I'll come across and I input a taper. Let's go 15 degrees. Okay, and we see that tapering extrusion cut moving out there. If I press Okay, we've now got that feature added. Remove that plane. So that's how we add the offset plane, nice and simple, select the face, selectors position, and then we can begin sketching. The next construction plane is a plane at angle. So the second one down. So if we select this, we then need to define a line or an edge in which we can generate this plane from. So, for example, I'm going to choose this edge here if I left click once. Hey, I then need to input an angle. But here, I can control the wheel. Okay? I can input the plane like so, or we can input the angle. So I'm going to about 45 degrees plus enter, and now plane's generated, and then we've got plane ten under our construction folder appearing just there. Right click on that. Create a sketch. Let's put some geometry here. I'm going to go with a circle. Just going to draw that anywhere for the time being. Let's go 25 mil, go solid, extrude, rotate that slightly. Then with the arrowhead, we can move this to add material in this direction, or we can remove material if we add it in the other direction, but also we can add material if we choose a joining operation. But in this case, I'm going to go with the cutting operation, preso then you see we've input this feature here. Next, we have the tangent plane. So I'm going to demonstrate that using this cylinder here. It's come up to our construction tools. Let's go to the tangent plane, third one down, and then our toolbox just dictates that we need to select a face. In this case, I'm going to select this face, and we will have a plane that's tangential to this face here. Left click once and our plane appears, and then we can use the wheel to rotate that or we can enter in an angle. I'm going to control this by going on minus 315. I think that's the angle I want. Yeah, that's correct. That's okay. Now to demonstrate a use for this, I'm going to right click create sketch. For this, I'm going to add some text. To create text. I'm going to add it in a text box, all that out. But fusion 2025 plus okay, happy with the size and its position. And we see that text now upon that plane. So it's not wrapped around that face. It's just sitting on our plane 11, in this case. Turn that grid off. Then let's come up to solid, go to our creation tools, and let's emboss that text. I'll select the text, and the faces, I'm going to select this circular face. Okay. And then we can see we have that emboss text there, or it's actually engraved in this case. I want to switch that to IbosspsoG that from the home view, there we go. That's how we wrap text around in an embossed fashion onto a cylindrical face like this. A very straightforward tool to use. It can be very useful when we're referencing construction planes or any type of geometry from planes that are tangential to an existing face. And next, we have the midplane. I use this one quite regularly. It's the fourth one down, select midplane, and then we just need to define two planes here. Okay? So if we want a plane to appear in the center of this square, I'm going to reference this face here and rotate the model and select this face here, and then you'll see a mid plane appears in the center. Okay. And likewise, if I use the same tool again, the same on the other two faces, we've got that plane appear there. I'm going to pres Control Z on the keyboard to remove those, and I want to give you one more example of how we can use the mid plane. Let's say, for example, you choose this space. Now, we don't need to choose a face that's parallel to this one. For example, this one here, we can choose one that's perpendicular, so this one here, if I select these two, we'll then see this plane appear at a 45 degree angle, and we begin doing any sketching or work on that. So another very straightforward plane to use, and one that we use fairly regularly when model the next construction plane is the plane through two edges. I'm just going to hide this plane first, so our plane 12, let's remove that one. Come to construct, select our plane through two edges. This is very simple, so we just need to define two edges. In this case, I'm going to use my two bodies over here. I select this edge here, and then I'm going to reference this edge here, and you'll see how plane applies. Likewise, if I do the same thing, so two edges, let's go for this one, and this one here, we can create a plane, go through those two edges asll. But notice a slight limitation here where if we go through plane through two edges and we select this plane, we cannot select this plane as well. And so by means of angles, it's just not possible because the angle is indefinitely variable the further down this line that you go. So in this case, the two edges have to be parallel with one another. So if I hide this plane here, I'm going to do a sketch. Right click Create sketch. Make sure that we're looking at that plane. Let's go in this case, let's just go for a rectangle, a solid, extrude, turn around. And then we're modeling from this plane here. So we can use the arrow to push material out or remove material like so I press okay. We've then got that slot running through this body here. Let's move on now to the plane through three points. Let's come under construct plane through three points. And quite self explanatory in the title, we just need to select three points and identify these points within our model and then a plane will be formed. So we're under the selector already. I'm going to select, in this case, this point here. Let's go for this one and go for this one here. These three points, we should have a plane that will form that's in contact with all three of them. I very rarely use the plane through three points, but it can be used when working on something that's particularly complex. That's an overview of the plane through three points. The next construction plane is the plane tangent to face at point. So I'm going to go ahead and turn this plane off to demonstrate this. Let's go under construct. It's like plane tangent to face at point. In this case, again, I'm going to use the cylinder. So the face that I want this plane to be tangent to is this face here, and then I need to define a point. So this point can be any existing point, and a plane will form that's related to that point. For example, if I go for this point here, we'll see how construction plane form, and that can be really useful for when we're working with, like, complex geometries, and we need a plane to be in an exact location. I do an example there, right click, let's create a sketch. That's a good example of the plane tangent to face up point, got a tangency and then just referencing off any point. And the last plane is the plane along path. So we need a path to demonstrate this on. I've drawn one in. I think it's sketch nine. That's correct. So I've got a path here. It's going to construct. I want to select plane along path. And then very simply, we just select the path left click once, we'll see our construction plane appear there. And we can use the arrow there to manually position this anywhere along the path. Okay, or we can control this. So when it comes to proportional distance type, number one would be right at the end of the path and zeros at the start. But if I go 0.25, that's a quarter of a way down the path, 4.75 would be three quarters. And as we move this, we can see the distance will change accordingly. Another option here as well, it's physical. So this takes into account the actual length of this path. If we put a distance there of, let's say, 150 mil, it will jump 150 mil into the path. Likewise, let's go for 250. It's okay. That's how we put a construction plane in on a path. Then it can be used to sketch profiles, and then we can sweep along that path in either direction. Okay, so that is a summary of the construction planes within fusion. I hope that all makes sense, and you can understand where each of them would come into play. We will be using them throughout this course, for sure. I look forward to seeing you in the next lecture. 33. Extrude & Revolve to Objects: Now that we have completed the lecture on construction planes, let's revisit the Extrude tool and understand the use behind the extrude to object, extent type. So let's jump into fusion, and you'll see that I've drawn a few parts here to demonstrate this. Let's first of all, focus on this bracket and this plane here. So this is a construction plane that I've added. I use the offset plane tool and offset it from this face here. And on that plane, I've drawn in a circle. We're going to come up to solid, going to hit Extrude. We're going to select our profile that we want to extrude this one here. And then coming down under the extent type, instead of stating in a fixed distance, so if I said, let's say 50 or in this case, I -50, we can come under the extent type and we can go to two object. And then we've got a new option here to select an object to extrude two. So I could select this object here, for example, and fusion will calculate the distance and bring that material all the way up to this face here. We've also got the option here to add in an offset as well. So if we wanted to offset from this face, let's go for, let's say, 25 mil offset. Okay, well then see where 25 mill offset from that face. We can also add a taper in there as well. Put the offset back to zero, tab, put in a taper there. Let's go for five degrees. Okay, so then we're extruding with a taper with zero offset up to this face using the two object extent type. Other example, as well, so I've selected this face here. But we can also select any object. For example, I could select this object here, and likewise, we have that extrusion all the way up until that object there. I'll put that back as this face for now, press okay hide that plane or hide the sketch. Let's take a look at another example, then. So over here, we've got two cylinders that I've drawn in a sketch on this face, this circle here. Let's go and extrude, select that profile. Again, we'll come to the extent type. Let's go to object, rotate the model. Now I'm going to select this face here. Click once, and you'll see we're extruding all the way to that face, precalculated. No need to specify any distances. But in a taper there, let's go for ten degrees. Okay. And so those are examples of the extent type being object to. So a nice quick and handy tool to use infusion when extruding. Just a quick lecture there and look forward to seeing you in the next. 34. Fillet & Chamfer: In the two D sketching section of this course, we covered how to add fillets and chamfers to our two D sketches. And in this lecture, we'll learn how to add these features in three dimensional modeling. Adding these features in three D is our preferred route to adding fillets and chamfers because it avoids any conflicts or losses of dimensions and constraints in sketching, and they're also easy to modify later. So today, I'll be demonstrating these tools using this model here. I will include this part file as a separate download in the resources section, so feel free to download it and work with this part if you would like. Let's start with the radius tool, and there are a number of different things we can do with this. So both the radius and the Shafer tool are located under the solid tab, under the modification tools. We've got Fillet and ShafR available to us. We got the shortcut F on the keyboard for Fillet as well. So let's start with the Philip tool, it F on the keyboard. We've got our toolbox pop up. The first thing we need to do is either to select a face like so or an individual edge. In this case, I'm going to choose this edge here, left click once, and then from here, we can adjust this blue arrow to determine the size of the radius so that we'll do it manually or we can use the parameter box here or the one in the tool box up here. We're going to go with a rad of four mil in this case, and then presso. So that is the fundamental of the radius tools very straightforward, and I will give some more examples where we can do more things with radii. I'm going to right click on that feature and delete that F on the keyboard again. And now I'm going to select the same edge. But this time, under the radius type, instead of constant, I'm going to hit the drop down and we're going to select variable. In here, notice we have two arrows. So this one we can adjust, or this one we can adjust as well. And this will give us a variable fillet as we see in that preview there. We can control both of these parameters in the toolbox. So let's say at the start of this fillet, let's go for one mil. And let's say we finish with, let's go for six mil. And if we press okay, we've then got that variable fillet there. So one transitioning nicely into six mil right at the end of that fillet. We can also apply fillets to a face as well. But, for example, if I hit F on the keyboard, and then if we hover the mouse over this face here, there are eight edges in total in contact with this face. And so if we select that face, then move the arrow, we can see there that all of those eight edges are being radiid. Let's go. Let's go a three mill. Okay, press Okay. There we see we've done a shortcut there, so we can select any face and all edges in contact with that face will be radiid. Give her another example. I'm going to hit this face here, select that one. Let's go for a ads go have a two mill. Okay. So just a nice shortcut there where we can select faces instead of individual ledges. Example we should take a look at is corners. So corners are quite unique when it comes to radicing. Let's hit F on the keyboard and let's select individual edges here under a constant radius. Let's go for this edge here, this one, and this one. We're encapsulating that corner within that. I'm going to enter in a fillet there or let's go for two mill. Actually, I'll make that four mill, a bit more obvious to see. Now if we see the corner here, we can see that this nicely blends into the other three fillets. We've got the option at the bottom here for corner type. But this is currently what they call a rolling ball corner, whereas we've got the option there to do a setback corner. If I select that, see by the preview that fusion is now adding material into the transition between each fillet. And so I jump back to rolling ball. This is the default option, and then setback is another option we have there as well. I'll leave that as rolling ball for now. That's the standard. Preso. So we've taken a look at exterior edges. We've taken a look at corner points. Now let's look at joining edges like this one here. To hit F on the keyboard. We're going to select this joining edge just down here, left click once. Go to put in a fillet there. Let's go for four mill. And as we can see here, we're now actually adding material as opposed to this exterior edge where we would remove material. Fusion is now adding material and forming that nice smooth transition between this face here and this one here. Again, we can change the radius type, so I could make that a variable. Let's start from two mill and let's jump up to six and press Okay. And we can do transitions like this using the Philip tool. If we have a part which consists of different size fillets, we can include all of those different filets within one feature. So if I hit F on the keyboard, that's I'm going to choose this exterior edge here, I'm going to go for a constant radius, and let's give that 2 millimeters. We can then click the plus icon here. Let's add a selection set. I can then choose this edge here, and you see this one then appears in my toolbox. We can give this a rod of, let's say, one mil. I can add another selection set. And let's go for a face, in this case. Let's go for four Milt, and then we can press Okay. And there we've got different size fillets all included within one feature. So we don't have to have a huge list of fillets within our timeline. We can do all of them under one feature. We can always right click on that edit, and then we can select the according one we want to edit and make any changes from there. So that's an overview of the fundamentals of the Philip tool. Now let's move on to the ShamfaTol. So I don't have a shortcut assigned to this one. Again, we can do so about a three dots and add a keyboard shortcut. I'm going to just leave that as selecting under modification. So I'll click on ShamFA and then just like the fillet tool, we need to define either an edge, a face or a feature. So to demonstrate this, I use this edge here again, and we can use the arrow to add in our ShamfA like so or using the parameter boxes. So in this case, I'm going to go let's go for two mill So we got a 2 million shamfa there, and this type of chamfer is an equal distance. So that's 45 by 45. We look at that from the right view. We can see that's two millin from the horizontal and two millin on the vertical. And hence this is a 45 degree angle, or as fusion calls it an equal distance chamfer. I'll give another example there, use the same edge, but in this case, I'm going to use two distance chamfer. If I zoom in a bit, we can see we have two arrows. So number one determines the length in the horizontal and number two determines the length in the vertical. So we no longer have that equal Shanfa or that angle of 45 degrees. And instead, we're only defining two lengths, horizontal and vertical, and again, we can put these parameters there. Let's go over two and eight. It's okay. Look at that from the front view, and there we see we've got a much sharper angle there. So two millin from the horizontal and eight mill up from the vertical. Another type of chamfer we can add is the distance and angle chamfer. I hit plus, and I'm going to select this same edge here. And here you see we have an arrow, so we're defining a distance here, in this case, on the horizontal, and then we've got a wheel defining the angle of that chamfer. So again, we can modify these manually or we can input parameters here in the boxes. So let's go for a four mill in the horizontal and an angle. Let's go for 60 degrees. Okay. Look at that from the front view. There we have our four mill and our 60 degree angle, which will then determine the length on the vertical. Let's go back to the type of hamper being equal distance, and I'll just use this to demonstrate on joining edges, as we can see here. So if we select this edge, we then see we have this arrow. So if we draw that arrow out, we can then see we're adding in our shampa. So I'm just going to leave it as that, press okay. And again, just like the fillet tool, we're adding material there and forming, well, in this case, not so much of a smooth transition between this face and this one. As with the fillet tool, we are forming a transition of such, in this case, a 45 degree to 45 degree. Okay, so that is an overview of the Fillet and Chamfer tool. I hope that all makes sense. Any questions, please let me know. Aside from that, I will see you in the next lecture. 35. Shell Command: I In this lecture, we'll study the shell command. To demonstrate this tool, I've drawn in some models that we will work with today. And you can download these models if you want, from the lecture resources and feel free to follow along with me. So the shell tool is located up in the modifications tool, and it's this one here. So the third one in on the defaults shell or we're going to hit the drop down and we'll see it's the fourth one down, shell. And feel free to assign a shortcut if you'd like. So let's select the shell tool, and we have a toolbox pop up. So nice and simple, here we need to define either a face or a body. So in this particular case, I'm going to work with this cube, and I'm going to select this face here. And we can hold down the left mouse button and we can draw that into the shape, like so, and you'll see we have this preview of a shell. I'm going to put in a figure from that, let's say, five mil. So it's a constant five mil thickness on all the walls, and that includes the thickness of the base as well. So we've got some more options that have popped up now that we've select the face. These are the shell type. So for now, we're going to stick with a sharp shell, and I'll demonstrate round it later. This is the parameter where we dictate the thickness of our shell and then the direction. So we got inside outside and both. Let's stick with inside for now, and I'll show you the other two in a bit. Let's click Okay. And you can see we've shelled out this box. And if I come under the inspection tours and hit section analysis, I'm going to rotate the model and select this face here. Just use the arrow to draw that in on the front view. As we can see now, we've got this five mil thickness on the walls and also on the base as well. So that's the basics of the shell command, and that is a single face shell. Now let's take a look at the multiphase shell. So again, we'll come out of the shell tool, I'm going to work with this model here. And in terms of faces, let's select this face here, then throw in a value of five. That's okay. You'll see there we've shelled that out. But if we want to remove this face as well, we can quite simply do that. So I'm going to go back into the feature, edit the feature. And when we are identifying the faces, we just want to hold down Control on the keyboard and then select any other faces which we want to shell. I've just hit this face here. I'm going to press Okay. And now you'll see that we've removed those two faces, and we have our remaining five mil wall thickness. Another example of that. If I come back to the cube, right click on that feature and go edit. And here, hold down Control. I'm going to select this face here and also this one. So these three faces are selected, and if we press okay, we'll see then that we've removed those walls as well. So we can remove as many walls as we need. I'll give you another example on this part, right click on this part, hit Edit feature, hold down Control, select this face here. That's okay. Now I can see those two faces have been removed. So far, all of the shelling we've done has been in the direction of inside. Let's now take a look at shelling on the inside. So a toolbox pops up. I'm going to choose this face here, for example, choose this one. And then the default direction is inside. So if I type in there, let's say ten mil, we're shelling the inside of material, but notice that the wall thickness, so the thickness that we've assigned a ten mil is actually going on the inside direction. And if we change that to outside, and I put in another ten mil, we'll notice that the material is now exterior rather than interior. I go back to inside, okay, the material goes inside, likewise, outside. Outside. Another option we have in terms of direction as well as both. So where we have the perimeter of our three D model, if we select both from there, we can control the material inside and also outside as well. And we can use these parameter boxes to control that. Let's say we go five inside and let's say 20 exterior. We've come in five and where exterior is 20 mil. That's okay. So that's another useful feature when it comes to shelling the opportunity to shell in different directions or in both. And the last feature I want to show you is the shell type. Let's go on the shell command, and so far we have been working with the sharp shell type. There's also the option here for rounded, as well. I'm gonna go sharp for now. And if I select this face, hold down Control, select this face. Let's put five and five. This is the sharp shell type. But if we select the rounded shell, you'll see that every edge coming about from that shell command is now rounded like so. That's okay. Now, I just do one common shell feature, which would be for the vars at the back. To go here with a sharp shell, select one face, and I want that to be inside direction. Select this one. And let's go go for two mill thick bars. There we go. And again, if I come under inspect, go on section analysis. Okay. And then if we look at our bars, we see we've got that uniform two mill wall thickness coming about from that shelling operation. So that's an overview of the shell command. It's a really unique tool, very useful in certain circumstances. And I look forward to seeing you in the next lecture. 36. The Hole Command (Threads, C/Bore, C/Sunk etc.): This lecture, we'll study the whole command. With this tool, we can design many kinds of industry standard holes, including counterbore holes, countersunk holes, simple threaded holes, et cetera, all conforming to relative thread standards. In previous lectures, we've learned to create holes using the extrude command. I give an example here. If I right click create sketch circle, just draw in a circle there, solid, extrude. So like that circle. We've previously learned to make holes by extruding like so. Okay, we have a hole there. So in this lecture, we're going to explore the whole tool and what additional options that gives us. I'll right click on that feature and delete that, and then we'll come up to create. And if we look here, we have the whole feature, which is a shortcut H on the keyboard. So I'll hit H on the keyboard, and then our tour boox pops up. The very first thing we need to define is the placement. So whether it's a single point, so I a single hole or whether it's multiple points. So we'll cover that shortly afterwards. But for now, let's focus on a single point. So I'll select this, and then we need to define a face. So in this case, I'm going to select this face here, left click once. Now, as we can see by the preview, in the location that I clicked, a hole has appeared. I'm going to look at this from the top view. So this is not a fixed position, and we can move this as we want. So with the circle here, hold down the left mouse button and we can move that to any position we want. And if we see in the center there, there is a snapping point, which is the center of, in this case, a two dimensional square that we're looking at. We can step on there, but let's say that we wanted this in an exact location relative to these two lines here. What we can do in our toolbox is use the two references. So the first reference, let's click Select. I'm going to use this edge here as my first reference. I'll say 30 mill. And then I've got the option to add a second reference. So select that. I'm going to use this vertical line here, and again, let's go for 30 mil. And then we can position this hole exactly where we want it. So after we've placed our hole and we've determined its exact position, we then come onto shape settings. So first of all, we've got extents. So just like when we extrude, we can do a distance, which we set manually. We can do two, like to an object or a face, or we can do all, so all geometry in the way of where this hole is. So if I click A for now, you'll see it extends all the way down, and the preview shows us the hole going all the way through. We then need to define the hole type. We've got simple countable or countersunk. For this example, let's go with counterble then we need to define the tap type. So it's a simple hole, there's no thread, but it's a clearance hole, a tapped hole or a taper taped. So let's just keep it simple and go with this simple hole, and then we need to define the dimensions relating to this countable simple hole. So in terms of the height, okay? That's our very first parameter. Because we've selected the extents to be all, that will remain as all. And we can change that if we go into distance, we can then say, let's say a 25 mil hole, we'll see the preview change there. I'm going to leave that at all for the time being. And then we need to define the diameter of the counterbe, the height of the counterbar, and then the diameter of the hole. We can also do this manually as well. So we have this arrow and these two sets of arrows as well. So this arrow here would determine the depth of the counter baall. This would determine the diameter, and then this one here determines the diameter of the hole. So we can adjust those manually. But in the case of holes, I would always recommend to do them using the parameters here and get the exact dimensions that you're seeking. So as an example, for the diameter of the counter baall, let's go 50 mil, the height of it. Let's go 15. And for the diameter of the hole, let's go for 30 mill. Let's press Okay. There we have our countable hole. I'll just look at that from a section analysis. We'll see that a bit better. There we go. That's our hole there. So we could also do this using the Extrude tool, but it would be many different extrusions and sketches. I would take a very long time, and here we've got an accurate, exact countable hole as per our dimensions. Let's move on to another example of a hex snap. So we've got our hex nut here and we need to implement a through hole that's threaded. Let's hit H on the keyboard. In terms of placement, we'll go for a single hole. We can also define our hole type as well. So for a henut we'll go simple, want that to be tapped. And we want the extends to be all. So I'm going to left click on this face. I'm going to look at that from the top view, rotate that. Zoom in a bit. I want this to be in the center, right? So as we drag this around, we see the center point there. Let's snap onto that. Okay? There's no need to reference to any of the edges or the joining points. In terms of the dimensions, so we've got the hole going through all, which relates to the extents. We've got our diameter here, which we cannot edit. And the reason this is is because this is a threaded hole, so a tapped hole, and we need to use the parameters down here to adjust that. So in terms of thread type, we have many different related standards. We've got the ACs, dns and we got IOs down here. So I typically use isometric profiles. In terms of size, I'm going to leave that as 30 now, but feel free to adjust. You can't adjust that to 25. But for this particular size nut, I'm going to go with 30 designations. So that's the pitch thread. So I'm going to leave the standard there 3.5 class and then direction of thread, as well. If it's a right hand thread or a left hand thread, and then the final option we have here is modeled. So if I rotate the view now, we can see a visual thread in the preview. I click Okay there, see that thread is just a visual. So it's just a texture on top of this surface. It's not a physical thread. Whereas if I right click on that feature, edit feature, I I now select modeled, you'll see the appearance changes. I click Okay. We now have all these additional faces and geometries, forming a physical thread within that nut. And that's absolutely fantastic. If you are three D printing. This is what you want to have a physical thread so that you get that when you're three D printing. However, if you're designing many parts with many threads, I would recommend where necessary not to have the modeled selection ticked and just to leave them as visual threads. And the reason that is is because if you have many parts with many physical threads, all those additional geometries put quite a bit of strain on your computer's graphics card and processing unit. So where possible, I would leave it unmodeled and just as a visual thread like so. If we click Okay, there we have our hex nut with a visual thread. So far, we've covered single hole positioning. Now let's take a look at multi hole positioning. Let's press H on the keyboard. Then under our placement type, let's go on multi holes. Now, here we need to define sketch points. So we need exact locations for where these holes will go. We're going to do this on this block, but currently, I don't have any sketch points, but cancel on that. I'm going to create a new TD sketch on this face here. Left click once. Go on the creation tools, and we'll select points. Put in two points. I'm also going to draw in a line. I'm going to put that as a construction line, and I'm going to mirror these two points to the other side. We'll start at the midpoint of this vertical over to the midpoint of this vertical. Press D on the keyboard for dimension. Dimension this one, the vertical 20, and then to the top horizontal 20. Let's use the horizontal constraint between these two points. Press D on the keyboard again. We'll put in a distance here of 20, then that's fully constrained. Now I can use the mirror tool. Select these two points here. Then under the mirror line, going to select my construction line, and we can click Okay, then we can finish the sketch there, back to the home view. And let's press H on the keyboard, back to the whole tool. Let's go on our multi hole placement. And here we need to define our sketch points. So I'm just going to drag around this one, this one, this one, and the last one. Look at that from the top view, rotate that again. So that's how we use the multiple tool placement. We must have these points input in a two dimensional sketch that we can later identify as the positioning that we want to have these holes. So an example here, let's cover a whole type. Let's go on counter sunks and hole type tab. Let's just do simple. And under the extents, let's go through all. In terms of dimensions relative to the size of this piece, let's go on 20 as the diameter of the counter ball, 90 degree counter ball standard. And then the diameter of the whole. Let's go for 12 mil. Let's have a look at that preview. It's looking good. Again, we can adjust any of these parameters with the two arrowheads here. I click Okay. Now got our multiple holes positioned just from one feature. And again, like any feature, we can edit them by right clicking, slacking edit feature, make any according changes in our toolbox there. In the last example, I just want to show you that holes can penetrate existing features. For example, I've got this cube here with a slot feature running through it. Let's press H on the keyboard. In terms of placement, we'll go for a single hole and we'll select this face here in terms of positioning, snap that onto the center there. Let's choose the extensors all the whole type is simple, and let's put a thread on this one, as well. Let's go an isometric profile, and for the size of this, up 30 press okay. We can see we have our through hole feature there that is threaded running through an existing feature. Okay, so that is an overview of the whole tool. I hope that all makes sense. Any difficulties, please send me a message. But aside from that, I will see you in the next lecture. 37. Applying Threads: In this lecture, we'll visit the Thread tool. It's nice and simple to use and a great feature when working in Fusion 360. I've modeled up some parts here that I'll be working with. I'll add them as a downloadable resource, so you can download these and use them if you like. Otherwise, feel free to model your own parts and you can work with them. So on the left hand side, I've currently got a shaft, which we're going to add a thread to so that'll become a rod. In the center there, we've got a generic hex head bolt, and then right at the end there, we've got a nut. So we're going to work with two external threads and then an internal thread on the nut. Let's start first of all with a shaft, and let's make this a threaded rod. So the thread tool is located under the creation tools under solid There's left click there once, as we scroll down, we've got thread there. And again, feel free to add a shortcut if you like. I'm going to select the thread tool. And then our toolbox pops up and we need to identify here a face that we want to apply the thread to very simply left click once identifying this face. We've then got the option for this to be a modeled thread. So just like the whole tool, we can actually make this a physical thread. We can see right now this is just a visual thread that's been applied. But when I click modeled, you'll see then that a physical thread forms, which adds many faces and geometries. And this is ideal for three D printing. So any part where three D printing that requires a thread, we would always go with the modeled selection on. However, as explained, when we're working with a whole tool, if we have got a lot of threads within our parts and designs, we need to be a bit conscious about having them all modeled because it can be quite demanding on your graphics card and processing unit. I'm going to leave that as a model for now, then I'll scroll further down. So we've got full length, in this case, a threaded rod, I'm going to leave that as full length. Another thread type, just like in the whole tool, we've got all the various standards available here. I'm going to go with isometric profile. And the size, it's currently assigned 12 mill, and that's based off the diameter of what the shaft was. But we can change this. For example, if I manually move this arrow like so, it will change the diameter of the rod. And likewise, if I change the size here, so currently it's on 14, I bump this up, let's go to 24. We'll see the increase in diameter there. I'm going to drop that back down too. Let's go for 12 mile designation, sort of thread pitch. Leave that 1.75 standard, last, and then the direction. So clockwise or counter clockwise thread, then we can click Okay, and we're left with a physical thread there. That's a full length thread. Let's now move on to this hex spot here. Come in the decoration tools, go for thread. Going to select this face here. Left click once. I'm going to turn modeled on as well for this one. But instead of full length, I want there to be a shank and then followed by a thread. I'll take off full length. I want to offset this, so I'm going to offset this. So this will be my shank length. Let's Let's go for 25. Yeah, that's suitable. But in terms of length, I'm just going to manually adjust that. I'm going to leave that as a size 12 mill, but again, we can change this. So if we go to 18, you'll see the whole diameter jumps up in size. I'm going to leave that as 12 mill for now, leave everything else as the default. Press Okay. There we have our hex head bolt with a 25 mil shank followed by the thread. So those are two examples of exterior threads, and then on the nut here, we can apply an interior thread. Again, creation tools, go for thread. The face, we want this cylindrical face here, left click ones. I go to put this as modeled as well, ready for three D printing, full length, of course. And again, yeah, we can change this. So I drop this down to. Let's say seven, the diameter drastically reduces. Put that up to. Let's go for 14 mill, leave everything else as standard, right hand thread. Click Okay. Now we've got our physical thread. I'll just show you that through the section analysis by section from here. Like, okay. And then we can visually see or we can see much better here, the actual physical thread form as it weaves around. The same with our bolt with the shank and then with the nut as well. All of those parts are now ready for three D printing. And that's it for the thread tool. It's a very straightforward tool to use. Really useful especially when it comes to three D printing. And so I will see you in the next lecture. 38. The Projection Tool: In this lecture, we're going to take a look at projections. This is an incredibly useful tool when we are designing. Projecting infusion is the process of taking existing geometry, edges, faces or bodies, and referencing them into a sketch. So you can build new features based on these referenced geometry. So the key points here are that projections copies geometry as references, keeps designs parametric and avoids manual resketching. So let me give an example of where we could use projections. And from this, you have a good understanding of what this is used for. To demonstrate this, I'm going to create a new sketch. And for this, let's go on the Y Z plane. And I'm going to create a rectangle. Let's go to the two point rectangle, start at the origin. Let's go for a height of 40, press tab on the keyboard, and a length. Let's go for 100. Let's press E on the keyboard to extrude. Now fusions automatically selected this profile here, and let's just drag this out. Let's go for a distance of 50 millimeters, plus Enter on the keyboard, and there we have our three D model. Now I'm going to do a new sketch on this face here. And on this face, I'm going to I'm going to hit C on the keyboard and drawing a circle here. Let's go for a diameter of 15 millimeters, press enter. Go to hit. Let's actually go for a rectangle. Let's go for a center rectangle, start that here and I'm going to give that a height of 15 millimeters, press tab on the keyboard, and let's go for a width or of 15 millimeters. Okay, I'm going to constrain these in place. So I'm going to use the horizontal constraint. Come over to this line here, hold down shift, select the midpoint, and then I'll select the center point of the circle here. Then I'm going to do exactly the same with the center point of this square here, and I'll choose this point as well, right click. Okay. So the circle is now constrained with this point here. So we just need to give that a dimension from this line and the same with the square. We can only move left or right. It's a D on the keyboard, center point of the circle to this line here. Let's go for 20 mil, Enter. I'm going to repeat that process between the square and this line. Let's go for 20 mil Enter. Okay, that should all be fully constrained. Yeah, correct? Okay. And let's finish that sketch there. Now, let's go for E on the keyboard, so extrude. I'm going to select the circle profile and the square profile. Drag these in to make an extrude cut. And let's go for a cut of -10 millimeters. Okay, that's looking good. Let's press Okay. And now we have these two features in place. Now, let's say, for example, that we want to replicate these two features on the other side, but instead of extrude cutting, so going into the block, we want to extrude, so as to go away from the block. So this would be a manual process where we'd have to essentially sketch on this plane again, the circle and the square, reconstrain them, re dimension them, and then extrude from there. But projections allows us to project these geometries onto this face here. So I'm going to demonstrate that now. Let's go and create sketch, and let's select this face here. I'm just going to rotate the model. Now, remember that we're still working on this two dimensional plane here. So this face, what I'm going to do is I'm going to hit P on the keyboard. So if I hit P on the keyboard, we have the project tool come up. And notice that you can find this just up at the toolbar. So come Create. And we've got down here, project. Let's go on project here. Okay, so our tool bar pops up. And then we need to select our geometry. So I'm going to zoom in here and I'm going to select this circle here, and we'll see a preview of that on the other side, that red circle we can see. And then as a hover over to the square, we'll see exactly the same. I'm going to select the square as well. Now, we do have some options here, so we can either select specific entities as we've done in this case, the circle and the square or bodies. But in this case, we just want to go for the circle and the square. And projection link. We're going to leave this ticked, and I would recommend in the vast majority of cases leaving this ticked and you'll see why in a second. Let's click Okay. Now if we come back to where our sketches on this face, we'll see that we've projected these to the circle and the square. We've projected those geometries here. And then from here, we're going to hit E on the keyboard. Then maybe let's select these two profiles, and we can extrude them out. Let's go for ten mil press Enter. So that's an example there of how the projectol works. An example of where it can be quite useful. Now, back in the projectol, we kept the projection link. I'm going to show you why. Let's now go back into the sketch that we made these two on, which I believe is this one here, right click and edit. Now, I'm going to change these dimensions here. So instead of 15 millimeters on the diameter, let's boost that out and go for 30 millimeters. On the square, I'm going to change that to, let's say, 10 millimeters, and I'm going to change the height to Let's go over 25. Okay. And yeah, we'll leave it like that. And we're going to finish sketch. So we can see these two features have changed according to the dimensions that we change in the sketch, okay, as expected. And now let's see what's happened on the other side. We can see here that because we kept that projection link, we maintain that relationship, and this is a great example of what parametric modeling is. So here we can see our extrusions now conform to the change that we've made. And so we've maintained that relationship by using the projection command. So I hope that makes sense. And if you have any questions on projections, please don't hesitate to send me a message, and I will be using projections later on in this course, so we'll be sure to revisit this tool then. So I'll see you in the next lecture. 39. Assigning Material & Appearances: In this lecture, we'll take a look at how we can assign materials and appearances to parts or assemblies. So first of all, let's differentiate between materials and appearances. A material assigns physical properties as well as an appearance, whereas an appearance only assigns a physical appearance. And so if we are wanting to understand the weight of a part, for example, we need to apply a material from Fusion's library of materials to get a realistic representation of the weight based on the materials associated density properties and the volume of the part itself. And Fusion will pre calculate this for us. Another example of where we would want to apply material were to be if we intended to use stress analysis simulations, we would want to ensure that the according material is assigned to stress test those specific properties under the stress conditions. So let's jump into Fusion now, and let's come up, first of all, to our profile, and then let's click on preferences. And under here, if we scroll down to where material is and we select this, we can see what the default materials and appearances are. But, for example, here, we've got the physical material category is a metal, and then the material, so the default material assigned to any part that we draw is steel. And in terms of the appearance, we just down here, we've got steel satin. And you can modify this how you like, so these are the defaults. So if you wanted all your parts to be let's say in copper, we just select copper, press apply, and then go from there. I'm gonna leave those for steel for the time being. In terms of assigning a material or appearance, we come up to the modifications tab, hit the drop down, and then we got physical material here and appearance here, which is A on the keyboard for a shortcut. So let's start with the physical material first. Our tour boox pops up, and at the top, it says, In this design, and this will be the default material that Fusion assigns. I hover my mouse over. We'll see it's a steel there. And then as we come down, we've got our library. So within the library, we have a range of materials, and we can select any one of these, let's say, the metals, and we can scroll through, and we've got a huge library of available materials to us, which come with their own properties and appearances. We've got our aluminums, got some aluminums anodized, brass, copper, gold, iron. We get down to stainless steel and the carbon steels, et cetera. So let's say, for example, we wanted to change this material from a steel to an aluminum. We come under the metals folder, scroll down. I'm just going to go with the generic aluminum here. There are different ways we're going assign this. Number one, we can hold down the left mouse button and actually drop it on the part, or we can drop it on the body itself under our browser. And another way as well is just to come up in this design and then just drop it on the preexisting material. So if I go ahead and do that, we'll then see that now our aluminum is in this design, and we'll see that the appearance of this part is changed to that of a aluminum. So this aluminum that's assigned has preset properties. And we can edit those if we right click and then select Edit. We can straightaway change the density, also change the name as well, and then we've got the advanced section. I won't go through all of these here, but let's take a quick look at physical. We can change any one of the, let's say, the thermal properties or mechanical properties. So if you're working with a material that's been supplied to you with its own data sheet, and those properties aren't quite in line with the defaults of fusion, you can go ahead and adjust these as you need if you wanted to progress on to do any form of simulations. Look like counts all there. So that's how we assign a material. Quite simply, we select it and let's go for another one. Let's go for a ceramic, have a porcelain. I'm going to drag this up, drop it on the existing one. We see the appearance has changed, and now we're working with a porcelain part. I'm just going to change that back to the default, which is steel, and then we can move on to appearances. Close the physical materials. Let's come up to modification now, and then here we have appearance. At the very top, we need to select whether we're applying an appearance to a body, a component or just an individual face. If I just select face, then it would just be an appearance assigned to an individual face. But in this case, I'm going to go for the bodies. So in this design, we've got the default appearance, which is a steel satin look. Let's say we wanted this part to be painted. So let's go for a paint for a glossy paint. And then let me just move this over. What we'll see is we've got these download icons next to some of these appearances. So this only appears in the case that we need to update that appearance and have it more local, then we can apply that. For example, if I go for the blue, click Download. I'm just going to drag that up and drop that on my existing appearances and design, and then we'll see it's changed to a nice blue color. In this case, enamel glossy blue. Let's go for green. So same process, drop it above. Let's now go for an individual face. So let's choose let's go let's go for the gray. We're going to hold that down. Then we're going to actually drag it over the part, and we're just going to drop it on this face here. Likewise, for the blue, drop it on this face there. And that's how we can apply appearances. Another handy tool within this library is the ability to search the library. So we've got a lot of appearances listed under all these folders here. But if we do a search, let's just say we go for type of just having red, for example, come to the Fusion appearance Library. We've got all these variations of red here available to us. And we can choose to use these. Let's go for a match drop this in. Okay, something like that. Okay, so that's a summary of applying materials and appearances, and I will see you in the next lecture. 40. Decals & Images: In this lecture, we'll learn how to add dackls to our part files. And this is very straightforward, and Fusion makes this really easy for us. So to demonstrate this, let's create some parts to put these decals on. Let's go and create sketch, select the XY plane, its C on the keyboard, start from the origin with diameter of 50 mil, press Enter. I'm going to press R on the keyboard. I draw in a rectangle. Let's go 50, hit tab on the keyboard, press 50 again, Enter. Got two profiles there. Let's finish this sketch. Let's press E on the keyboard for extrude. Let's select this profile and this one. Then in the parameter box, I'm going to put in 100 mil enter. Now we've got our two parts. So our cylinder and our block, let's go ahead and put a decal on both of these. So on the cylinder, I'll show you about wrapping a decal to a face. And then on the block, we'll just go to one face and also multiple faces as well. So let's come up to the top and our insert, let's hit the drop down. Then we have decal just here. Left click once. And then Fusion will bring us to our project folders. And so if you're storing your decals or images in here, fantastic. I've got mine just down here, fusion logo dot PNG. But otherwise, if you want to pull a file from your computer, you can select Insert from my computer, locate the according file, and Fusion will import that. I've chosen my image, and I select insert, then our tour boox pops up, and very simple, we just need to define a face. First of all, let's go for this face here. Left click once, Look at that from the front view. And we can adjust this manually so we can move it up and down on the Y, cross on the z. We can also flip it horizontally, so we just left click once in the same vertically as well, like so. We can rotate this to any angle that we need. We've got the square here, so that's just a free move. Can move that anywhere on the X and Y. We've also got the scales here as well. So the one on the corner is a uniform scale, and the one here is a scale in the Y axis. Go put that back as one, and then the other one is a scale in the X axis, and I'll put that back as one as well. So let's position this roughly in the center. We're going to scale that up slightly. Let's go for this size, looking good. And then we have all of those options available to us in the toolbox. So the very first option available is opacity, so we can use the slider there. If we bring that down, we'll see there that parts becoming very much transparent. Bring that up to 100, control the distances, angles, and scaling. I got my flips here as well. We're going to press Okay there, rotate the part, and we'll see that logo nicely positioned. Let's go ahead and edit this decal, then right click, select edit feature, and that's move this up until we breach onto this face here. I continue to drag up just for an example there, and then we can see that the logo has kind of wrapped to this face and this face. Likewise, we can do that with other faces as well. So if I drag in this direction, we can see that it wraps around, although it doesn't look kind of odd if we do that. So I'm going to move that back, keep it on this face here. Press Okay there. Okay, let's do the same full of cylinder, as well. Commun insert decal. Select my same image insert. Gonna select this face here. Not too keen on that angle. Let's rotate that around. Yeah, so -90 degrees on the z, reposition that. Go to scale that up slightly, as well. Okay. Then we can see that that has wrapped around the cylinder. It's a really nice tool to use in fusion, very straightforward. That is how we insert decals into our parts. Hope you're able to follow along, okay. Any questions? Please let me know. But aside from that, I will see you in the next lecture. 41. Rendering: In this lecture, we'll learn how to use the core rendering features in fusion. Rendering infusion is a fantastic way to generate high quality images, and I much prefer it over other CAT softwares which tend to overcomplicate rendering tools. So to demonstrate this, I'll be using the part that we modeled in the extrusion lecture of the three D modeling section. So feel free to use this part if you'd like, or you can experiment with any other parts or assemblies that you've modeled. So let's jump into fusion. And if we look at the tabs at the top on the left hand side, you'll see that we're currently working in the design environment, which has been the environment we've been working on so far in this course. Let's hit the drop down, then it's come down to render. Now we enter the rendering environment, which looks very different. We can already see our part there having a different visual appearance. In terms of the render tools, if we come up to the top under the tab render, we'll see we've got the setup tools, the ability to in Canvas render. So that's in this environment here. We can just render without then generating JPEGs or PNGs, and then we've got the final render option here. So today, we're going to be taking a look at appearances, the scene setup, decals. We'll take a look at the in Canvas renders and the final render setup as well. So let's start with the setup then. Let's come into appearance. And following on from the materials and appearances lecture that we did, the appearance toolbar is exactly the same as in the design environment. But here we can apply appearances to the bodies, components, or individual faces. Currently in my design, I've got the default steel satin finish, which is associated with the steel material. I'm going to change that though and come down to my library. I'm going to choose a metal, and I want to choose a aluminum in this case. And we're going to go for aluminum anodized rough blue. We make sure that we've already got that downloaded, which I have a left click, drag that across, drop that on the part, and we'll see the change there. We'll then click Close. Next, in the setup, let's take a look at the scene settings. So there are many options that we have to play with here. We've got the settings, and then the other tab is the Environment Library. When it comes to the settings, I suggest that you have a play around with these and familiarize yourself with each of the values that we can change. And if you ever want to revert back to the default settings, we've always got the option here at the bottom to restore defaults. So if we do change some of these figures, we can't quite remember what the defaults were, we can just simply click here. So in terms of environment, we got the brightness. So this is measured in lux. To illustrate what type of lux values might be relevant to the type of scene that you're generating, I'm showing a table here, which is a generic guidens table telling us the according lux values as per the type of scene that we can sort of expect to achieve from there. We've then got the position as well, so here we can position the light. So currently got that on around 75 degrees. We're going to adjust that like so when we see the shadow moves around. Put that back to 75. Once we're done with position, make sure that we click off it. We're all the background. So here, I've got a single color gray background. Now, if you want a solid color background, you can adjust it here. So we click and edit. We can adjust this anyhow we want, so we can move the mouse c. So let's say here, we click Opli. We've got a very harsh red there. I can move over to. Let's say a blue, go free. Okay, looking nice. But for this one, I'm going to stick with the green, something along the lines of this. We've also got the option there as well for environment. So if we select the environment, then we come under the environment library, these are the fusion built in environments. If we want to use any of these, let's say, field, for example, we can left click and drag it into the environment and then drop it like so. If we pan around, we can then see that we are in a field. But the default is cool light. Okay? And if we come back to settings, and we change that to solid color or then revert back to the green that I selected before. Underground, we're going to include the plane, which will give us a shadow. So for example, turn the shadow on and off. Got the option to flatten ground and also reflections as well. We we see this reflection in the ground plane, we can adjust how sharp or kind of blurry or rough that is with this slide here. So if we go all the way up, that's the most rough and all the way down is the most sharp. Leave that as 0.1 as the default. The camera, we've got the options, so just like we did in the design environment for orthographic view, like so, and the perspective being a more kind of realistic three D appearance. And then there are options for focal length and exposure, which I'm going to leave as the defaults, but feel free to have a playground with those. One thing I will show you about the focal length, let's go back to the environment library. And if I throw the field environment in there, come back to settings, make sure my background is the field setting. If I adjust the focal length, it will also play an effect on the background as well. And in this case, we might want to turn off the reflections. Okay, let's cut close. Moving on, we've got the options in this environment to add decals. So I select that, then need to choose our decal. So that's in your fusion projects, you can find your appropriate project in the image there, or you can insert from your computer. I'm going to go ahead and add in my fusion logo, which is under my fusion course project insert. Let's go for this face here. Okay, that's looking quite interesting. One option we do have this environment is to use in Canvas renders. We don't have to perform a complete render, but we can look at a IcavasRnder, which is essentially a preview. If I click In Canvas render. And then if we move down to the bottom right, you'll see here that we've got options to adjust this slider here. I can adjust it in any direction. Here is referred to as a excellent render, which has so many iterations. I will give us an excellent render, supposedly. We then got the final render, which I believe is 100 iterations, and then infinite. So infinite is when we would then later pause once we're happy with the number of iterations upon that part. Now, this is being done locally. So your graphics card, your processing unit, is processing each of these iterations. So depending on your hardware, this will determine how long the render takes. I've just got this going at excellent quality at the minute. Got this background, the settings that we set, the settings that we set in the scene setup and this part here with the logo. And that's looking okay as an in Canvas render. Just one thing I would advise here, because it's in Canvas, we can actually rotate this and continue to work with it. I would suggest that if you are doing that, to turn off the in Canvas render. And by doing so, we're not asking too much RPC, and also it's not necessary for when we're here adjusting parts and such. Also, under the in Canvas render, we've got options to adjust some of the settings there, and we've also got the option to capture image as well, and we can save that locally. And then finally, we've got the option to render. If we select this so there are some presets here and a mobile web print video, but in this case, I'm going to go for custom my image size. I'm going to leave that as a 16 by nine ratio, one megapixel. Leave the exposure as default in the file format. I typically do as JPEG. But if you do do a PNG, you can make the background transparent. I'm going to leave that as JPEG. I want to have the background in there. And under the renderer, we can do this either in the Autodesk cloud or we can do it locally, so on RPC. Doing this in the Cloud is a good option. However, it requires us to use Cloud credits. And depending on your license type, you might have limits here. And to be honest, I don't notice any particular difference in render time compared to running it locally. But again, it would depend on your PC and what you're doing at the time. So I'm going to go on a local render, make sure we've got the advanced settings open, and then under here, we can adjust this slider. So the number here represents the number of iterations. So a draft would be 25 standard 50 iterations, final 75, and then excellent quality would be 100. For a final output render, I would always recommend either final or excellent. But in this case, I'm going to go with final and then let's click Render. When the render begins, it will appear in the bottom left here in our rendering gallery. If you hobble the mouse over it, it will tell us some details, like how long it will take the image size, render quality. And once that's complete, it will then show, and then we can go ahead and save that image. And then our render is complete. I think that's looking okay, quite happy with that. And if we come up to the top here, we've got the option to download, and then we can download that locally and make sure we got the right file type selected. So in this case, we rendered as a JPEG, so we've got type JPEG, click Save. And there we have our final render output. So that's an overview of the rendering capabilities with infusion. If you are rendering regularly, I strongly suggest that you have a good study of the parameters that you can adjust in these scene settings. I look forward to seeing the renders you produce in the future. And I will see you in the next lecture. 42. Part Properties: This is just a very quick lecture where I'll show you how we can review part properties, such as the surface area of a part, the density of that assigned material, the total mass of a part. It will also confirm the assigned material and appearance, and also show us the center of mass location and a few other properties as well. So I'm going to be working with this part here. Let's say, for example, we wanted to understand what the mass was and just double check what the assigned material was and perhaps the density as well. If we come over to our browser tree, where we have bodies, we have body one, which is this part here. We're going to right click on that. We're going to come down to properties. The left click once, our toolbox pops up. We have all the information here. So we've got the total surface area millimeter squared, the density of this particular material. And if we look down here, the physical material assigned is the default infusion, which is steel. We've got the mass of this part, so it's coming in at one kilo as these dimensions. The volume of the body, confirming the appearance, which again is the default that goes alongside steel, so steel, satin finish. Then we've got the center of mass and some other properties here. One useful tool here if you want to communicate this data with your client or boss, you can copy the clipboard and then paste that perhaps in an email or a document if you're doing a report or something like that. So yeah, a very quick tip. Come over to the browser. We right click on the body, go to properties. I've got all the relevant data there. And one quick tip, you'll see here that all the units I'm working with here are in metric. If you work in imperial, no issues, that's okay there. Come across to the document settings under the browser. Next to the units. Let's change those guys to inches. I'm going to right click on the body again, go on properties, and then you'll see the units are in imperial measurements. So I hope that helps, and I'll see you in the next lecture. 43. How to Cross Section: This is just a quick lecture on section analysis. It's a tool that you would have seen me use in previous lectures. We're on to run through it in a bit more detail in this lecture. So let's say that we have this part here, I'll include it in the resources section. So if you want to download it, feel free to do so. Now, let's use the section Analysis tool. So it's under our solid tools, and we come across to inspect, we hit the drop down there, and then we come down to section analysis. And from here, we need to determine a plane to start the section analysis, but also we can choose a face. For example, I could choose this face here or this one, this one, and this one. But to demonstrate this, I'm going to use the X Z plane, which is this one here, and we can select that from the origin folder in the browser. We can come down to Zed. So I'm going to left click once. Within my toolbox there, I just want to quickly flip this so I'll select the flip icon. And now you can see that we've cross sectioned this part, and we can see this additional detail in here. So there's a change of diameter, which we couldn't otherwise see if we hadn't done the section analysis unless we looked from the top. So when we've implemented our section, we can adjust it. So we can offset that from the plane which we chose, okay, like so. We can also specify a distance in here. So the distance offset, let's just go for zero for now. Angle one, so again, we can adjust the angle of that plane. In this case, this is around the X axis. I'm going to put that at zero, and then this angle, we can adjust using the wheel as well, and we can adjust that like so. Again, put that at zero. We've got a section color here as well. So you can use from component, or you can go custom in which case you can select here and make any color change. Let's go for a red. Okay, and then we can see where the part has been intersected. It's now red in color. So let's click Okay, now we've done our cross sectional view. That's looking good. But how do we come out of that cross sectional view? To do that, we come over to the browser, and you'll see that we have a new folder input here, which is analysis. So in this case, it's called Section two. We can right click and rename that how we like. We can delete it or edit it. We can also hide, so hiding that section. So it's just normal. So we can actually keep that section view there for future. Let's say we do some more edits. We want to see that section again, and we can just click there. So nice and easy. Remove it, as I say, just right click select delete, and then the whole folder disappears, and then we're left with our original part. Okay, so yeah, I just wanted to cover that. It's a really useful tool, and I'll see you in the next lecture. 44. Export STL 3D Model: In this lecture, I'll show you how to export files in a dot STL format, which is suitable for the vast majority of three D printing slicing software. So I'm going to use this part to demonstrate. There are two ways to do this. There's a very quick and simple way, which gives us a very standard STL file to which we can't edit the mesh. And then there's the more detailed way to which we can edit that mesh. Let's start with the simple way. Let's come up to the top left where we've got file. Click the drop down there. Then we come down to Export, left click once. Then very simply, we can just choose a location on PC and save that file and make sure the type here is STL. But if we want to edit the mesh and ensure that we get some nice smooth curves like what we see around here, we can come across two bodies where we have our body there or if you have multiple bodies, right click, then come down to save as mesh. And then another toolbox, we want the preparation type to be export, the object, which Fusion has already selected for us, the format, yet, keep that as XTL unit type millimeters, which pulls in from the document settings here. Then if we do a preview of the mesh, come into the top view, see that a bit better. We can see that there aren't a great deal of triangles here around the curvature areas, and this may result in a low quality print, depending on what settings you're using in your slicing software. Therefore, if we come over to our toolbox, hit the refinement settings, then under the refinement, currently we're on the low setting, so we've got a triangle count, 744 triangles. Let's bump that up to Let's go for a high triangle count and see the difference there. Immediately, we can see many more of these triangles form and especially around any complex areas, such as the circular areas, any arcs or the slot. And so by leaving everything else as a default here, if we then click Okay, we can then either save that to our projects or we can save that to our computer, choose a suitable location, and then click Save. And that is how we export an STL file in fusion. 45. 3D Modelling Assignment 1: This is your first three D modeling assignment. It builds on the fundamental three D modeling creation, modification and construction tools covered in previous lectures. This part requires us to use various three D modeling commands and we'll test your understanding of each one. The dimensions for this part are shown in the three D technical drawing here. This is displayed in third angle projection and will help you to visualize and understand each feature's geometry. Now there are multiple ways in which we can model this part, so there's no single correct method. The key objective here is to achieve the same final result. But during this lecture, I will demonstrate a method and selection of tools to model this part. And so at this point, it is recommended that you pause the lecture and attempt modeling this part. And once complete, you can continue watching this video to see one modeling method that I will demonstrate. So if you could pause the video here and have a go at modeling this part and I'll see you shortly. Okay, welcome back. I hope you got along well with the part. And so now I will model this part myself as a demonstration, and I'll talk you through the tools that I'll be using. If you do have any questions, please feel free to contact me, but aside from that, I'll begin to model this part. So let's jump into fusion, and let's take a look at this part. It's built up of several extrusions. We've got some fillets. We've got a non equal hamper. We've got some threaded countersunk holes. We've got some extruded text in there, and we've also got a deco as well. So there's quite a lot of features within this part. Let's start now by drawing the base. I'm going to press C on the keyboard, I'm gonna do this on the XY plane. R on the keyboard, rectangle, start of the origin, to draw that out. That has a horizontal length of 96. Press tab on the keyboard, and we've got a vertical there of 64. Okay, that's looking good. Let's continue with the line tool then and we can input this slot feature just here. Go back to the top view. I'm just going to draw this in anywhere for the time being and then position that more accurately later. That's got a dimension of 20 mil, and a left click once there, H down the left mouse button, I'm just going to drag out an arc, let's say somewhere here, bring that back to the start line. Move that dimension out the way, press D on the keyboard. Let's put in the rad here. But this slot worth 16 mill so that'll be a rad of eight mil per center. Then we want this point to be aligned with the midpoint of this line here. For this, I'm going to use the horizontal constraint, start at the center point of the arc. All down shift on the keyboard, and then we select the center point of this line here. Now that's fully constrained. We double check our sketches, see the red padlock there. That's looking good and ready for us to extrude this profile here. Now, at this point, we could input fillets on this corner, this one, and this one. But I much prefer to do this in three D modeling. It gives us more flexibility and an easier way to edit, as well. So let's finish the sketch there. A E on the keyboard extrude. In terms of profile, we're going to select this one here on the home view, input a distance there. As per the drawing, it's 16 mill Enter. Nice, let's get these fillets in here then. Let's come a modification tool. Let's go and fill it. Select this line, this line, and this line. These are constant fillets at four mil radius, into four there. Press okay. That's looking nice. And now let's focus on this wall at the back here. Again, there are different ways to do this, but I'm going to hit C on the keyboard. I'm going to do this on this face here. Press R on the keyboard. We'll start the origin again. We've got a wi there of 16 mil. I'm going to bring that up and snap onto this line here. It's fully constrained. Finish that sketch. It's head extrude, let's extrude that profile, and that comes up by 64 -16. So that's 48. Just enter. We've now got this Shamfa on this corner here. We want the modification, on Shampa. We want the type to be a two distance Shafer, so make sure we're under two distance. Select this edge here. In terms of this dimension. I want this one to be 20 mil, press tab on the keyboard, and the vertical is 30 mill. Okay. We've then got this slot feature in here. So I'm actually going to draw this on this plane. It's C on the keyboard, press space here. Press R on the keyboard, let's draw in this rectangle. I'm just going to draw it roughly here and then position it later. In terms of the width, we've got the same width as the champs, let's say, 16. I tab on the keyboard. Then we've got a dimension there ten mil center, and now we just need to position this. But to do this, I'm going to use the coincident constraint. I'm going to select the center point of this line, hold down shift on the keyboard. I like the center point of this line here. Then want to do exactly the same for this line. Hold down shift. I like that midpoint there. Good. Let's finish that sketch. E on the keyboard. Going to select this profile. We're going to enter a distance of minus because we want to cut the depth of 2.5. It's okay. Looking good. Let's go ahead now and add these hole features to this face here. There are two holes. So within a toll tool, we need to use points to identify the location of those two holes. So we need to do a sketch for that. It's C on the keyboard, select this face here. Come under the creation tools, select points. Going to throw in two points anywhere for now and dimension these I mentioned the first one from the top horizontal, we've got ten mil. And then that's align that with a vertical constraint. So from this point, go down shift on the keyboard, select the midpoint of this line. It's now fully constrained. You need to do the same here. So let's continue in the vertical constraint, select this one and this one, hit D on the keyboard, and then this one from this top horizontal line is 34 miles enter. That's now fully constrained. Got our red padlock. Finish the sketch there. Got our two points here. We don't need this one, but that's okay. Come over to the creation tools. Going to sect the whole command. And in terms of placement, we don't want a single hall. We want multiple. But now we need to select the sketch points one, two, Looking quite interesting in a preview. These hole there specify a two holes, ten mil diameter of the countersunk and 90 degree countersunk. So I want to make sure that we're under the countersunk holes. Make sure they're tapped, fully threaded, and the depth there is 25. The diameter of the counter sunk as per the drawing is ten. There are 90 degrees in there. And in terms of size, we're going for M five by 0.8. So make sure we got five meal selected here. And under the designation, make sure we got the thread pitch, 0.8 selected, six H right hand. Okay. Looking good. Let's now rotate the part and get this other feature in. It's C on the keyboard, go to select this face here. Use the rectangle tool for this. Let's start at this corner point. Going to bring that out. That has a width of 56 -16, so that's 40 and a total height of 42 -16. Just a quick tip, by the way, we can actually enter 42 -16, let's enter, and it will pre calculate that for you. We've now got this arc in here. I'm going to use the circle tool for that, hit C on the keyboard. Start from the midpoint of this line here to snap on. That has a diameter of well, it's got a rad of 12. So a diameter of 24 press enter. Okay? And this is the profile here we want to extrude. Finish that sketch. E on the keyboard, select this profile. W that to be in a distance, but in this case, we want it to be minus. That's minus. We got 56 -16. So again, that's 40 press enter. We're back on the home view. That's looking good. Now we've got some text up here. It's C on the keyboard, select this face. Go to the creation tools, select text. In this case, we want the text on path, and our path is this line here. Select that.En through our text Fusion 2025. I'm going to leave font aserial. If that is not bald, height five, okay? Placement above the line. We don't want it under. We're not too concerned about fit to path. Let's press Okay. Finish the sketch there. Come under the creation tools. We'll go on Ibo. We will select that text feature there or we can select sketch six. In terms of faces, so we want to reference from this face here, go on the home view, do them in a bit. We want this to be an Ibo, not a DBs, the depth we want. If we change that 0.5, Enter. Okay. Go to decal on this face. Let's go under Insert, elect Decal. I'm going to take this from my project, and I will include this as a downloadable resource, so feel free to download this part if you'd like, or you can use any decal that you have. Select Insert. My face, select this one here. Go back on the sorry, the right view. Want to rotate that by 90 degrees, or in this case, sorry 270, reposition that, scale that up slightly. Leave that there. That looks good. Press okay on the home view. Everything there is looking nice. We just need to add in this rib feature here. To rotate the part, C on the keyboard, this face, L on the keyboard. This endpoint to this endpoint, and then we've got our profile there in blue. So we turn profile off, white color profile on, we see the blue color. So a complete profile there on finished sketch, E on the keyboard, like that profile. Blue arrow is going this direction, so that's the positive. You want to go negative in this case. And we're going negative 12 on the home view. And then we just need to input the fillets down here. Get on the modification tools, hit Fillet. I want this to be a constant fillet on this edge, this one, this guy and this guy. Under the fillet size, the drawing states two mill. Okay. And there we have the completed model. That's looking nice. The only final touch we could do is just to change the color of this text. Recommend we do now. Let's hit A on the keyboard, change the appearance. In this case, I want to change the appearance of faces only. And I'm going to drag select across these faces. I don't want to select this face or this one or this one. So left click on each one of those. And then I'm just going to choose. Let's go for a paint under a glossy paint. I'm going to go for enamel glossy red. Drop that on Yep, close on the home view. And there we have the completed part. I think that's looking quite nice. I hope that you were able to do that yourselves. If you were fantastic news, World unto you. And again, if you do have any questions either about the sketching or the modeling, the tools that I'm using, please do send me a message. I'll reply as soon as I can. Aside from that, I will see you in the next assignment. 46. Modelling Assignment 2: This is your second three D modeling assignment. But the first thing to do here is to review the geometry of the part and determine which is the most suitable three D modeling tool to complete the main body. The dimensions of this part are shown in the three D technical drawing here. This is displayed in third angle projection, and it helps you to visualize and understand each feature's geometry. So during this lecture, I will demonstrate a method and selection of tools to model this part. It is recommended to pause the lecture here and attempt modeling this part yourself, and then once completed, you can continue watching the video to see one modeling method, which I will demonstrate. So if you could pause the video here and have it go at modeling this part yourself. Okay, welcome back. I hope you got along well with modeling this part. And now I will give a demonstration of one way in which we can model this part here. So, let's go on create new sketch, and I'm going to sketch this on the XZ plane. I'm going to use the revolve tool for this. We could do this using the extrusion tool, but it'll be much more time consuming and easier to edit and sketch using the revolve tool. So let's start off with a line tool then, and I'm going to draw in our revolution line. Make that let's say 100 mil for now. Got a construction line. Good. Move that dimension out the way, turn off construction line, hit L on the keyboard again. I'm going to roughly draw in this geometry. I'm not going to dimension it up for the time being and fine tune it a bit later. If we come across, we come up, come back to the right, go up across down, and then we coming in a bit of a recess, we're going down again. So let's constrain and dimension this part here. First of all, this line needs to be vertical, so use the vertical constraint. Apply that. That's now vertical. I need a horizontal constraint between the origin and this point here. Horizontal constraint, this point, origin. Now I'm going to start dimensioning. So let's dimension this point here from the origin. And as for the drawing, we can see that we've got a 50 mill inner diameter below that recess. We need to divide that by two, but in 25. And then from the outer point here to the center point here, we have a dimension of 200/2, so 100 mil. We've got a wall height here of ten mil. Put that in ten mil. We've got a distance from this line to the origin, and that is 100/2, so 50. Then we can do this line to the origin, which is 58/2, so 29. And then we need to assign a length here. So this vertical line is 50 minus ten, so that's 40, and then the same for this line here. So this line is 30 mil. Okay, that should be fully constrained. If we open up our sketches, yet, we see the padlock there fully constrained and ready to revolve. We can finish the sketch there. We're back on the home view. Come up to the revolve tool, select that. Fusion has selected the profile already. It's the only one available. We just need now to identify the axis. I use the construction line here. Okay, previews looking good. We've got our recess in there looking nice. Let's press okay. One thing we could have done in a sketch is to implement the Shamps on this edge, this edge, and this edge, I much prefer to do this in three D modeling mode as opposed to two D sketching. Let's come up to the modification tools, go and Shampa. And here we've got all Shamfs are four mil by 45 degrees, so they are equal distance shafs. I'm going to select this edge here, this edge. And this edge going to input here four mil. Okay. Looking nice. And now the only two features left are the series of counterbar holes around this face, and then the series of simple threaded holes around this face. Let's do the counterblls first then. Hit C on the keyboard, select this face. And for these countable holes, we've got a total of 12. So we need to input our points in a pitch circle diameter, 12 of those, which will then use the whole tool in three D modeling tools. So let's start with a circle tool then and I'm going to input a construction line going to be a circle, in fact, and that's going to be our pitch circle diameter. So we've got 150 mil there, we know that our 12 circles are distance equally around this PCD pitch circle diameter. I'm going to move that dimension slightly. Let's go ahead and add a point, then. It's coming to create at a point. I'm going to snap that on, so it's coincident with the PCD. They're going to use the vertical constraint from the point to the origin. Now that's fully constrained, can't move anywhere. Now come under create you're on the circular pattern, and we are going to circular pattern this point around the center point, which is the origin. And in terms of instances for the quantity, we have a total of 12 holes. Okay, preview looks good. Let's press okay. But this is the center point of all the holes we'll make. Finish the sketch there. Come over to the hole tool. In terms of placement. So we've got multi holes. We'll select that. Need to identify our sketch points. Let's go for these four. Sorry, these five, these five, and these two So we've selected our 12 holes. These are countable, so I'm going to select countable and they are threaded. They've got eight thread. Make sure that is selected. They're fully threaded and drill point with an angle. We can't go for flat actually because they're through holes, so it doesn't matter which one. So depth, yeah, well, that's through so we could leave it as 25, but we're actually going to go with the thickness of this plate here, which is ten mil. Then the counterbll diameter as per the drawing is 14 mill, so leave that as 14, and the depth of the counterbll is four. And then as we come down, we need size. So yeah, we size eight M eight, make sure we got eight selected. Make sure the designation is correct. So 1.25 mil pitch thread. Okay, six H right hand. Okay, let's look at the preview then. Looking nice. Okay. Select okay. There we have our 12 counterbll holes. One more feature to add then, which is exactly the same process for this face here. But these are simple threaded holes. Press C on the keyboard, select this face. Press C on the keyboard again for the circle tool, start at the origin. This has a PCD, pitch circle diameter, 75 mil plus Enter. Going to select that circle at a construction line. Move that dimension. To create put in a point, snap that to the PCD, same process, vertical to the origin. Come on the create circular pattern, point there. Center point the origin here. In total, here, we've got six holes as per the drawing. But our six points there. Okay? Finish the sketch. Come on to the whole tool. Again, we're going to choose placement multi holes. Choose our points. Let's go for these three and these three. These are simple holes the whole type. We want simple. They do have an assigned distance here, which is 25 mil deep, okay? They are tapped. They've got an Might by a 1.25 mil pitch thread, holds to be fully threaded, and the drill point, in this case, will go in an angle. Let's put the depth in here, then. We've got 25 mill. We'll come down to the bottom, make sure we've got eight mill selected, the correct designations, a 1.25 mil pitch thread, six H right hand. That will look at the preview. Looking good. Coming down 25 mil, okay? And there we have our completed part. That's looking good, but I just want to do an inspection on that, do a section analysis, and let's do our section analysis on the plane. Just go to flip that direction. Everything here is looking good. Okay, that's looking fine. Our shamps in there, counter boors. 25 mil simple threaded holes. Yeah, yeah, that's looking good to me. Okay, go to select right there. Back to the home view. I'll turn off that section analysis. That's one way in which we can model this part. Again, it could be done with the extrusion tool, but much more efficient and easier to control with the revolve tool. I hope you got along well with that assignment. And again, any questions, please send me a message. I'll reply as soon as I can. And aside from that, I will see you in the next assignment. 47. Modelling Assignment 3: This is your third three D modeling assignment. This is a plastic injection molded housing consisting of quite a few features and a threaded simple hole in the center. The dimensions for this part are shown in the three D technical drawing here. They're displayed in third angle projection to help you visualize and understand each feature's geometry. During the lecture, I will demonstrate a method and selection of tools to model this part. So at this point, it is recommended to pause the lecture here and attempt modeling this part yourself. And then once completed, you can continue watching the video to see one modeling method as I will demonstrate. Okay, welcome back. I hope you got along well with that part. And so from this point in, I will demonstrate how I would typically model this part. So let's hit C on the keyboard, start a new sketch. We're going to do this on the XY plane. Start with the rectangle tool press R on the keyboard, start with the origin. Going to come across 160. We're going to come across 160 on the height as well. So that's the footprint there. Let's go ahead and finish that sketch, then it E on the keyboard. We're going to extrude that one profile there. And that's a height of 40 mil plus Enter. And we can see this is then shelled out. So an option here is for us to shell out this box and then add in the remaining features. So the housing wall thickness is four mill. So let's come up to modify. Let's hit the shell tool. We're going to select this face here. We want to remove it. And in terms of the wall thickness, we're going to go four mill. It's okay. Now we've got our shelled box. It's looking good. Et's now go ahead and start adding some features to this. So I'm going to hit C on the keyboard, create sketch. We can do this either on this face here, in this case, I'm going to choose this face, either one or two. Let's start off with the corner feature here. So we've got a hole there with a diameter of ten, and that's got a wall around it, that's got a radius of 20 mil, and then that leans into four milradite edges, which goes into the thickness of the wall. Let's hit C on the keyboard, put it in the circle, give that a diameter of ten. Going to dimension that. In this case, from the origin, 14 mil. And again, we're going to dimension that on the horizontal, I get in 14 mill. I select 14. I've just clicked that dimension there, so it's referencing D seven. I've got that link in there. From here, we've got an arc with a 20 mill radius. I'm going to draw that in as a circle. We can delete any part of that circle we don't need. So put in a diameter there are 40. That's looking good, and then that's one profile here for us to extrude. Then in terms of the radii, which are around these edges here and here, we can add those in later. Let's move to the center then. Hit C on the keyboard. Let's go for a circle. We've got a 30 mill diameter circle there. We've got a hole in the center. We're going to go I'm going to do this a different way. Instead of using the hole tool, I'm just going to add in a hole by means of using an extrusion and then add a thread to that later. But if you want to go for a point, you can do, no problem. I'll put an 18 mill there. Dimension this from the outer wall. That's a dimension of 80, and then dimension this from the top horizontal. That's also 80, so that's centered. Everything's in black. Everything should be fully constrained. We've got our red padlock there. That's looking good. Let's come over to this feature up here. So there's a wall that protrudes out with two holes in. Let's go on the line tool. I'll start at the edge here, come across down, join that back. Put in some dimensions. The thickness here we've got, actually, we're referencing to reference that dimension from this line to this outer edge, 34 mill we've got a height of that of 15 mil. And then from this line here to the outer horizontal edge, we've got 20 mil. Just need to input the circles at the circle tool, add in the two circles there, make sure they're constrained horizontally, one, two, is good. I want to make sure there's a horizontal constraint with the midpoint of this line and the center point of these two circles. I've selected this center point here, hold down shift on the keyboard, and then we'll select the midpoint of this line here. You'll see they will move accordingly. We just need to dimension those. So this circle here from this outer wall as per the drawing, 12 mill, and then this one is 27. Let's put it in a diameter, hit D on the keyboard, but in the diameter, one of these circles is six mill. Then I'm going to put a equal constraint, and I'm going to select this circle and this one here. Now they are both locked equally. So both six mill both are constrained fully as they're dimensioned. And that feature there we can leave as is, and we've got our profile to extrude there. I'm drawing on the top lane, as we can see, we've got one profile, two profile, and three profiles ready to extrude down to this face. And so the last feature to add is the slightly complex one down in this corner. I'm going to go ahead and use the line tool and roughly drawing this geometry. Come across down, cross and down. Dimension this up. Line here going to reference from the outer edge there. So that's 34 mil. Dimension the height of this 115 mil. Height of this one as per the drawing 38 mil. Then we've got a distance from this line here to the outer edge. That is 50 mil. Okay, all black color looking good. Let's go ahead now and add the we've got a hole here, so I press C on the keyboard, bring that out diameter six. You can dimension that from the outer wall 19 mill. And then we've got a dimension here to this wall here. That is eight mill. Okay, that's fully constrained now. Then last, kind of hit R on the keyboard, and I'm going to draw in two point rectangle, dimension that. Width, we've got 30 and height, we've got 20. And in terms of positioning, we've got this line here to the outer edge, which is ten mil. And then one more dimension from down here, which is 12 mill. Looking good? Okay. So all of the radii, all the fillets. I'll be adding them after we do our extrusion here. So we're going to make sure that's fully constrained yet, got the red padlock. That's looking good. Finish the sketch there. Jump into solid, E on the keyboard and select the profiles to extrude. So we're going to choose this one, this one, this one, and this one. In terms of direction, we on them going up. We want them going down. But in this case, I'm actually going to choose the extent type to be two object, and then my object to select, I'm going to choose this object here or rather this face. Click once. You can see all the extrusions will go down to that face. We can do join or a new body. In this case, I'm going to do join. It's all plastic molded as one part, but it's okay. A few more features to add here. Let's go ahead and add this thread. Let's come under Create. Come under the thread command. We're going to select this face here. And in our toolbox, it's already recognized the diameter there is 18 mil. Press that okay. Happy with. And then we just need to add the fillets. Let's go and modify, choose the Philip tool. I'm going to select this face, so all of these edges in contact with this face will be filleted by, in this case, four mill. There are also a few more. So this one here, just speed up the video and go through these. Okay. I think that's just about everything. We'll click Okay there. Let's see how that looks. That is looking good, and that is the completed part. I hope everything made sense there, and if you were able to do this yourself, a big well done a good job for recognizing to use the shell command here. That's a nice shortcut. Any questions? Again, please send them to me. I'll reply as soon as I can. Aside from that, I will see you in the next lecture. 48. Creating Assemblies Introduction: In this section, we'll learn how to form assemblies of multiple parts with infusion. To start with, we will mold each individual part of a Pulley assembly and then bring these into a single design file and form the appropriate joint types for this assembly. We'll also learn how to take advantage of the built in Autodesk contents library, which offers us an array of pre built parts that we can customize to suit our needs. In addition, we'll learn how to manipulate part visibility and opacity, how to use pattern tools when working with assemblies, and much more. Just like in previous sections, each lecture in this section is presented step by step, and I will walk you through and demonstrate how we can generate assemblies using Fusion's joint command. I'll be giving a range of examples throughout the lectures, which I recommend you follow along with me and take the opportunity to practice these tools and familiarize yourself with what they are used for. So, let's start creating assemblies. 49. Baseplate: So the very first part of our assembly that we're going to model together is the base plate. So let's jump into fusion, and I recommend, at this point, hitting save at the top. And then under the location, let's hit the drop down. Let's come into our fusion course project. Then I suggest creating a new folder there and calling that pulley project or creating assemblies. In this case, I've already created the folder here, creating assemblies, and I've got all my various parts in there. So once you've created a new folder, name this appropriately, let's call it. Base plate. Fully assembly, then hit Save. And now let's begin to model this. This is the drawing of the part, third angle projection, with all our dimensions there. If you would like to model this part by yourself, by all means, please do so. And now it will be a good opportunity to pause the video and have it go at modeling this. But aside from that, throughout the remainder of this lecture, I will be showing you how I would typically model this part. So let's begin and come up to create a new two D sketch. Let's do this on the XY plane. That's the orientation we want this part to be in, considering the full assembly. But let's select that plane. Let's hit R on the keyboard, rectangle, start of the origin, drag that out. We'll do a WI there 100 as per the drawing. Press tap on the keyboard, and we'll do a height there of 50. Press Enter. Let's go ahead and add these whole features then. Hit C on the keyboard, begin to draw a circle anywhere for the time being. That's got a diameter of eight enter. D on the keyboard, dimension between the circle, this line here. That's ten in the drawing and circle to this top horizontal line there is also ten. And then going to draw in some mirror lines. So I'm going to start at the midpoint of this line so we can see the indicator just there. Make sure that's construction line first, and then draw that down to snap onto the midpoint of this line, exactly the same process starting midpoint on the vertical line to the midpoint of this vertical line. Ahead and use the mirror tool. I like the geometry to mirror, the mirror line, select this center line here. Press o. Select the mirror tool again. Rags like the first circle, second one, as well. Mirror line, this one here, press o. That's looking good. Now, we could add the radii on the corners there. So we've got this eight mill radii on each corner. But I'm going to be doing that using a three D modeling fillet tool. Again, I much prefer to do this in three D modeling as opposed to sketching. Let's go on finish sketch. The E on the keyboard extrude. I'm going to select this profile here. On the home view. I'm going to extrude that by a distance. As per the drawing is ten mil. Enter looking nice. Go ahead and add these fillets in. Select the filllet tool. Drag select around this edge here, this one, this one, and this one. Back to the home view. This is a constant radius fillet. So no need to make any changes, leave everything as default. The eight mile fillets there. Press Enter. Okay, that's looking good. Alright, so the last part we need to do is just to remove material. So I've got some material being removed here, here, then on the underside, as well. So the best plane to sketch on is this plane here. Hit C on the keyboard. Gonna select this face. And then we're going to model in some rectangles and remove that material. So if we hit R on the keyboard, we'll notice that we can't snap to this corner point here. That's because it's not actually in this plane. If we look, it's offset from the plane. That's absolutely fine. What we're going to do there is project. So let's come under the creation tools. Let's go now to project, choose project here or P on the keyboard, and we're just going to project this point here, also this point here with our two points selected, our toolbox there, where then going to click Okay, and now they are projected onto the plane that we're modeling on. Go back to that face front face. That are on the keyboard then, and we start from our projected point. We're going to come across there by 30 mil as per the drawing, tab on the keyboard. We've got a depth there of two mil. Press Enter, one rectangle. Let's get the other one in there. So starting from the other projection point, 30 tab, two, enter, and good. Then rectangle going to snap on here. Take that across. We've got 70 -30, that's 40. Depth there is also two. Press Enter. Now I need to position this. So to do this, I'm going to use the horizontal constraint. Going to hold shift on the keyboard, snap on to the center point of this line, hold shift on the keyboard, then snap on to the center point of this line here, which is here. Enter. Sorry, left click. Okay, that's all fully constrained. Got the red padlock there. That's looking good. Finish the sketch. Let's go on solid, go on extrude. And there are profiles. Let's select these two, these two, and this one here. We want this to be a cutting operation. Let's go cut, move that in the correct direction. And these cuts are through all. So in terms of the extent type, we're going to click on here, and then we're going to select A. It's okay? Let's look at that from the front view. Yeah, that's looking nice. Can finish that off by applying an appearance. A on the keyboard. We want this to be applied to the whole body, so we'll keep that selected. Right now, we've got the steel satin finish. Let's change that then. Let's go for quite like the one of the metals. And this is just an appearance. This is not we're actually applying physical properties here. I quite like the aluminum anodized rough blue. So rag that up, replace the existing appearance, close that on the home view again. And there we have our completed part. So that is the base plate, and now we can move on to drawing the remainder of the components prior to building our assembly. So I'll see you in the next lecture. 50. Bracket Arms: Let's move on now to the second part, which is the bracket arms. On the screen now, I'm showing the dimensions of the part. So if you would like to model this yourself, please feel free to do so. Aside from that, for the remainder of this lecture, I will model this part myself. So let's jump into fusion, and let's go ahead and save this file. Make sure we save it in the same location as the first part we did the base plate. I'm going to call this racket arms pulley. Look save. Now let's begin modeling. But let's start off with the footprint of this part. Let's go and create sketch. Best plane to choose here is the XY plane. That's for the correct orientation. R on the keyboard. We're drawing a rectangle. Now we've got dimensions of 50 by 30. Press Enter. Let's go ahead and draw in these circle features then. Hit C on the keyboard. Is diameter of eight mil, plus D on the keyboard, dimension that from this line here, it's ten mil. And again, from the horizontal lower line ten mil. We can go ahead and mirror that on the other side, plus L on the keyboard. Or a construction line down to the midpoint of this line. Go to mirror, drag select the circle, mirror construction line. Okay. Again, we could put in the radii here, but we're going to do that in three D modeling mode using the Fillet tool. Finish the sketch, it E on the keyboard, select this profile. Let's extrude that by distance, in this case, as per the drawing eight mill. Now we can go ahead and input these fillets. Let's select this edge here, this one, they're constant fillets, they've got a radius of eight mil. Okay. That's looking good. So there we've got the footprint of the part. Now let's go ahead and draw in this vertical part which sits on here. To do that, I'm going to sketch on this plane here. C on the keyboard, select this plane. We go four. Let's go for the rectangle tool. The snap onto this line here. Let's come up. Let's got a width of 20 mill plus tab on the keyboard. Got a total height there of 58 mill. That's the rectangle, and then we're going to hit C on the keyboard. And from the center point of this line here, we're going to expand that out so we get that nice arc geometry at the top there. You can also draw in the through hole as well. So start that at the same center point, draw that out. That's got a diameter of eight mill as well. Now we need to position this. It's just kind of floating around. Let's go for the coincident constraint. I'll down shift on the keyboard, select this midpoint. I'll down shift. And if we can find it, select that midpoint there. Good. Finish that sketch then, hit E on the keyboard, let's choose the profiles we want to extrude, which are this one, this one, and this one. We want them going in this direction, minus, in this case, no minus eight mill as per the drawing. Okay. Looking good. Got these fillets to add on on this edge. And this one here, go on the Fillet tool, select these two edges. They constant fillet, and the radius is 15 mil. Press Enter. Okay, that's looking nice. And now just one last feature to add, which is the rib down here to do that, let's go for a construction plane. Choose a mid plane, house this face we choose this face. Get our new plane input there. Press Okay. Let's sketch on this plane then, hit C on the keyboard, select this plane. I'm going to press L on the keyboard. I want to snap to this point here, which I can't do, so I'm going to press P on the keyboard, projection. Project this point here. That's okay. You see our projection point there. Let's go back on that plane then. Go under construction. Plane one, create sketch. G that from the right view. Press L for line two, start at the projected point, draw that up. But then in randomly there. We need to project some more geometry here so that we can dimension between this line and this line here. Press P on the keyboard, select these two lines, go to select this one as well. And this one okay. And now see we have those lines projected onto the plane we're sketching. Go back to the right plane then. A coincident constraint I point this line to this line here. Let's hit D on the keyboard and put in an angle from this line here to this line here. That angle as per the drawing is 60. Okay, that's looking good. Go ahead and finish that sketch then. Go and extrude. Profiles already selected for us. Now we want to go in both directions. So under direction, we'll go two sides, and then we've got a total width of six. That'll be three inside one and then three inside two. We press Okay. Have a look at that. That's looking good. And that's all other features for this bracket. Let's just wrap this up then by applying an appearance. So let's it A on the keyboard. Bring that over here. In terms of appearance, I'm actually going to choose a paint in this case. I'm gonna chooe a glossy paint. Gonna go for enamel glossy red. Drop that on the existing appearance, close. There we have our completed bracket. Okay, so in the next lecture, we'll be modeling the pin, and then finally, we'll be doing the pulley itself. And so I will see you in the next lecture. 51. Pin: Let's move on now to the third part, which is the pin for our pulley. These are the dimensions for the part here. So if you would like to model these yourself, please feel free to do so. But aside from that, I will now model this part myself. So let's jump into fusion, and first of all, let's save this design. Let's give this a name pin. We want to make sure that location is under our project folder that we've been working on so far. Looks save let's go ahead and model this. So there are different ways to construct this part. The most efficient way would be to use the revolve tool. I would just simply draw a profile, a revolution axis, then revolve around that axis. So let's go create sketch, and we're going to do this on the Y Z plane as per the orientation of the assembly. And different ways to start this sketch, Let's start with the Let's go for a center point arc. Let's start from the origin. Let's come out. So we get a radius of seven there, okay? Make sure that's coming out. Like, so, bring that around 90 degrees. Going to use the horizontal constraint on this line here. Make sure that's horizontal. Move that radius out the way. Use the line tool then, start at the end point of our arc, and we're going to come down. So we've got seven, and that's four. So that's three. Okay, down. Click on. Then we're going to draw out another line, which is 8.5 then from here, we're coming up. We've got 20 there. That'll be ten from there. So I'm just going to draw in this roughly like so. Now let's use the dimension tool. So from here to the center point, let's put the drawing. We've got that dimension available there. 20/2, that's ten. In terms of the width, we've got 12.5 -8.5, so that's four. And then I'm going to dimension from the origin to this endpoint here. It's going to be 56/2. Press Enter. And we just want to make this line here collinear with this one because right now, this one can move up and down. Let's go for a collinear constraint between these two. Everything there should be fully constrained. We've got our red padlock, okay. Next, I'm going to use the line tool. I'm going to draw in a construction line down. And so the idea here, I'm sure you recognize already is to mirror this across and then we'll draw in our line of revolution, and then we'll go and use the revolt tool. Let's use the mirror tool. We go to select all of this. Then use the mirror line. Be the construction line here, press ok. And finally, I just want to use a line, not a construction line. We need to complete a profile here. I go to start from the endpoint of this arc and finish at the endpoint of this arc. And now we'll see this is shaded blue indicating a profile that's ready for us to use. Finish the sketch there. Go on solid tours, go on revolve. The fusions automatically selected, the only profile available. In terms of axis, you want to select this one here. We a preview of the part. Want to go the full 360. We're not looking for 270 or minus 270. Let's go 360. And then let's look Okay. And there we have our pin. Let's go ahead and assign an appearance to that. Here you on the keyboard. And for this one, I'm going to go with enamur glossy black, replace the current appearance, close, and just go to hit Save on that. Okay. And there we have our pin. If you were able to model that yourself, yeah, fantastic. Big, well done. But otherwise, I hope you were able to follow along with how I modeled this part. And I look forward to seeing you. In the next lecture, we'll model the pulley. 52. Pulley Wheel: So that leads us on to our final part, the Pulley wheel. These are the dimensions of the part here. But if you would like to model this yourself, please feel free to do so. Aside from that, I will now have a go at modeling this part myself. So let's jump into fusion, and first of all, let's click Save. Let's title this Pulley wheel. And make sure it's in the correct location under our project folder, hit Save. Let's start a sketch. And we're going to do this on the same plane that we drew the pin on. That's the correct orientation. That's the Y Z plane. Select that one. And from here, the first thing I'm going to do is put in a construction line, and this is going to be our axis of revolution. So just like the pin, we're going to revolve this part. We're just going to draw a profile and revolve that around the line I'm about to draw in now. In that to be a construction line. I go to put in a dimension there of 40 mil over that dimension down there, and the construction lines off. Alright, let's book from the top because that's quite easy then. So we've got a rectangle up here, it's got a width of 20 and a thickness of three. Put that in the right position. So I'm going to constrain that vertically to the origin, and I'm going to put in a dimension there from the top corner point to the origin. And as for the drawing, that's 30 mill. Looking good. Let's continue with the rectangle tool then. Going to snap on anywhere on this line now. But in the width here, which is two mill and the length here, which is 18 minus three, that's 15. Okay. And now we can only move it across like this. Let's go ahead, and let's put in a horizontal constraint. The center point of this line, hold down shift, select that. There we go. And I want to constrain it horizontally with the midpoint, sorry, of this line. So everything there should be fully constrained. I've got a red padlock, ok? Good so far. Move that dimension out the way. Then from here, let's use the line tool. I'm going to start from this corner point. I go to come down here roughly. I'm just going to put in the rough geometries like so, something like that, and then we'll tidy those up. So let's go with the vertical constraint. I go to select this point to this point. Gonna go ahead and dimension from this point to here. In the drawing, we're given that dimension as 24. And then this point is a top corner point. We're giving that dimension as 26. Okay, looking good. I want to put in an equal constraint between this line and this line here. They are the same height, and we just need to put in a vertical constraint between the origin and this point here, and there we have our profile. One more detail to add. That is the arc down here. So to do that, go to use the circle tool, press C on the keyboard, snap to the midpoint of that line. I'm going to bring that out by a radius of one, so diameter of two. It's good. So we've got one profile here, one here and one here. That's fully constrained. We've got our axis of revolution here. Let's finish the sketch. We over the solid, hit the revolve tool. Then from here, select our profiles, so one, two, three. Okay, we just want those three. And the axis, let's select our construction line here. Let's just have a quick look at that preview. That's looking good. That's what we're after, okay? Nice. All 360 degrees direction one side, and operation new body. Okay. Okay, just one more feature to add, which is the holes around this face here. Let's press C on the keyboard. We're going to select this face here to draw those holes on. Start with the circle tool, and let's input the pitch circle diameter, which we're giving in the drawing as 41 mil. I'm going to make that a construction line. Okay, click once. Turn off the construction line. Now we'll stay in the circle tool. I'm going to draw in a circle here with a diameter of three mil. They want to use the vertical constraint, center point of the circle to the origin. That's now fully constrained. Now we can go into the create tools, circular pattern, drag around our circles, and the center point, that would be the origin quantity. We've got three plus three. That's six. Okay, that's looking good. Let's finish the sketch there. Come into solid, extrude. Profiles. Let's select these three, and these three. There needs to be a cutting operation. So I'm going to move the arrow across. But in terms of the distance, I'm just going to select all. Now I'll cut only the material in that extrusion's direction. The preview looks good. Let's press Okay. There we have our completed pulley wheel. Go ahead and add an appearance to that. Here on the keyboard. And this one, I'm going to go I'm gonna go for a paint glossy enamel glossy green. Brag that over the existing one, replace that. Then we have our complete part. Yep, I hope that was okay. You were able to follow along okay. And again, if you do that yourself, a big well done. And now we're about to move on to assembling these parts together. So I'll see you in the next lecture. 53. Placing & Positioning Parts: Okay, so we have modeled each of our individual components, and our final goal is to create a full assembly here and also input the fasteners from the fusion parts library. So let's go ahead and start to make our assembly. So to do this, let's come up to the top. Let's go on a new design. And it's within this new design that we are going to insert each of the individual components. We're going to constrain these using joints infusion, and then our assembly will be complete. And so the process of forming an assembly infusion is considerably different from traditional CAT softwares, such as Autodesk inventor, solid works, Semen Xenx. In these traditional programs, we create a dedicated assembly file and then draw in the individual part files that we drew previously, whereas in fusion, we form an assembly within a design file where each of those components have a link to their associated design files. So with our new design open, let's come up to the top left, and we're going to hit Show data panel. And then within the data panel, you need to locate under your projects the And then within the data panel, you need to locate within your projects the four parts that we previously drew. So mine are in home fusion course project. I've got a folder called creating assemblies, and then under Assembly tutorial, I've got the past four parts that we've drawn. So let's start by inserting one of these. Let's go for the base plate. To do this, we right click, and then we select insert into current design. Left click one. Another part is brought into this design, and straightaway, we have the option to move this. So this is relative to the X Y and Z axis in this environment. We can move it in any direction xa. We also have the ability to rotate it, and we can control all of these parameters with the toolbox here. We've also got the circle in the center, so that's a free move, and then we've got three individual squares here, and they relate to just moving under two axis. So, for example, this one here is the X z. This one here is the Y Z, this one here is the XY. Let's go back on the home view then, and let's rotate this part by 90 degrees in this direction here. By happy with that orientation, go to press Okay. Our first part insert. And then if we come over to our browser, we'll then see that we only have one design in here or one part, it is the base plate. And we see we've got this chain symbol here, and this represents a link to the original file, which is here. And at this point, it would be a good idea to save this file. So let's click Save. I'm going to type this Bully assembly, and that is the correct location. Make sure the projects correct. Click Save. And then we should see that appear in the data panel here as we see it. It's just popped up there and it's just uploading that data. Let's continue with our assembly then. Let's inputs and more parts. Let's go for the bracket arms, go to right click insert into current design. And I'm just going to roughly position these. So you could accurately position them, but I want to show you how to use joints, and so I'm just going to roughly throw them into place, okay? Something like that. That's good for now. Happy with that position. Let's press Okay. Let's do exactly the same. We want the other side. Again, I'm going to use these arrows down here, move this into position, move that up. Rotate that 180. Like so. Okay. Let's go ahead and put the pin in, right click insert. Roughly position this. Let's go on the right view, move that arrow up. Okay? That's right. And the same for the wheel. So right click, insert into current design. Again, going to go on the right view for this one. Roughly position this. Okay. Go back to the home view. And then if we want to readjust any of these, it's very simple. We just hold down the left mouse button and we can drag and move that around. Now, some students have advised me that they are unable to do so. No problems at all. We come up to our tools at the top and we come under these selection tools, hit the drop down. And you'll see here there's a checkbox for component drag. And with that turn on, we can freely drag items. If I have it turned off, we're unable to freely drag unless we hold down Alt on the keyboard. I I hold down Alt, I can then move these parts around, but without Alt held down, I'm unable to move this part. I would always recommend keeping comona drag on. Personally, it's just easier for moving things around. Now, there's one item here, which is the base plate that we are unable to move. So I'm holding down the left mouse butter now, but I'm unable to move this part. However, all the others I can. And so this has formed a relationship with this particular design, and it's what we call ground to parent. Okay? So if we come up to our browser and then we go another base plate, we'll see there's this anchor symbol next to the part, and that indicates that it's a ground part. So if we right click on this, we've got the option here, unground from parent. So the parent, in this case, is referring to this particular design file. So it's referring to the origin, the X Y and Z. This part is ground to that data and so we are unable to move it. But we can right click on it, unground it, and then we have the free option to move that. I'm going to keep that ground for the time being. I like to have the first part grounded, and that's what we do in traditional CAD software because then every other part, as we form the constraints or the joints infusion with this part, it's then all related, and everything is fixed in position, so we can be ensured that all the relationships that we want are in place. Just another tip for moving parts. If we did want to move ap precisely, we can come over to the browser. Let's say we wanted to move this part precisely. We can right click on that part and then select move copy or Shorku M on the keyboard, and then we've got our arrows and our wheels. We can adjust that how we need, like so. We can use the parameters in the box here to control that. Okay, so that's how we place parts inside a design file and roughly position them. And then in the next lecture, we'll begin to use joints where we'll form constraints and relationships between each individual part. So I look forward to seeing you there. 54. Using Joints in Fusion: So now that we've input each of our parts into this design file, it's now time to give these parts relationships and complete the assembly. So in traditional CAT softwares, we would use what's called constraints. So, for example, in Autodesk inventor or solid works, we would use a series of constraints to align parts and fully constrain those parts together until we've got a complete assembly. A fusion works quite differently and uses what's called joints. Joints and fusion are quite a simple method of joining parts together, and it's actually very efficient to use. Joints are located under the assembly category here. We've got the outron here for joint or it's the shortcut J on the keyboard. To begin with, I'm going to remove the data panel, so I'm going to click the X up there. We no longer need that. I'm going to press J on the keyboard. And as a demonstration, the first two parts that I join are this bracket arm here and our base plate. So this bracket arm is going to sit somewhere somewhere on top of there. Going to throw that there for now. I'll sit J on the keyboard, we've got a tour boox pop up. The process here is to select a joint on one part and then a corresponding joint on the other. For example, I'm going to move to the base of this bracket here, and as we hover the mouse over the face, we'll start to see all of these joining points appear. We can select one of these. The one in the very center is the most logical one to go for in this case. I'm going to select this joint here. Then if I rotate the part, come down to the base plate, I hover my mouse over this part here, the corresponding joint would be right here in the center. So if I left click there once, I'll then see the bracket arm move to that position, and then we can offset it. Where those two points are joining, we can then offset it in this direction or this one, and we can also rotate the angle as well. And you can control any of these parameters in these boxes here. And we press Okay. And that's looking good. And if we look at the top of our toolbox, we've got position and motion. If we go to motion, we can then select different types of motion. So rigid is essentially rigid, nothing moves. They got the option for revolute. So about that joint between the two parts, this bracket arm can revolve, so it can revolve around, in this case, the z axis. Also the option for slider and various other motions as well. But the majority of cases we're using rigid motion, okay? We will be using revolute for the pulley itself. We'll get onto that later. Make sure we got rigid selected, my position. I'm happy with that joint type, happy with the alignments. Everything there is good. Press Okay. Now, if we try to move the bracket arm, so we're unable to do so. Holding down the left mouse put and cannot move, the same with the base plate. But the base plate is grounded to the origin, and then the rigid joint between this bracket arm makes it unable to move. However, this bracket arm, we can still move. So let's put a joint in there, press J on the keyboard. I'm going to do this slightly differently. So instead of selecting this middle point here, actually going to choose the center point of this circle and just show you that this is another method. And in fact, there are many different joining points we could use. But just, for example, going to select this joining point here, and then the corresponding point would be the center of this hole here. Left click once there, see those two parts come together. Happy with the alignment. We don't need to rotate that or do any offsets. And in terms of motion, we want that to be rigid, as well. Like so that's good. It's okay. And out this part, we cannot move as well. Though good. We're getting there. And now we need to position our pin. Let's J on the keyboard. Again, a variety of ways in which we can do this. I'd say that the most simple way is to select the center point of this face here. So I've got my mouse over this face, and then go to move the mouse down I can select the center point there as we can see. So I'm going to left click once. Then the corresponding joint point will be over here as I move my mouse over this whole feature, I got the option to select this point here. Go left click. Okay, that's good. Reviews looking good. Everything there is fine. Click Okay. Come out nicely, again, that cannot move now. There's only one part left to join, which is our pulley wheel. So we're going to do this slightly differently. I'm gonna press J on the keyboard, and this time, instead of using the simple origin mode, we're going to use the between two faces. But let's select that. We're going to come across to our pulley wheel, and we're going to select this face here, and then we need to select a second face. We're going to choose the face on the other side. And then what we see is, we have this kind of like plane in the center there. Now, on that plane, there will be a series of points which we can snap onto. So as I move my mouse more towards the center, we can see at the very center there is a snapping point. I want to take that snapping point on the left click once. And in terms of our component two, we're going to do exactly the same. So between two faces, and this time, I'm going to refer to the pin, although we could refer to the bracket arms. But for the pin, I'm going to choose this face, and then I'm going to choose this face. And then under my selection point, as we bring the mouse to the middle, we'll see this sort of plane up here where we can select only one point here, a left click there once. Pulley wheel move into place. By the preview, that is looking good. Happy with that. But in terms of the motion, I don't want this to be a rigid motion. I would like to show the animation and have the ability for this pulley wheel to rotate about that pin. So under the type, I'm going to go ahead for revolute. And so about where that joint face is, we are rotating. So in this case, around the z axis. Now, we could change that and rotate around the X, but that's not exactly what we're after or likewise, for the Y. But yeah, the obvious one to go for is the Z. We look at that and that's what we're looking for. We do have motion limits, so we can set a minimum and a maximum. For example, I'm going to turn these guys on. We're going to put 180, and then we'll see we've got a 180 degree motion limit there. If we clicked to preview, we'll see it will only travel 180 and then back like so, but cannot do the full 360. That's not what we're after, but in certain circumstances, you may want that. We're going to turn that off. I don't want there to be any limits. I want the full 360. Let's play that, make sure we're doing 360. Okay, looking good. Let's click Okay. There we have our completed assembly all fully jointed. And you will notice that about the positions or the joints are these indicators that there are joints there now. And we can right click on these. We can edit that joint. We can suppress the joint, animate that joint, and so forth. So we did want to edit that. Let's say that we wanted to change this one to a rigid joint, come edit joint. Then the motion, we can change. We can change exo, cancel there. And we can also see that if we come down to our timeline, we've then got the four joints there. So we should have three rigid joints, and then the last revolute joint, which is this one here. And again, we can edit any from here, so right click and edit joint. If we don't want to be seeing these indicators that we have joints present, we can come under the display settings and the object visibility, then we can turn off joints, and then you'll see that the indicators are gone, and then we can just refer to them from the timeline or we can turn them back on, like so. And so that is a overview of using joints infusion. I think it's a fantastic tool and an interesting and simplistic approach to forming constrained assemblies. I also think that compared to traditional CAT software, that this is much more of an efficient process, but it can be slightly problematic when we're working with large scale complex assemblies. Now, I would recommend having a good study of the joint tool and adjusting where needed any of the parameters, such as the alignments and the various motion types. If you have any questions regarding joints and assemblies, please do send me a message, and I'll see you in the next lecture. 55. Contents Library: Okay, so at this point, we've used joints to assemble each of our individual parts. Everything's looking good there. We've got the poliwheel rotating like so with everything else being rigid. There's just one more thing to add then, which is the fastness, which go in the holes here. And I'd like to show you one of the built in features with infusion, which is to insert fastness. Go back on the home view. W to come up to the tabs at the top, I'm going to go under insert. We're going to select insert fastener. You can't hit the drop down, second one down there. Let's go insert fastener. Then from here, our toolbox pops up. We can do a search for fastness from there. You can also select some viewing options. So whether they're listed or tiles. For me, personally, I prefer tiles, so I'll leave it as that. We can then filter as well so we can filter by a standard. We can also filter by the unit system. So imperial inches, metric, mill. For me, I work in metrics, so I'm going to leave it as metric. And under here, yeah, we're looking for fasteners. And in this particular case, we're looking for, let's start off with some bolts. And we've got various options here, so the countersunk flanged hex. Let's go for instead of going for a flanged hex, we're just going to go for a hex, and then I want to insert washers as well and show you that option. So I'm under the hex head fasteners. Got options for self tapping sheet metal shoulder. Then we've got various options or hex head bolts here. I'm going to go with the very first one just as an example. And then we have quite a lot of parameters that we can adjust. Now, what's great about fusion and what I really like about this feature is that where we move the mouse point, fusion will do its best to pre calculate what the size of the fasten will be. For example, if I bring my mouse over, let's say, this hole here, okay? So that orientation is not what we're looking for, but if we move the mouse slightly, it will then recognize what will be the correct orientation. And it will also put in fastness, like we see on the other side as well. Which fusion we'll see as being similar. And we don't have to do that if we don't want. So under select similar, we can take that off, and if we come back, it will just do the one here. But in this particular case, I do want to have the same fastener in this hole as well. So if we can adjust this down like so, and a left click once, and then we can adjust the parameters here. The fusions recognize the whole site, and as assigned this Mate, okay? You can adjust this if that's not accurate, but in this case, Mate is good for us. In terms of the nominal length, so fusion now has input 30. Let's go on the front view. Yeah, 30 is okay. It's a bit long. We can get a nut on there with these. Let's go for 25 mil. Happy with that. And the material. We can assign a material here, stainless, aluminum. Gonna go for steel, another finish. Let's go for a black finish. And then once we're done with that, let's click Okay. Then you'll see that fusion has input the two fasteners there as per the parameter boxes, and they've applied a visual thread as well, so not a physical, and we need to repeat that process for the other side just here. That's insert fastener. Again, let's go bolts and screws. Let's go Hex head. I'm gonna pick the first one again as an example. Of the mouse over, click once, and then I'm going to adjust that to 25. By for the finish, I'll put that as black as well. Then presso. And then we have four hex head bolts put in place. That's nice. It's also had some washers there as an example, as well. Let's go back on Insert fastener. And here, let's choose the washers folder. Do we want a plane, a spring washer or a square? This is eight bolt. Springwher under that torque will do very little. So let's go for a plain washer. I'm just going to choose the first one as an example again. And it's the same process. So I've got select similar selected. To hover the mouse over. Then when I click once, I then hit the green tick here or press Okay. Fusion will adjust that bolt so that it then sits onto the fastener, which is a really nice feature. And perhaps at this point, actually, we might want to revert that length to 30 mil, as we haven't got much length on there for a nut, which we'll do in a second. Okay, and fusions applied washers to all four of those. That's fantastic. If we want to change any of the parameters about these fasteners, let's say, for example, we want to change the washers to black. Come down to our timeline. You can just simply right click on the feature, Edit fastener. Go on the finish. Let's put that as black. That's okay. We've adjusted that. That's nice. Let's also add on another five mill. So let's go for that 30 mill on the fasteners. Okay, so I'll come down to that feature there. Ed it fastener. But in 30 mill that's going to do these two over here. That's okay. And repeat the process for this feature as well, which is these two bolts here. G 30 mil, okay? And there we go. That's how we make use of this brilliant feature bit winter fusion. In my experience, a lot of the calculations that fusion does in order to auto adjust the size and length of fastness is actually really good and quite accurate, but at times we do need to implement some manual adjustment to get exactly what we're looking for. Okay. Any questions about that? Please send me a message. And I would recommend having a play around with the insert fastener toolbox. Plenty to choose from lots of different variations, according standards, et cetera. And overall, yeah, really useful and efficient tool. Saves us a lot of time when it comes to generating and assigning fastness as well. So I'll see you in the next lecture. 56. Cross Section Views: In the three D modeling section, we took a look at section analysis. In this lecture, I just want to show you that the same feature is also available to us when we're making assemblies. So to do this, we come under the inspect, we'll hit the drop down there. We'll come down to section analysis, and then just like in the modeling section, we need to select a plane or a face. So we could go to this face, for example, or we could go with the default plane here or this face. Going to select this face in this case. We've got some parameters we can adjust, but we can also adjust them manually as well. I bring this into let's just say halfway, and we just wanted to check the clearances and check the mating parts. Everything there looks good. And it's quite interesting to see if we look at the front view that we can see here the profile that we drew in order to revolve the pulley wheel. And also the same can be applied as well for the pin here if we saw split down and half there. That's the profile we sketched out. Now we see it being three D modeled. From a section analysis, I'm happy with that. I'm happy with the joints that we applied. That's looking good. Go back to the home view. And again, to leave the section view, come under to our browser and under the new folder analysis, you can hit the drop down. I've already got a section in there, but the one we just applied is Section two, and we can hide it like so or we can hide all of the analysis like that. If we want to edit the section view, we can just simply right click on it under the Analysis folder. We can select Edit, and then we can adjust any of the angles and so and also move it as well, like that. Exactly the same as three D modeling. And yet, let's hide that section view then. So just a quick tip for this lecture. I hope that helps, and I'll see you in the next lecture. 57. Visibility & Transparency: Another useful tip as well when we're working with assemblies is to control the visibility of a part and also the opacity as well. The visibility is very straightforward to control. Let's take this assembly here as an example, and let's say that we wanted to show this without the fasteners or without the hex head bolts and without the washers, as well. But very simply, we come over to the browser, and when we've got our folder here called fasteners, next up, we've got the eye icon. And if we select that, we'll then see that those are then hidden, though this essentially is the show hide option. If we only wanted to show or hide individual ones, we can hit the drop down there. And let's say we wanted to turn these guys off, maybe the two washers as well. Locate that one. There we go. So yeah, we just control everything in terms of visibility by shot and hide. And likewise, let's say we wanted to hide the base plate, could locate that we could hide that part, like so, or one of the bracket arms as well. And that's how we control the visibility of individual parts. Turn those back on. Another way to do this as well is to right click on a part. So let's say the Pulley wheel here. We right click come down to Show Hide, select that, and then hide that part. And then to turn the visibility back on, we come over to our browser where we've got the pulley wheel, hit the drop down there, hit the bodies, and then we turn the visibility of that body back on. But for me, I would recommend by using the show and hide icons in the browser. It's more easier to control and turn back on the visibility as opposed to right click and then selecting Show slash Hide. We may also want to change the opacity of a part. So, for example, if we take, let's say, the Pulewheel here, we didn't want this to be 100% opaque and we just wanted it to be partially transparent, we can control the element of opacity. So let's locate that part in our browser. It's come down. We've got pulley wheel here. I'm just going to select the pencil icon next to that part so that is edit in place. Left click that once. And now the environment has changed. Although we're still in the design environment, we aren't specifically editing only this part here. So if we come across again to the browser where we have our bodies, so in this case, we just have one revolved body here. We can right click on that. We can come down to opacity control. Let's say we want to set that to 50% and then right click on the part, select finish edit in place, and now we're back to the full assembly, and you'll see that our Pulewheel has that transparency there. If you want to change that just the same process, select the pencil icon. Come down to the body, right click. I'm under opacity control. Put that back to 100. Okay, right click, finish Edit in place. Now we're back to 100% opaque part. So that can be really useful if we're doing presentations or reports, and want to highlight certain parts. We can make the others partially transparent like that. Okay, another useful tip, and I'll see you in the next lecture. 58. Pattern Assemblies: In this lecture, we'll talk about patterning and assembly. So just like when we're two D sketching or when we are three D modeling, we do have the ability to pattern complete assemblies, as well. I'm going to give an example of that here. Let's say we wanted to pattern our entire assembly there. We'll come up to the creation tools, hit the dropdown, then we'll come down to pattern. And in this case, I'm going to go for a rectangular pattern. Sing left click that once. Then with the toolbox popping up, make sure we have rectangular patterns selected. Then in terms of object type, I want to make sure, in this case, that we're selecting components as we can now select each one of our individual components, including the fastness. We don't want to be selecting faces or features or bodies. Just want to select the components we've input. So when it comes to objects, we need to select these components. The easiest way to do this is just to click drag around our assembly, like so. And then you'll see in the browser that each one of our components are selected. And if we open up the fasteners folder, we can see that each one of the fasteners are selected as well. And so we can choose to deselect one of these. We hold down Control, left click once, or then see that bracket arm is no longer selected. But for this pattern, I want to make sure this is selected, hold down Control and select. Once we've identified everything to be patterned, they come to the axis, let's select that. In this case, I'm going to choose the Y axis, which is this one here, back on the home view. We've got our toolbox pop up, and I'm going to control this manually with this arrow here. I'm just going to drag this out. Currently, fusion has input a default, I have a quantity of three, but in this case, I'm going to go for four on the distribution to be extent and under distance, let's say, 500 mil Again, we can control that manually with the arrow there. I'm happy with that. Click Okay. There we have pan, our complete assembly. We have four in total. It's looking nice. A little army of pulleys there. And then if we come across to the browser, we'll then see that these additional components have been added, and it's also the same for the fasteners as well. So suddenly our browser tree has become very populated. That's how we can pattern assemblies. I just wanted to show you that to make you aware that you can pattern complete assemblies, as well as three D models in any sketch entities as well. So just another quick tip there, and I'm sure that will be of great use to you, and I will see you in the next lecture. 59. Editing Existing Assemblies: In this lecture, we'll take a look at different ways that we can edit our assemblies. So the first and foremost way to edit an existing assembly is refer to the timeline, just at the bottom left down here. Again, we can scroll this arrow back and forth to kind of go back in time and see where we were at that point. And as we scroll through, we'll then see the complete assembly form. We can make an edit to any one of these items here. So, for example, this joint here was from the bracket arm to the base plate. We can make a change there by right clicking and editing. Likewise, we can do exactly the same for anything here. So in terms of the fasteners, we can right click, edit the fasteners there, we can edit their joints and so forth. Can also edit joints as well from the browser. So if we come up here under our joints, all of these joints here are associated with our first assembly that we did here, and then those are then patterned across. If we want to make an edit to an existing part with in assembly, there are different ways in which we can do this infusion, but I recommend following the structure behind traditional CAT softwares as that keeps things very easy to control, and it ensures that we're not prone to making mistakes. So to do this, I'm going to give an example here. Let's say that we want to edit the base plate. So we've got the same part here, which is all linked to the same base plate file. So let's find that in the browser, then, we've got the first base plate here, but the second one here and so forth. And we can make this change. And we can make one change to any one of these and they'll be reflected in that linked file. So for example, I'm going to choose this base plate here, which is this component here, and we're going to right click on that and then select Open. Once a part file opens, let's make our change. So I'm just going to go for a simple change. I'm going to increase the thickness of this. So that's our extrusion right here. I'm going to right click on that, select Edit feature, and I'm going to bump that up to, let's say, 25 mil o. That gives us a much more beefy base plate there. Following that, we want to hit Save. We click Okay. And then let's come up to our Pulley assembly file. And what we'll see here is we'll see a warning message appear in the bottom right here saying that one of our references or one of our components is out of date, and we need to update that. So it's referring to the change that we just made regarding the base plate. So let's come up to the top left and where we've got the update icon here. We left click that once, and then fusion will process that change and then refer to the latest saved file, which in this case, is the linked base plate file here. And as we can see, that change is then reflected to all of our patterned base plates here. Another way which we can edit files as well is to select Edit in place. But I would recommend avoiding to do this because if we edit in place, it will edit in reference to this particular design here as opposed to the original linked file. And so, yeah, any changes we want to make always right click. Let's go open, make the change, hit Save. And then in our assembly file, click the update icon, and then we'll see that change reflected there. And that will also be reflected as well in the original linked part file. I hope that makes sense. And again, any questions over editing parts or assemblies, please do give me a message. Aside from that, I'll see you in the next lecture. 60. Project 1 Introduction: In this section, we'll start our very own first project, a workbench that features a lower shelf and a 96 millimeter pattern of dog holes on the top base. This workbench was actually a custom design project for a client of ours in the UK back in 2022, and I think that it's a good exercise for those who are learning fusion in order to practice two D sketching, three D modeling, and forming assemblies. So the sketching and modeling, they're fairly straightforward, but the positioning of each part according to the design needs to be done accurately by adjusting certain parameters in the joint command, which does require certain considerations. But overall, I think it's a fun ject and realistic for any woodworker to build. In terms of joinery, there are many techniques available to construct this part, I pocket holes, angle brackets, or just wood screws, et cetera. We're not so much interested in the joinery techniques, but rather the focus is on modeling and construction. And I hope you enjoy this project, and please send me a message if you have any questions or comments. So let's model and build our workbench. 61. Table Top & Shelf: In the first lecture of this project, we'll model the tabletop and also the lower shelf. But let's start with the tabletop. Come under a new design, and I'm just going to show here the dimensions. And if you would like to draw this yourself, please feel free to do so. But continuing on, I will model this part. But first of all, I'm going to click Save. I'm going go down and title this. Make sure the location is correct. So it's in our project folder, and then under here, I've actually created a new folder, which is Project one workbench. You can go on the drop down and you can add any new folders you want to your current projects. We click Save. Then I'm going to start sketching. So let's hit C on the keyboard. Let's go on the XY plane. Let's hit R on the keyboard, rectangle, start of the origin, and we'll drag that out 1.8 meters in length. So 1,800 mil plus tab on the keyboard, and then 750 mil on the height, plus Enter. Double click the middle mouse button there. Okay, that's looking good. Now, as for the dog holes, we can pattern these in here, and then we can only extrude one profile, but that will give us all of the features we need. So let's say C on the keyboard. We're drawing a circle, and each one of these holes has a diameter of 20 mil. Let's position our first one, press D on the keyboard and dimension from the center point to the vertical. That's a dimension of 180. And then from the center point to the top horizontal, we've got a dimension there of 13, five. Then from here, let's go create and we're going to select rectangular pattern. In terms of our objects, we're going to drag select around the circle. And then in terms of directions, we're going to take this direction and this one. Under distribution, we want to be under spacing. We want to have suppression turned on as we will be suppressing a number of the holes. I'll show you why later. In terms of quantity, and this is coming across the first direction, we want to have a total of 16. Press tab on the keyboard, and then we're going to put 96 mill. That's a spacing between each one. And then for the other direction, we're going to go for a quantity of six, press tab on the keyboard, and we want these to be a square pattern. So let's put 96 in again. That's looking good. Now, there are a few of these that we need to suppress, which is the fifth row in from both sides. And the reason for that is in this area here, this is where one of the braces sit beneath this tabletop, so we don't want to have any conflict there. Let's go ahead and select these checkboxes here to remove them and exactly the same process on the other side. One, two, three, four, going for five, one, two, Okay. Once that's done, let's click Okay. It's looking good so far. Let's finish this sketch. Let's extrude on the keyboard. And then select this profile here. And then in terms of distance, let's go for 20 mil, let's enter. That is looking nice. We just need to add. We just need to add a good appearance. So let's go for A on the keyboard appearance. And then in the library, so the material that I went for is a wood in brackets solid, and I went for an unfinished, in this case, I went for three D pine unfinished. I'm just going to drag that up, drop it down on the existing appearance, click Close, go on the home view. And there we have the tabletop. That's looking nice. And next up, we just need to model the lower shelf. So let's go on new design at the top, let's go ahead and save this part. So I'm going to title this. And again, make sure that's in the correct location. Look safe. These are the dimensions of the lower shelf. So if you would like to model this yourself, please feel free to do so. But otherwise, I will continue to model this myself. By nice, easy sketch this one, hit C on the keyboard. And again, we're going to go for the XY plane. Use the rectangle tool, start of the origin, drag this out. Got a length there of 1.7 meters, 1,700 mil, and a height of 650. And then within that we need the cutoffs for where the legs will sit. So to do this, I'm going to go for a rectangle tool again. I go to start at this corner point. Back that out, 75 tab on the keyboard, 75. Do the same process down here, origin, 75 tab, 75. And just to mix things up a bit, I'm going to put in a construction line, so select construction in this palette there. Start at the midpoint of this line. Make sure it's 90 degrees, finish at the midpoint of this line. I'm going to choose the mirror tool, the mirror, and I want to mirror these two lines and also these the mirror line, select that construction line. Let's click Okay. Review is looking good. I like that. Let's go on finish sketch. It's said E on the keyboard. We only want to extrude this profile here. There are quite a few profiles we can choose from. We just want this one here. In terms of distance, we have another 20 mile there. That's okay. Yeah, that's looking nice. Write it A on the keyboard. Let's go ahead in our materials, and let's apply the same one. So three D pine unfinished. Drop that on the existing appearance, click Close back to the home view. And there we have the lower shelf, nice and easy. Okay, so that concludes for this lecture, and I'll see you in the next one where we'll continue to model this workbench. 62. Legs: Next up in our assembly, we need to model the table legs here. So let's go on a new design. And these are the dimensions of the table leg, so feel free to draw this yourself. I'm going to go ahead and click Save. Make sure it's the right location. Then click Save. Nice straightforward. Let's go and create sketch. Let's do this on the XY, R on the keyboard rectangle, start at the origin, 75 tab 75. A, finish the sketch there, hit E on the keyboard. Our oniPfile has been automatically selected by fusion in distance here, 850 press ok back to the home view. Hit A on the keyboard. We're going to apply the same appearance here, three D pine unfinished look. And there we have the workbench legs. Very straightforward, but a fundamental part of our workbench. I'll see you in the next lecture. 63. Frame Aprons: So far, we've modeled the tabletop, the lower shelf, and also the legs. And in this lecture, we will model all of the aprons, which are these parts here. So let's go in a new design, and let's start with the long apron first. So there are four of these in our final assembly. These are the dimensions here, so feel free to model this yourself. Let's set C on the keyboard. We're going to draw this on the Y Z plane, press R on the keyboard, start at the origin. We're going to type in 25, so 1 ", press tab, 75 mil. So that's three inch, press enter. That's then press extrude. And we're going to extrude this by distance as per the drawing of 1550 preso. Home view, going to hit A on the keyboard, and let's apply the same appearance three D pine, close. Save that part. We'll call that apron long. Look, save. Now let's do these short aprons. So new design. These are the dimensions here, so feel free to model these yourself. Let's C on the keyboard, and in this case, we're going to go for the X z plane. R on the keyboard rectangle, start at the origin, 25 by 75, E on the keyboard extrude, distance here, 500, Enter, go on the home view appearance. We'll apply the same appearance, drop that in, press close, and we'll save that and call it short aprons. Okay, nice and easy. And then in the final electrons, we'll model the braces before we complete the entire assembly. So I'll see you there. 64. Braces: The final parts to be modeled are the braces for our workbench. Which are these parts here. So, let's go on a new design. These are the dimensions of these support braces, so feel free to model this yourself, if you'd like. But I'll put them in a corner now, and then I can model this part. The first of all, we'll start with these support braces. Let's hit C on the keyboard. We're going to draw these on the E z plane, hit R on the keyboard rectangle, start from the origin, 75 tab 75, E on the keyboard, extrude that distance 580, enter, on the home view, appearance. Again, let's apply a three D pine unfinished close. Let's save that part. We're going to call that support brace. Save. And then we'll start a new design. And here we'll model the shelf brace. Same process, C on the keyboard, same plane, rectangle tool, origin, 75 by 75, E on the keyboard. I'm gonna extrude that by 500, enter home view looking good. Press appearance, apply three pine, unfinished. And we're going to save that part as well. Gonna call that shelf brace. Look, save. Okay, and that's all the parts modeled now, we're ready to form the assembly. So I'll see you in the next lecture for that. 65. Workbench Assembly: So now we have modeled all of the parts of our workbench. We can now go on to forming the complete assembly. So if you select the nine dots just in the left corner, you'll see the data panel, and then within that, you should have every part that we've previously drawn. So let's start off with the legs, then, and we'll use this as a reference to add in all of the other parts. Let's right click here. Select insert into current design. We've got our leg appear there, and that's landed at the origin. We'll click Okay. We're happy with that. And the first thing we're going to do is go to our creation tools, come under pattern tools, and we're going to rectangular pattern this leg. So in terms of the object type, we want to make sure we have components selected. Okay? And then in terms of objects, we can either select the part here or we can select the part in the browser. So our left click once on the part. Then in terms of axis, we want to be going down the X axis and also down the Y axis. Let me bring out the X axis then. Okay? So fusion is using a default of three as a pattern. Let's change that to two. Then the distance that we're patterning by is 1625 mil. Okay, and then we'll move on to the Y. And again, let's change that to two. And then distance there is 57 5 millimeters. Press Okay. You'll notice here that all of the parts that we've patterned, we cannot move. And that is because they are patterned from the original part, which is this one here, and that is grounded to this file. So all of these four are now fixed, which is great. And we can move on now and add in. Let's go for the apron. Let's go for the short apron. Right click on that, insert the current design. That's in the correct orientation and almost in the right position. Just roughly position that. Click Okay. And then we're going to use the joint command. So we need to select a point. That's first of all, choose the apron. I'm going to choose this face here. We see our available points we can select. I'm going to go with the top corner here. Left click once. Then if we rotate the part, then we match that to the corresponding point on this face, which is this point here, left click again. It's looking nice, and we're going to bring that in. We want that to have an offset actually minus ten mil, in this case, minus ten. Press Enter. There we have our short apron. Let's go ahead and add a long apron, right click on that, insert current design. See, that's in the correct orientation? That's good. Let's bring that up, okay. Press J on the keyboard again. And in this case, we're going to select this face. So mouse over this face, and then bring up to select this point. Left click once. And then its corresponding point would be on this face. And this point here, left click. And again, we're going to offset that by ten mil, press Okay. Looking good. Let's add in the other one. Right click Insert. Bring that across slightly ups, okay. Is J on the keyboard. Let's go for this point here, and its corresponding one would be this point here. We're just going to draw that in ten mil like soap. Then let's add the last short apron insert. Bring that across. J on the keyboard. And we're going to reference this point here to this point here, again, offset that ten mil. It's okay. There we go. So our frame is forming. Let's also add in the braces. So these are these support braces insert into current design. Similar process here. But in this case, we're going to press J, and we're going to reference from this face here, which means we want to select this corner point here, so mouse on this face, select this point. Corresponding point would be this face point here. And then we're going to offset that by distance of 400 mil. Okay. Repeat the process again for the other side. All that across, then up. Okay. Okay on the keyboard. Select this point here. Corresponding point this one here. And we're gonna pull that across. That's -400 offset. Press Okay. There we go. Looking good. And at this point, we can add the tabletop. So let's right click on that part. Insert current design. Now, let's push this up, like so, okay. In terms of reference point here, let's use joint, and let's use this corner here and we'll match that to this point here. And now we want to offset this by 50 mil in this direction, offset 50 and also 50 mil in this direction. Yeah, 50 and 50's press Okay. Have a look at that from the bottom view. That's looking nice. And I'm just going to use the inspection tool here. So the measurement tool, hit I on the keyboard. Select this face, select this face. Should see there 50 mil. That's good. We clear those, select this face. And this one here. Yeah, 50 mil. Perfect. Okay, yeah, we know that's in the right position. And now we can go ahead and do the shelf. So just before I do that, I want to turn off the joints and to do that, display settings, object visibility and just turn off the joint visibility there. That's looking better already. So for the shelf, let's put in our braces between the legs. So right click insert current design. I'm just going to click Okay there. And I'm going to choose in terms of a joint, let's choose this face here. And we're going to choose this joint, this point, sorry. And then that corresponds with this point here, left click once. And I'm going to offset that. In this case, it's 150 mil. That's okay. Same process on the other side, insert current design. Draw that across. Okay, Let's J on the keyboard. Let's select this point here and make a corresponding joint with this point here. And let's offset Let's offset that as well. 150, enter. Okay, that's looking nice. Let's also get the aprons in there for the shelf, as well. The Rilk insert current design. Then process again. Move that roughly's J on the keyboard. Let's go from this point here. Do this point here. Offset that by ten mil. And then in this axis, we want to offset that offset that by 150 enter. Do the same on the other side, right click insert. Okay, just go to put that into position roughly with a mouse, J on the keyboard, this face, this point, this face, this point. Ten mil offset this direction, and then this direction. We want an offset of 150, Enter. Go on the home view. Okay, coming together, let's also get the support braces in there as well. So right click Insert. Okay, roughly position that. Let's press J on the keyboard then, and we're going to go we're going to go this face, this corner. The corresponding point there is here. We're going to offset that by 400. Okay. Nice. And one more. Repeat that process. -400 Enter. And now we're ready to add in the lower shelf. So let's get our lower shelf. Right click Insert. Okay, go to bring that up. Press okay. And then in terms of a joint here, we've got many options to select, but in this case, I'm gonna owe this face and this face and this point. And that corresponds with this face and this joint, except it's going to be offset by ten mil, like so, press okay. There, see that? It's a nice fit. Same with this corner. Let's check the other two as well. Yep. Okay, yeah, that is our workbench. So it is quite a repetitive process when it comes to joints. In terms of efficiency, it's about understanding, which points to select and their corresponding points and then forming the appropriate joints from there. Just one thing I want to point out is if I go and edit one of these joints, I just want to highlight that on the motion type of every joint we just made was rigid as it should be. Like we wouldn't want to, let's say, check, uh choose the revolute motion type, for example, or perhaps let's go for a pin slot. Okay, we definitely don't want our workbench to be doing that. So yeah, all joints here are rigid in this case, as they should be for a workbench. Let's press Okay. And as you can see, the reason that we removed the dog holes down this column here and also down this column was just to avoid any conflict with the lower braces here. The client was yet more than satisfied with that. Okay, so that is the project for the workbench. Hope you guys get along well with that. Any questions? Please do send me a message. But aside from that, I'll see you in the next project. 66. Project 2 Introduction: In this section, we'll model a phone stand and a generic design of smartphone. And both of these parts are suitable for three D printing. We'll start by sketching and three D modeling each part. We'll then form an assembly and learn how to export each file individually as an STL, considering the mesh refinement settings, and then you will have the ability to import that file into your slicing software for three D printing. So both the phone stand and the phone itself are interesting to sketch and model, as they make use of multi body components and a large variety of sketch and modeling tools. So let's start designing for three D printing. 67. Modelling the Phone Stand: Let's start by modeling the three D printed phone stand. Although this part looks fairly simple to either extrude or sweep, we need to be conscious of the assignment of different appearances, I E, the gray and the green appearances. To enable these features, we need to create two individual bodies that we can each assign appearance to. So if we look at the browser, we can see under our bodies folder, I have two bodies here, one that I've titled outer body gray and out of body green. So if I hide the green, we'll see the single body there. Okay? And then if we hide that, switch those guys around, we'll see the other body there. And this makes for an interesting two D sketch where we will take advantage of the offset tool to give us two separate profiles. And we can then later project these sketches and form two different extrusions, therefore, giving us the two separate bodies. So I've included these sketch dimensions here, if you would like to model this yourself, and from here on in, I will have a go at this sketch and model. So let's begin. Let's go on a new design. So to model this, the technique I would recommend here would be to model the inner profile line and then by simply offsetting that in both directions so that we get the two profiles, and then we can extrude both of those as separate bodies. So let's go on Create sketch, and we're going to do this on the X z plane. And we're going to start to the origin to start with. We're going to do an arc, to do a three point arc, start to the origin. I'm going to bring this roughly down here and just raw in a rough arc, which we can later dimension and constrain. Let's then press L on the keyboard, and we're going to come across here by the dimension 66 mil. Let's enter. Going to stay on the line tool, hold down the left mouse button until we draw out a tangential arc like so. Then we're going to come across by 42 mil, again, stay on the line tool and draw out another tangential arc roughly like so, and then we're going to draw up this line here, which is about 60 degrees. Going to tidy up these dimensions. And first of all, I'm going to apply a tangential constraint. As we can see here, we need a tangential constraint between this arc and this line, and also the same between this arc and this line. And likewise, it's this arc and this line here. Let's now go ahead and press D on the keyboard, let's dimension this arc here. So we've got a rad there of 6.5 mil, okay. Let's dimension this arc here. Let's got a rad of seven mil. And this arc here also has a rad of seven mil. We're going to apply a length to this line here of 60 mil And then we're just going to revisit the arc down here. So this is still mobile, like we can see here. What we want to do is have a horizontal constraint between the origin and this point here. Let's choose the horizontal vertical constraint, select the origin, and this is the center point of our arc here, or select that. Now we'll see the majority of our sketches in black. The only thing we need to define here is the angle of this line here. So let's hit D on the keyboard. I'll select this line and this line here. And this has a dimension of 60 degrees. Press Enter. And now we should be fully constrained. Everything's in black. And if we go into our sketches folder, we'll see the red padlock there indicating everything is now fully constrained. That's fantastic. And now we need to create the two profiles to us to extrude, both of the individual bodies. And for this, we're going to use the offset tool. I'm going to refer to the entities that we've already drawn. So we don't want these to be creating any profiles, and so I'm going to drag select around those, and then we'll identify them as construction lines, like so. I'm also going to turn off all of these dimensions as well. It's getting a bit hectic on the screen. So in our palette, turn off the dimensions much easier to see. I'll also turn off the constraints for now as well. So let's go ahead and use the offset tool then. Hit O on the keyboard. And then in terms of our curves, we need to select our curve here, and we want to make sure we've got chain selection turned on. We want to make sure also we've got two sides turned on as well. So if we select this entity here, we'll see it with change select, left click once. We've got the offset then in both directions, and the distance we want to go for is 2 millimeters. Want to leave everything else as the default. Click Okay. Then we want to repeat that process. So I'll press O on the keyboard, select our construction line again, keep everything else as the defaults. Make sure chain selection is turned on, two sides is turned on as well. And then in terms of the distance, we're going to go for naught 0.75 press Okay. And then from here, we need to complete the profiles. So here we need to close up these gaps and the same on the top, as well. Let's start with this one down here. We're going to press L on the keyboard, use a line tool. We start from this point, hard down the left mouse button, draw out a tangential arc, we'll finish that at this point here, and the same process, bringing this one around here. I'm happy with those tangential arcs just turn my constraints on. Make this one tangential, as well. This line to this point, and this arc to this arc. That's looking good. Now, there's still a bit of movement here. That's because we can move this arc up and down, and the same with this one. So we just want to make sure these center points are matching to the endpoint of this construction line or to the origin. So let's go on the coincident constraint, and we'll select the center point of this arc here. Select. Then we'll select our place of origin there, do exactly the same process. So the center point of the large arc, bring that to the origin, as well. Black in color, fully constrained, looking good. Let's now take a look at the top. Same process, on the keyboard, hog down the left mouse button and draw around that tangential arc like so. And the same process here. Looking good. I want to get that tangential constraint between these two. Select that constraint. Straight line to the arc. It's looking nice. There's still some movement here. We can see we've got two arcs coming out. So let's repeat the process again, coincident constraint. This time we're going to go center point of the small arc to the endpoint of our construction line, centerpoint of the large arc, endpoint of our construction line. Right click. Okay. And then if we take a look at our sketch, we've got the red padlock there. That's fully constrained. That's good. And if we look, we've got our two profiles. So this profile here, the outer one, that's our gray colored body, and then the inner one here would be our green colored body. So that's now ready to extrude. Let's finish the sketch there. Let's go on our three D tools, hit Extrude. Let's go with the outer one first. I'm going to take a look from this corner here, and I'm going to right click on the ViewCube and set the current view as home fit to view. So this is now our home view. And we're going to extend this by a total of 18 millimeters. That's okay. Then if we look at our folder here, we've got body one. Okay. And if we look, we've then got this gap in the center there, which is where our second body will be. So to do this, we're going to create a new sketch. We're going to do this on the same plane, so the plane. And in this case, we're going to project this existing body onto this plane, and then we can extrude from there. So hit P on the keyboard. In terms of geometry, we want to make sure that we're not specifying an entity. We'd have to select a lot of entities for that, but instead we're selecting a body. And in this case, I'm just going to choose this body here or we can choose body one from the browser. Click Okay. Now you can see in purple, all of the sketch entities about that body are now projected. Let's finish the sketch there. E on the keyboard extrude. You need to select a profile. In this case, we want the inner profile. Just zoom out a bit and make sure that's going in the correct direction yet, like so. We only want that going 80 millimeters. And we want to make sure that under our operation that we're going with new body. So this will give us the both bodies we can apply each appearance to. So once that's selected, press Okay, now we could see we've got this joint between the two there. And if we look in our bodies folder, got body one, the exterior, and body two is the interior. Okay, so there we go. There we have our phone stand. Now let's apply our appearances. So hit A on the keyboard, and we're going to come down to our appearances. We're gonna come under the paint options, and we're going to go with the powder coat smooth folder. And then under that, for me, personally, I've gone with the powder Coat dark ray, but feel free to select any of these. And we want to apply these to one body only. Going to select that appearance, and I'm just going to drop that on body one in the browser, glow of that. You can see the color change there. I got a nice smooth powder coat gray in this case. And then for body two, I want to go for one that's called LED green. Hold down left mouse button on this one, and drag that over to body two. Then we can see that appearance up here. We can close that. Just have a look at that from the front view. Everything's looking good there. All the geometry is correct. I just wanted to add at this point that if you are using a multi color three D printer, the splicing software would need to distinguish between the green and the gray bodies. So in order to do this, I would recommend having a protruded face coming from this profile here. So if we hit E on the keyboard and we then select that profile, we can draw that out by, let's say, our 0.25. Okay. And instead of the operation join, we're going to go for a new body Okay, and do the same for the other side, then hit A on the keyboard and assign this appearance to those new bodies. Click close, and then we can even add a fillet to that, as well. Let's chain this edge here. Let's go for the fillet 0.25, give us a nice round over there. And there we have that face protruding. So again, depending on your slicing software, you may need to identify these faces here as the ones to apply the green filament to. Yeah, that's looking nice. Okay. And there we have our phone stand. I hope you were able to follow along okay there. And again, any questions, please do send them to me. I'll reply as soon as I can. And I look forward to seeing you in the next lecture, where we'll model a 380 printed phone. So I'll see you there. 68. Modelling the SmartPhone: So now we have completed the phone stand. Let's go ahead and three D model the generic smartphone. Just a quick disclaimer, by the way. If you are intending to three D put in this, it will not fully function as a smartphone, but just as a model as a bit of a gimmick for maybe a desktop present, it can be done. Okay, so let's go ahead and let's hide the stand, and this is what we're going to be focusing on today. So all the features here we'll add, including the decors if you like, as well. So let's go on to a new design. Now let's start with a create sketch. And we're going to start the sketch on the X z plane. That's the most suited plane to do this sketch on, and then we'll extruded from there. So we'll select that plane there, hit R on the keyboard. We're going to start at the origin. We're going to give this a width of 78 mil, press tap on the keyboard, I give that a height of 160. Press Enter. Go on to the home view. Okay, there's our footprint there. Let's add some fillets to this then. I'm going to do this in sketch mode. Start, select fillet, select this corner point here, this one, as well. And also the remaining two here. Going to give that a dimension of that's got a radius of 15 mil. Plus enter. Looking good. Let's finish this sketch. Let's go extrude. Let's extrude that body by eight mil. And then just around off these sharp edges that we've got around both sides of the phone. Let's use the Fillet tool again. Make sure that we've got tangent chain selected, okay? We're going to select this chain here and also this one, we're going to give that radius of two mil. Okay, press enter. And next up, we will model the screen face. So this is going to be the front of our phone. So let's right click on this face. Go and create sketch. We're going to offset all of the entities surrounding the phone on this face here. So let's select the offset tool. Make sure we've got chain selection turned on. We don't need two sides. We're only going to offset in one side, so we'll turn that off, and let's go ahead and select this chain of entities here. I want to be chaining inside to a negative value. And we're going to go for in this case, it's a negative three. Press Enter. And then if we come up to the top, we're going to make some allowance for the speaker and also the proximity sensors. Let's L on the keyboard. We're going to start anywhere snapping on to this line here. Going to come down, go to come across and then back up, go to position this centrally in a second. Let's press D on the keyboard then, select this line, and they're going to select the endpoint of this arc here. We'll put in a dimension there of ten mil. And we're going to repeat that process for this line here. So the end of this arc in this case, and also ten mil. And then we can select let's go this line to this one. We can put in a dimension there. That's three mill, and then we're going to apply some fillets here. So we'll select the fillet tool, and we're going to take between these two lines. Give that a fillet of 0.5. We also want to do the same on the other side. Gonna put that line back in then from this point to this point, select our fillet tool. We're going to go this corner here. And again, we're going to choose 0.5 for us enter, then we'll also give some fillets to these corners here. Let's go back on the fillet tool then. Select this corner point here and this corner point. Then we'll give radius two mill there. Looking good. Notice over here, these lines are blue. Okay, they're not fully constrained, so we've got some movement going on here. So this line here, we want to use the horizontal constrain, ay that to this line, and then we have all black color fully constrained. And we can confirm that with the sketch to having the red padlock. And that's our sketch down. We've got one profile here we want to extrude. Let's go on finish sketch we'll press E on the keyboard extrude. We're going to select this profile here. Then in our toolbox, we're going to enter a dimension of 0.25 mil, and we want to join that to the existing body. Press Okay. Then we can revisit this face here, we can add in our speaker and also the proximity sensors. So I'm going to right click on this face, select Create sketch. Knock down there. Let's come back up to the top. Press L on the keyboard, and I'm going to draw in a construction line. So just a reference line from this point to this point. And then from here, we can use the centerpoint slot from the midpoint of this construction line to give us our speaker grill. So we go on create slot. Choose a center point slot, come across till we snap onto the midpoint there. Gonna draw that across. That's got a distance of five mil. G to make sure that that is horizontal, like so. I'm gonna turn off construction line as well. And then that has a diameter we want to give. So we got diameter three, enter three. Okay. And then we just need to add in these sensors. So press C on the keyboard. We want to snap to this line here, it can be anywhere for the time being. L span those out, give them a diameter, 1.5, repeat the process for the other side, C on the keyboard, 1.5, enter. Press D on the keyboard dimension. We're going to dimension from this center point here to the center point of this arc of a slot. Put that dimension there, we'll give that five mill and then same process for the other side to this center point. Five mil. Then we go fully constrained. And then we're going to extrude cut these three profiles here. So let's finish the sketch to E on the keyboard. And we'll select this profile, this one, and this one here. Then we go for a cutting operation. So we're extruding by minus, and in this case, it's 0.25. That's okay. And there we have the slot there. It's going to represent our speaker and the two holes there, which will represent the sensors, proximity sensors. Okay, that's looking good. Next, we need to add the volume buttons. So these are going to go on this face here. So I'm going to right click on this face, and create sketch. And I want to draw in a slot. In this case, I'm going to go with another center point slot. Start that just anywhere for the time being, and I will position that shortly after. So that's got a overall length of ten mil, so we're going to go with five between the center point of the slot and the center point of the first arc. Then that's click once. Let's draw out that slot there. That's got a diameter of 2.4. Press Enter. Now we just need to position this. So I'm going to press D on the keyboard and from the center point of this arc to this line here or this point, we're going to go with 25 mil. And then I just want to do a vertical constraint between the center point of this line. So I'm going to hold down shift, select that center point, and then I'm going to select the center point of our slot. Okay, that's good. That's all in black, apart from this blue line here. So we just need to put in that dimension there, select this line. That's ten mil. Just enter so that's for the volume up, and now we need the volume down, which is the same button, same geometries, so I'm just going to pattern that. L on the keyboard to snap onto this line, and I'm going to make that a construction line. Okay? We don't want any profiles coming from it. It's just a reference line. We're going to dimension this from the center point of this arc at two mil. Okay, so the center point of the volume up to the center point of the volume down will be four mil. Let's go ahead and use the mirror tool. Go to drag select around our volume up button. And in terms of the mirror line, we'll select our construction line there. Press ok. Looking good. Everything's in black color, fully constrained. We've got the red padlock. Let's finish that sketch. And let's go ahead and solid. Let's hit E on the keyboard, and we'll select our profile for volume up and the profile for volume down. Now we'll extrude those by a distance of 1 millimeter. Okay, press ok. Looking right. Let's go ahead and get rid of these sort of sharp edges where this join is and also the sharp edges on the outside as well. Let's use the fillet command. And we're going to do two fillets here. Make sure we got tangent chain on. We're going to select this chain and this one. I'm going to give the fillet a 0.4, and then we're going to hit plus, give another fillet, which will be this chain and this chain, the two outs, and they're going to have a fillet of 0.1 mil. Press Okay. That's looking good. So we've got our two volume buttons, but we do need a power button on the other side. So let's start a new two D sketch on this face right click Create sketch. And what we're going to do here, we're going to take a bit of a shortcut. We're actually going to project this geometry onto the other side, and then we can extrude from there. So let's hit P on the keyboard and project. And in this case, we want to project specified entities. The entities we want to select are this one, this arc. This one here and also the lower rc. So we selected all those entities there. Let's press Okay, see what happens. Hopefully, on the other side, yeah, that's what we want to see. Our power button is based off exactly the same geometries and sketch profile as the volume button, so that's ready to extrude. So we can finish the sketch, E on the keyboard. We're going to select this profile here. And we're going to extrude that. Let's go for one mil or so, press Okay, and again, we'll apply some fillets to that. To fill it. Chain this 10.4. G click Plus and chain this one as 0.1. It's okay. There we have our power button and now volume up volume down, looking nice. Next, we can go ahead and add the charging port, which is on the bottom face here. So right click there once. Let's go and create sketch. And we're going to draw in a slot. It's come under our creation tools. Got a slot. Let's do a center point slot. Just going to draw this in actually away from this face, and then we can dimension it afterwards. So in terms of the length or center point of the slot to the center point of the first arc, it's going to be four mill. Left click once. And then the width of the slot, in this case, is 2.8 mill. That's okay. And then we can use constraints to put this in the right place. Just going to add in a dimension that eight mill in there. Let's enter. Okay, now we can move that around. We want it somewhere in the center. So let's use the vertical constraint. Let's snap on to the midpoint of this line. So again, hold down and shift on the keyboard, select the midpoint of that line, and then select the center point of our slot here. Okay, that's good. And now it's constrained too at the midpoint of this line vertically. Now we want to do the same practice, but horizontally with the midpoint of this line. It's a horizontal constraint, hold down shift, select that point, centerpoint of the slot. All black in color, fully constrained. And that's ready to be extruded. So let's finish the sketch. Yeah. Rotate that slightly. E on the keyboard, then, select that profile. And we're going to extrude this. So it's going to be an extrude cutting operation. So we're going to put minus in. Then we're going to add minus five operations cut. That's correct. Preview looks good. Press Okay. Then we have our charging port. Another feature that we need to add to this face here is the speakers and also the microphone. So I'll right click here, go and create a sketch. And to do this, we're going to pattern across a number of circles and then mirror them onto the other side. So I'm going to hit L on the keyboard. I'm going to put this in as a construction line. It's just for reference. I go to start at the midpoint of this line, bring that across to the midpoint of this line. And I'm going to hit C on the keyboard, I'm going to snap on to this line here, bring that out, although we don't want a construction line. We actually want this as a profile, so take construction off. Give it a diameter of one mil, enter and let's hit D on the keyboard and dimension from the center point here to the center point of this arc. Give that a dimension of five mile, and then we're going to rectangular pattern this in this direction. So that's come under creation tools, doing our rectangular pattern tool, in terms of objects, Tracks select the circle. In terms of direction or directions, we only want one direction. We're going to choose the construction line. Just bring this across. That's the direction we want to be going in. In terms of quantity, we want a total of six and distribution, we want spacing. So that's the spacing between each one. We want that spacing to be minus two -2 millimeters. That's okay. Looking good. And now let's mirror those onto the other side. So I'm going to put in another construction line, press L on the keyboard. Mark that as construction. Going to go from the midpoint of this line, bring that down, midpoint of this line. Then we're going to use the mirror tool, and we're going to select these holes here as our objects. Then in terms of mirror line, we'll select this center line here. It's okay. Now we've got one, two, three, four, five, six. We've got our 12 profiles there. Okay, let's go back on the home view. Let's finish that sketch, then. That's fully constrained. Let's hit E on the keyboard in terms of profiles to extrude. Select these guys, drag select, and the same for these guys, as well. Want this to be a cutting operation. So on the distance, go to minus. Then we want -2 millimeters. Are preview looks good. Pre okay. Then we have our speakers microphone. The next feature to add is the cameras on the back. Okay, so I'm going to do these in the top left corner here. Right click this face, create sketch. Let's go ahead and draw in a rectangle two point rectangle to hit R on the keyboard. Just go to draw in rough rectangle there, give that dimensions width 25, hit tab on the keyboard, height 30, press Enter. I want to give some radii to these guys. Just going to do that in sketch. So fill it. Hose this corner, this one, and these guys gonna give those a rod of five mil, press Enter. Just go to move these dimensions out, tidy that up a bit. And now let's position this a bit more accurately. So let's it D on the keyboard, let's do a dimension. Let's go from this point to this point here. That dimension, let's go for five mil. Then let's go from the same point to the same point again. But in this case, we'll go a height dimension. So that will also be five mil, and then that's fully constrained. That's ready to be extruded, so we can finish the sketch there, it E on the keyboard. Can select this profile here, and we'll extrude that by a distance of 2.5 mil. So we'll look at that from the side. Yeah, okay, that's looking all right. It's okay. Let's go ahead and get rid of these sharp edges here. So again, let's chose the fillet command. Choose this chain here. We're going to give that a fillet of not 0.4. And then click the plus icon. We'll go for this chain here. Let's also give that fillet of 0.4. Press Okay. It's looking nice. Now we just need to input some extrusions for the cameras and also the flashlight. I'll be this face here. Let's right quick. Create sketch. Oop, come back to that, press C on the keyboard. Let's enter in some of these circles then I'm going to enter one camera. Let's go for two and three. And we'll do a flash somewhere up there. So I want the three cameras to be equal in size, go use the equal constraint. So select these two. And I'm going to select these two. And then I'll give this one here a diameter, and that will make them all have the same diameter. So in this case, let's go for ten mil and let's position our first camera. Let's go D on the keyboard. We'll select center point here. Let's go to this line. Let's go for seven mil. And then center point here to this line. Let's also go for seven mil. Then this circle here is fully constrained. I'm going to put in a vertical constraint then between these two cameras. So centerpoint to centerpoint. Then I just need to add in a dimension from this point here, and we're going to go let's go to the same line or this point here. So this is going to be 15 plus seven, so that's 22. Let's enter. It's now fully constrained. Then as for this one here, let's dimension that to this one. And let's go for 7.5. Let's also go from the center point here to this reference point, and we'll do that at 13. We also want the flashlight to be vertically constrained with this center point. So I'll set the vertical constraint, center point to center point, and then just one more dimension to add. We'll hit in dimension, then more dimension this one. Let's go to this center point here. We'll give that dimension of 2.5. And also we need to give that a diameter as well. So select that one. Let's go for a diameter of four mil can be the smaller flashlight. That's now fully constrained, so we can finish that sketch. Then hit E on the keyboard, select our profiles, one, two, three, also the flashlight four. And we want these to extrude cut. In this case, so let's go four minus. Let's go 0.25, press Enter. And on here, we'll just put in the decals for the cameras and also the flashlight as well. Now we're on to the appearances. First of all, I want to give an appearance to this body and also a separate appearance to this extrusion here. Now, this extrusion, we actually did as a joining operation. So if we look at our folder here, we've only got one body available to us. But if we select this and we come down to our timeline, we can see highlighted here is this feature? Let's right click on this. Let's go into Edit feature. And then under the operation, let's select that, and we'll go on new body. And if we click Okay, you can then see we've got these two bodies here. So there's one and two. Now help us when we're applying our appearances. Let's apply I'm going to go for a powder coat blue for the body and then a powder coat red for this body here. So I hit A on the keyboard, and under my appearances, I'm going to come under paint, and then I'm going to choose powder Coat smooth. I'm gonna go powder Coat blue. So let's drag that across, and let's drop that on this body here, okay? We'll notice that body two is still the default color. And for that, I'm going to apply powder coat red. Drop that on that body. Close. Okay, looking good. And let's go ahead and add some decals. So the decos that I be using, these are just generic images that I got from Google, you're more than welcome to use these, and I will include them in the resource folder, so feel free to download them if you'd like. Unfortunately, they won't appear in your three D print, but just for visuals when three D modeling, they can be quite nice. So let's go on Insert, and let's go deco. And then I've input the three decels I'm using into the project folder. So I've got these available here. But if you have these images on your computer, feel free to insert from your computer. So first of all, I'm going to go with what I've called screen saver two, click Insert. We need to select the face. So I'm going to select this face here. Let's go on the front view and let's adjust this. So let's scale that up. We definitely don't want that to be chaining across faces. That looks very strange. Take off the chain, and there we see it's just on the one face there. Let's click Okay. I'm quite happy with that. I'm going to leave that as this, but feel free to play around if you. Then on the back, same process. We chose Decal, going to go for the camera lens, press insert, select this face. I don't want to be chaining this one either, so I'm just going to explode that. I'm just going to roughly position that, something like that. Okay. Repeat that process for the other two. I'll just speed up the video here. And then I'll just add the last decal for the flashlight. I'll speed up the video again. Okay, that's looking nice. And then there's one more I'll add to this space here, which will be the fusion logo. Okay, so I think that'll do. I won't spend too much time on that. Yeah, I hope you were able to follow along okay. And now we're ready to move on to our assembly, if it's something you want to do. But if you're three D printing, by all means, you can follow on to the next lecture or the next next lecture, which is when we'll export these as SDL files. So I'll see you in the next lecture. 69. Assembly of the Phone & Stand: Okay, so this would just be a quick lecture on the assembly of the two parts. It's not necessary for three D printing, of course, but yeah, if you'd like to have the assembly available, we can work on that in this lecture. So let's come up to the top. Let's go on plus go on a new design. And we're going to click on the nine squares at the top to open up our data panel, and then within there, you should have the two parts that you've modeled already. So yeah, depending on where you save them, if you could find that location. For me, I've got phone modeling tutorial and phone stand tutorial. I'm going to go ahead and put in the phone stand first. So we're going to ground this to the parent file. So in this design, let's right click, select Insert into current design. In terms of orientation, I'd like to rotate that by 90 degrees, like so. Let's press Okay. Looking good. Let's go ahead now and add in the phone. Right click on the phone, insert into current design. Okay. I'm just going to drag that away. Press Okay. And now we can use the joint command to position this in the center of the stand, and then we can adjust it manually. Sit J on the keyboard, and let's hover over this face. And in terms of the most logical joint, let's go for the one in the center. And then if we rotate, look at this face, we'll match that with this center point here. It's looking okay from the right side, so we need to bring it up on the stand. So use the arrow in this case, we're just going to draw that up until it's in contact. Just about so there. I'm going to click Okay. Have a look at that. That's looking nice. Yeah, that's looking good. I'm quite happy with that. So as per that joint, the phone is centralized on the phone stand. That is our complete assembly. Nice that we've got the logo in the back there. Just go to hide the object visibility under joints. I'm also going to change the visual style. Let's go and shaded. And let's go on the camera, go on perspective look. I think that's looking quite nice. Let's look at that from the right view. Yeah, that's looking good. Okay. There we go. That's our complete assembly. And so in the next lecture, we'll move on to exporting these as an STL file. And then if you'd like to three D print these, that's entirely up to you. Okay, so a nice and easy lecture, and I'll see you in the next one. 70. Export STL File: Now we can take a look at converting these components into STOs ready to bring into our slicing software for three D printing. So first of all, let's start with the phone stand. We're going to come over to the browser and where we've got our two components there, we'll go with the phone stand, right click on that. Then we're going to come down to where it says, Save as mesh. Left click once. And our toolbox pops up I want to make sure this is under export. In terms of object, make sure only that component is selected. Under the format, we want STL. That's the generic import file for slicing software. Unit type, this will draw out from the document settings, millimeters. Then under structure, we just want one file. Let's also have a look at the preview as well. So this will show us the STL format, in the case of triangles. And in this particular as per the refinement settings here, there are about thousand almost 4,700 triangles. If we go on the refinement settings, let's just have a quick look at these. So we see that the triangles and the complexities are all around the curvatures. And this is currently set at a refinement of medium. Okay? So if we bump that up to high, we'll see that our triangle count increases to almost 12,000, and you'll see there's much smaller triangles all around these complex areas here. But judging by this, on a medium setting, and based on the radius of these arcs, these curves, this should come up absolutely perfect on a three D printer. Wouldn't necessarily need to move to high refinement. But if you are looking for that better quality, might be worth jumping into high, and it would also depend on the type of settings that you're using in your slicing software as well. But overall, that's looking nice as an STL. I'm quite happy with that as a mesh preview. We click Okay. We can then save that. So I'm going to save that in my project file here, call that mesh STL file in my project file in the Cloud. I'm going to make sure that that's ticks. Don't need to save to my computer and then just click Save. And from there, you can access that file and import that into your slicing software and then over to you for three D printing. Thanks for watching and I'll see you in the next lecture. 71. Engineering Drawings Introduction: In this section, we will learn how to create two D engineering drawings manually in fusion. Fusion does have an automatic drawing creation option, but it's still in development and rarely outputs a drawing format that's considered professional. So first, we'll learn how to create a TD technical drawing from a design of a part or assembly, and then we'll study the drawing environment and take a closer look at how we can create custom to D drawing templates. Following that, we'll learn about drawing preferences, how to modify these, and how we can add dimensions, tolerances, parts list, and balloon identifiers. And finally, I will do a full tutorial on completing a TD engineering drawing of the Pulley assembly that we modeled in the assembly section. So let's start creating TD technical drawings. 72. Create a 2D Technical Drawing: In this lecture, we'll learn how to create a two D drawing using the default fusion template. And I'll also run you through the interface for the two D drawing environment. So to begin with, let's open up any one of our parts. So for this demonstration, I'll use this design here, which we did together from the three D modeling section. So if we want to create a technical drawing of this part, we can come up to the environment options, which are just the top left, and now we're currently in the design environment. Let's hit the drop down. And if we bring the mouse down to drawing, we've got two options there. We're going to select from design. So we want our drawing from the design environment. Left click there once. And within this toolbox here, we have a series of options which we need to select prior to clicking Okay. So the very first two are automatic and manual. Now, in this case, we're going to go for manual. Fusion has recently introduced the ability to create automatic drawings. However, unless the part is really simple, I would not recommend choosing this option. I think it's a nice feature. However, it's just not practical at this stage in its development. Feel free to experiment with automatic drawing creation, if you like. So that's where fusion will generate an entire drawing for you. But for this lecture and for me, probably about 98% of the time, so I always go with manual as it gives us full control of the drawing. So in terms of sheet count one, that's realistic. We only need one sheet for this part, and we can also add sheets later in the drawing environment. In terms of contents, so this is just one body here. Okay? It's not an assembly. And so for this case, we can just go full assembly or we can go select and then just highlight the body, which we want to display in our two D drawing. When it comes to assemblies, if you have got parts hidden and you only want to choose visible parts to be in your assembly drawing, you can choose Alexo or you can individually select them like we just did. So we can go select or full assembly and leave that as full assembly. In terms of destination, so drawing, yeah, we're going to create a new drawing. We don't have an existing one. And in terms of the template, we're going to go in this case, by from scratch. But if I hit the drop down here, you'll see that I've got one option. This is a custom title block that I designed specifically for this course, and we'll be covering that in a later lecture so you will then have the ability to design your own custom title blocks. For out, let's go with from scratch. Standard, okay, choose your recording standard there. I typically work in ISO standards. And again, with units, I typically work in mill, but feel free to change. In terms of sheet size, I'm going to go with A three. You can adjust as you need. And then we've got the width and the height there of this sheet in terms of its orientation. So, in this case, we're going to go for landscape, you can adjust like so. So let's go for landscape. And then let's press Okay. And welcome to the two D drawing environment. So very first of all, we can see as we move our mouse around, we have our part there. And in this particular orientation is the front view. And Fusion is asking us what location we want our front view to be in, and then we can project views from there and so forth. But for now, I'm actually going to click Cansel on our toolbox, as I just want to run you through the interface and show you the various tools that we have available to us. So let's start in the bottom left corner. Down here, we have our sheets. So we just have the one sheet available to us now, but if we do want to add more, we can just simply click the plus icon there. We can also right click on sheets as well if you want to delete them, rename them, duplicate them. And we can also export to PDF as well. And in doing so, we can either export individual sheets or all of the sheets within this drawing. On the left hand side, we have our browser, which is quite a bit different from the browser in the design environment. So first of all, let's have a look at document settings. Here, we can adjust our fonts, so we just select their change font. We've got the text height group, so size of the text. That could be dimensions, and it could also be any notes or any text that we add to the drawing as well. Dimension units, so we can adjust between mill and inches there, linewidth group, and also the revision scope. Now what we can do if we come under the font aerial and click change font, actually, all of those adjustments are available to us here. So for example, if you want to change the font, yeah, we can go under, let's just say area or black. Under the text height group, we can change that to, let's say large. Under the dimensions, so we'll go under units. We've got our units available to us there. So if I just change these as an example, press Okay, we'll then see that those changes are now reflected here. And likewise, we can do the same for the angwidth group as well. Moving further down, we have sheet one here, which we haven't renamed. We can rename that. So right click. Let's rename example sheet. Let's enter, and you'll see the name change will be reflected up there, and then any other sheets that we add will be listed here as well. Now in terms of the settings, hit the drop down there, and we have two objects here. The first is the title block, ok? So we can hide that visibility like so, recommend keeping it on. And we can edit this as well. So, for example, bring our toolbox across here, we can change the size and also change the orientation. And we can do that for any further sheets as. And then down here we have our title block, which is referring to this title block down here. Now, this is the default fusion title block, which I don't like personally myself, and I will be showing you in this section how to create your own customized title block. We'll be doing that together later. But we've also got the option to hide that, as well. We can also change that here as well if we do have other title blocks available to us. We'll take a look at that later. And along the tool bar at the top, if we start at the left hand side, and along the top, we have a series of tours available to us. If we start on the left hand side, we have our creation tools here, so these all relate to views, okay? So we'll run through those throughout this section, we've also got the option as well. If we want to add any sketches, we can create sketches similar to what we do in the design environment just with limited sketch tools available. Next, we've got the modified tour so rotate move and delete. Got some geometry tools, so this is where we would identify center lines, center marks, mark patterns, edge extension, and so forth. And under here, we have our dimensions. So the majority of dimensions we do we can do just with the general dimension tool, but it might be on occasion that we're looking for a specific type of dimension, in which case, we run through the list and select the according one. Next, we've got the text tools. So here we can add in some generic text or a note or a leader note. We'll run through those in this section. Then we've got symbols here. So if we identifying, say, surface finish, we've got our welding symbols and so forth. Got the option to insert images, very rare to do so, but it's there if we need it, and then we've got tables here. And this is where in this section, we'll be looking at parts lists and balloons, as well. And then the last is the ability to export. So we can export as PDF, for example, very similar to right clicking on the sheets and then exporting there. So that is the interface for the two D technical drawing environment. And in the next few lectures, we'll start to understand more about individual sheets, and we'll also start adding base views, projecting views. We'll be working with an assembly, and we'll learn all the fundamentals behind two D technical drawing. So I'll see you in the next lecture. 73. Customizing the Title Block: In this lecture, we will learn how to create our own title block infusion. Fusion supplies us with a default title block, as we can see here. However, this is very generic and may not include all of the part or assembly information that we need. So this sample here is a title block that I made in fusion. And in this lecture, I'll walk you through step by step how we can utilize the various tools that fusion offers to create our own title block. Now, some engineers would recommend creating a two D drawing template in another software such as Autodesk inventor or AutoCAD and then importing into fusion. But fusion has the necessary built in features to enable us to do this already. So let's begin. Let's jump into fusion, and we'll come up to the top left where we have file, hit the drop down there, and we'll select new drawing template. Left click once. You should see a toolbox pop up. And in terms of template, we want to select from scratch. You can then select your recording standard. So for me, going to work in ISO units. I've got imperial and metric. I'm going to stick in metric, then sheet size. I'm going to go for A three. Got our dimensions there, and in terms of orientation, I'll stay with landscape. Let's click Okay. And now we are in an environment to create a new template. So around the side here we have our border, and then just down here we have our title block, which is what we're going to be focusing on today. So let's say we want to add a new title block. We'll come over to the browser, hit the dropdown next to sheet settings and where we have our title block here. So if I hide that, then show it, we can right click on it and we can go new title block. Left click that once. And then with the toolbox here, there are three sources. We can create a title block from existing from scratch or from a drawing file. So we want to go from scratch. We're going to do this all infusion, and let's give this a name. Let's go for sample block. Okay. And now we are in a new environment where we are going to be sketching out the title block. So if we look at our tours at the top, we've got some very generic and basic sketch tours. We have our constraints available, modification tools, inspection tools. We've also got the ability to insert decals, as well, which is what we'll be doing today. So I'm going to sketch out the title block that I showed at the beginning of this lecture. Going to be referring to this. You're more than welcome to copy it and use it as it is, or if you're free to design your own. So let's go ahead and use the tools and me up this title block. So I'm going to sketch this out in the center of this environment. And then once that's done, once it's complete, I'm going to move it all down to the bottom right corner, which is where I prefer to have title blocks. But you can move it around the page wherever you like. So let's hit R on the keyboard then. We're drawing a rectangle. And notice here that sketching is a little bit different to when we're in design mode, and we cannot enter the parameters, let's say, the vertical, or the horizontal dimensions. When drawing out the rectangle, we can only do it with the dimension tool. So I'm going to roughly draw up that rectangle. I notice from my constraints that we have a parallel constraint between these two lines, we have a parallel constraint between these two lines, but a perpendicular constraint here. I want to make sure that this line here is horizontal, so it doesn't sort of shift and go at a funny angle. So left click there once. And for now, I'm also going to constrain. I'm going to use a fixed constraint on the bottom left corner to prevent that from moving anywhere. So now that's fully constrained. We can go ahead and use the dimension tool. I hit D on the keyboard. And first of all, let's dimension the width, which in this case, as per the drawing is 180 millimeters. Then we're going to go ahead and dimension the height, which is 60 millimeters. Let's enter. Then from here, we need to use the line tool, so I'm going to hit L on the keyboard. I'm I'm going to draw in a straight line. So I'm going to snap to this line here, but notice when I come down, fusion will not apply a automatic vertical constraint to this line, so we don't know that it's exactly 90 degrees, and it also gives it the ability to move as well. So I'm actually going to put an angle like so, and then I'm going to use the vertical constraint and apply it to this line, and now it's fixed vertical, and I'm going to give that a dimension as well. So this line to this one here has a dimension of 16 millimeters this enter. And then I'll use the line tool again and we can start, let's say, let's snap onto this line here and come across again, and go at a bit of a funny angle here. Use the horizontal constraint, constrain this line horizontally. Then I'm going to press D on the keyboard, then reference this line to this one and give that a total height of 40 millimeters. Enter. That's looking good. And now I'm just going to go ahead and input all of the other lines as per this current design, so I'll speed up the video for Okay, that's looking nice. I just want to take a quick look at a preview of this to make sure everything looks good. So let's go on the finished title block. Name you can see, yeah, that's looking fine. Got all my lines in there. All the spacing looks correct. Now let's continue editing it. So let's come under our sample block here so you'll see the name that we've given it has now appeared here. So right click Edit title block. And then from here, we're going to enter some text to identify each one of these fields here before we input the smart text. So to do this, we can come under our creation tools. We've got text here, shortcut T on the keyboard, or we've got the text option up here. So I'm going to hit T on the keyboard, left click once, and I'm just going to draw in a textbox, and I'm going to enter Title. Our parameters box, we can edit the font, the size, the color, and so forth. We can also add symbols where we need to as well. I click Close. I'm just going to repeat that process to identify the remainder of the field, so I'll speed up the video for that. Okay, that's looking nice. And next we're going to add the smart text or infusion, it's called attributes. An attribute is a property that relates to either a part or an assembly. So, for example, when we add a part in here, if we add smart text here, which is, let's say, the title, it will refer to the title of that part as it has been named. So whatever part or assembly we put in this file, it will pick up on that and always insert that text here. So it's really useful to have and saves us a lot of time in terms of editing the title block on every single drawing that we're doing. So to do this, we come up to our creation tools, and then we have attribute here of what's called the shortcut up there. Click that and then I'm going to enter the attribute under the title, and that is going to be, in this case, Title one. Again, we can change the fonts like so, click Close. Repeat that process, so I'm going to right click and select repeat attribute. So a bit of a shortcut there. Right click, and in our shortcuts wheel, we can repeat our last command. In terms of material, it the drop down, select material there, close. I'm just going to repeat this for all of the other fields as well that require attributes. I'll do that quickly now and speed up the video. I'm also going to add in some text here. This template will always be used for metric drawings. So I'm going to hit T on the keyboard and input a box there, put in millimeters in position there. Okay, and after we save this title book, we'll then create a new drawing and we'll see the Smart text, all the attributes working for us there. So here it will define the sheet we're on the first sheet of, let's say, five or the second sheet, et cetera, part number. That's relating to the model, and we'll learn how to adjust part numbers for models. Material. Yeah, we've got the title, who it was drawn by and the date that it was drawn, and then referring here to the scale. Okay, so I'm just going to finish title block there and make sure everything's looking good. It looks fine to me. Yeah, okay. Let's right click on that again, select Edit title block, and just two more images that I want to add here. So in terms of projection, we could actually sketch in the geometry for either first or third angle, but I'm going to choose to use an image that I just got from Google, and I'm also going to add in a decal over here and maybe add in some text here as well, about the tolerances. So to do decals, let's come up to insert and more select image. This will bring us to our Fusion library in the Cloud. So I'm going to try and find the fusion logo, which is good here. So all you can insert from your computer. Select my image and press Insert. And then you'll see that it's very much oversized, but that's okay. We're just left click once. We do have a toolbox here where we can adjust its position and also the scale. But I would recommend doing this manually. It's a lot easier. Click Okay there. Hold the mouse over the image. Then as we come to the outside of its border, we can select that. We can then scale it down with the corner points there. We can also position it. Oh, not that one. Control Z. Take the border. We can also position that. Yeah, like, something like that. That's looking good as our first decal, and I'll add another one for projection. A note here, when we created this template, we assigned the ISO standard, which utilizes first angle projection. And you'll see here that I'm using a third angle decal. But it's just to demonstrate the insertion of a decal. However, there is a lecture in this section specifically on first and third angle projections, and I'll show you how we can alternate between the two. Again, this one's very much oversized. I'm just going to click Okay, move to the border, left click once, scale that right down, and position it somewhere about there. Looking good. Let's just have a quick preview of that. Finish the title block. Yeah, that's looking good. Okay. Could make that a bit bigger. And our fusion logo. Yeah, that's okay. Right click Edit Title Block. And just one more thing I want to add in some more text. So I'm going to add in a textbox here. And I'm going to drop this text down. Let's go 2.5. See how that comes out. Type in tolerances. For linear, Let's go up 0.2 mill. Let's say some steelwork and angular. Let's go for 1.5. And I'm going to add a symbol here. So I'm going to drop down on the symbols, add the degree symbol, quite close. Position that roughly, like so. Okay, almost there, we just need to position this in the correct location on this sheet. So I constrained so I applied a fixed constraint to this corner here, which we now need to remove. So if you hole the mouse over here, we'll then see the lock constraint show up here or the fixed constraint. Right click on that, select the leak constraint. And now under the modification tools, I'm going to select move. In terms of my selection, I'm going to drag select around everything to move. Then we want to make sure that we transform point to point turned on. So we're just going to select this corner point here. And in my case, I'm going to snap this down to this corner point down here, like so. But feel free to move that wherever you like. And then when we click Okay, we'll see that everything has now moved over, and we can go on Finish Title Block. And there we have our custom made title block. The next thing we need to do is save it, and then we'll put it to the test. So first thing we need to do, let's click Save. Then we can name this appropriately. So we say sample, I'm going to put sample title block. And then we just want to make sure that the location is correct. So I'm going to put this in my engineering drawings folder under my project, but feel free to position that wherever you like, click Save. And now let's put this template to the test. Let's come onto a new design. And I'm just going to do a basic sketch here. Let's go on the XY plane. I'm drawing a circle. Let's go 100 mil hit E on the keyboard and extrude that by, let's say, 25 mil. We've got a nice disk there, okay? Go to save that file. Then we'll come up to design, come down to drawing, and then we'll go from design. And then in terms of our template here, let's go to our drop down. And you'll see we've got so here I've got the sample title block, and this is a separate one that I made, but this is the one that I just saved. So I'll select sample title block. Click this one. Then make sure we're under manual, and then click Okay. I'm just going to left click anywhere for now, so I'm just going to input the front view or the base view of this part. Click Okay. Then I focus is down here. So as you can see, the Smart text. So where it was here, so Title one has picked up the name of this particular part, which I call test. Okay, it's material. So it's using the default material steel, part number, and so forth. It's got today's date. It's got myname there, the scale, and also the sheet. So let's say we want to change some of these attributes, then. Let's go ahead and change the material on the part number. Let's come into this part. We modify going to change. Let's go physical material. And I'm going to make this. Let's go for a wood. Let's just go for a cherry. Close. And I want to change the part number. So I had to do this, come across to the browser, right click on the component, and then come down to properties, left click. And then here we've got the option to change the part number. So I'll call this wooden disk one, two, wooden disk one, two, three, four. Okay, click Close. Then we're going to save that Okay. If we come back to the drawing, we're being told you, there's a warning. So changes have been made referencing this component here. So come up to the top left and select this button here. So update those references. It's one of the fantastic things about fusion. A lot of it is automated. You can see here the material has changed to Cherry and the part number has changed as we named it there, WD 1234. And if we want to change the title of the part, we can come up to our data panel. Locate that part, right click, rename, call that wooden disks enter. Exit the data panel, click Update again, and then you'll see we've got the title change to wooden disk. So yeah, all automated. A part or assembly that we bring in to this particular template, the Smart texts or the attributes will pick up the according attributes and display that data here. That's a really fantastic tool instead of having to manually edit everything. I hope that all makes sense. And again, any questions, please don't hesitate to contact me, aside from that, I'll see you in the next tutorial. 74. Base Views, Projected, Section & Detailed Views: In this lecture, we will learn how to create base views, projected views, section views, and detailed views in our two D technical drawings. So to demonstrate this, I'm going to work with the assembly that we made in the three D modeling section. So if you would like to do the same, you're more than welcome to do so, or you can use your own part if you'd like. So let's take this assembly and make a two D drawing out of it. Let's come up to our Environments tab, click on the dropdown, come down to drawing, and we're going to select drawing from design. So from this design environment here, left click once. And then in our toolbox, let's definitely go a manual drawing. In terms of reference, I don't want to select the full assembly in this case. I want to give an example here where we exclude the fasteners. So let's go for select, and I'm just going to use the browser and select the base plate here for the bracket, second bracket, the rotary wheel, and also the pin as well. So in this case, I haven't got the fasteners selected. And if we hit the drop down next to them, you'll see they're unselected there. You can also see in the preview there. In terms of drawing, we're going to create a new, so we don't currently have a drawing specific for this assembly. So we're starting from scratch. And in terms of the template, let's also go from scratch, as well, but feel free to use any existing title blocks that you've made from the previous lecture. Let's stick with from scratch. The standard, I go for ISO, mill, A three sheet size, and landscape. Let's click Okay. And then as soon as we come into the drawing environment, you'll have toolbox pop up and we'll have a preview of the base view. So we can control that by this toolbox here. So the orientation of the base view now is the front view, which is very typical, but you can change these around if you need, so you can look at different sides, top and bottom, et cetera. We're going to stay with front for now. In terms of style, we've got the option for visible edges only. We can show hidden edges. We can do shaded and then shaded with hidden. But for the front view, it's very typical to go with visible edges unless you're doing something detailed where you need to show hidden edges as well. But for this, let's stick with visible edges. For the scale, so judging by the preview, it's very small here. Let's bump that scale up. Let's go for Let's go for 1.5. So one to 1.5 scale. I'm okay with that. Gonna be doing quite a few views, so I will need the space around it to work with. Terms of edge visibility, I want to demonstrate this by actually dropping this view just over here. So I'm going to left click once, and I'm going to select Okay. From here, let's zoom in a bit and double click on this view. And then here we've got the options to make any adjustments. And we can do that for any views when we're in the two D drawing environment. So double left click. Then under the tangent edges, I want to demonstrate the full length. So right now we've got tangent edges off. If I turn them into full length, we can then see any of these tangential edges. So if you recall as per the model, this is where a flat face will be joining a fillet, like so and that's represented by this line. And also, we've got the fillet down here. So showing this line here, we can turn them off. I recommend for this part that we turn them on full length as it better communicates about this part and the different bases. And for interference edges and thread edges, these are not applicable for our model, so we can leave them turned off for now. And then we've got the automatic center marks and center lines. So there are no holes showing in this face here, so no need to turn any of these on. In terms of center lines, we could turn on the round extrudes, and then we'll see that the revolve parts. So in this case, the pin and the pulley wheel will have a center line running through them. Click close there. Double click the middle mouse button. And there we have our base view. And we can move this around if we like. We hover over the view. Hold on the left mouse button. We can position that where we want. For me, I'm going to position that here. What's going to turn off the title block for this lecture. I need the space to work with. So turn that off. Close the sheet settings. Everything there is looking good. Okay, so we've got our base view in place. Now let's go ahead and add some projected views and get some more detail in this drawing. So if we come up to the top left, we have our creation tools. We're going to select the For me, it's the second one in the second one down, so shork P on the keyboard. That's the projected view. So if we select that, then we need to select our parent view, which in this case, is the base view. So if we pull the mouse out to the right hand side, we'll have a right view, a nice Io view there, top view, left view, and bottom view. Go with a side view, Let's also go with an IO view. And let's go for a top view. I think that will be enough views to detail this assembly. Then once we're finished, we can select the green tick here or right click and select Okay. Let's move this Io view, then. Let's move that over to the corner here. And let's change the visual appearance. So let's double left click on this. And under the style, we're going to click Shade. And in terms of the scale, I might bump this up a bit. So it's following the parent file one to 1.5. Let's bump this up too. Let's go one for one. Close. We got a nice ESO view there. I like to do the EO views in a shaded style. I feel that it better communicates about the part and makes it more easier to understand. Okay, and likewise, we can move the side view, but we will see here that we cannot move it up and down, and it is locked to the parent view, so identifying that it is, yeah, from the right. And likewise with the top as well, we cannot move it side to side, only up and down. Let's come onto the top view and you see we've got our extrusion holes here. Let's double left click on this. And under the center marks, these are defined as round cuts. So under center marks, let's select round cuts. I'll see you have the center marks there. That's good. Let's also do the same for the side view. But on the round cuts, plus closes looking nice. That's how we do projected views, nice and easy. And next we're going to take a look at a section view. So a section view is where a part is essentially cut in half, and then we look at it from the cut. So I'm going to demonstrate this on the base view. So first of all, we need to select our parent view, left click once and identify the start and finish of our cut. So I'm going to zoom in, and I'm going to try and snap to this line here and draw that up slightly, click once there, bring that down, make sure we're going vertical, and then click again. Take the tick. And here we have our section view, which I'm going to put to the side here. I'm going to leave all of the parameters as default. I'm happy with that. Press Okay. I'm going to move this up slightly. So here is our section view, and that's labeled AA. And as we see, by the cut line, we've got AA there, and the direction of the arrows indicate that we're looking at this view from this direction. So we're looking towards the right, if that makes sense. I'm going to drop this down to the other side. We can move that around. And it also indicates the style as well. We can modify this if we like, so we can double click and adjust accordingly. And perhaps also, we want to have some center marks on the holes here. Okay, that's looking good. And wherever the cross section will intersect a solid body, we'll have this nice hatching appear there. So we know this hatching is coming from the pulley wheel and this hatching here is coming from this material here. Okay, so we've done the base view. We've done our projected views, and we've also done a section view. Next, let's take a look at a detailed view. So this is located up here, so the fourth one in or creation tools. It is this one here. I'll select that. The detailed view is literally just an exploded view of a particular area where we might want to indicate more detail. So for this assembly, I wouldn't say it's really necessary, but zoom in on the base view or select that as the parent view. Then we need to identify the center of our detail view. So if I choose this point here and expand out that circle, so we go for this. Left click once again. I'm happy with that. We can then see our detail view, which we're going to drop down here. On that scale to bump up a bit. Let's go for one to 0.5. Let's put that in here. That's okay. You can see that's labeled or identified as section B with the according scale there. And just here, we might be wanting to communicate about the assembly in terms of the distances between the bodies, let's say, the pulley wheel and the pin and how that mounts with the bracket as well. One thing to note in this lecture is that your views might look slightly different to mine. And that will be because they're being projected in a different angle, and it's something that I'll cover in the next lecture where we'll take a look at first and third angle projection. So I look forward to seeing you there. 75. Switch Between 1st and 3rd angle Projections: In this lecture, we'll learn how to switch between projection methods, first and third angle projections. When working with the IO drawing standard, the default is first angle, and for ASM is third angle. But fusion allows us to override these should we need. To differentiate between the two, we can refer to this diagram here. It's a slightly tricky concept to explain, but there are some brilliant videos on YouTube that you can refer to to get a better understanding of it. So if we look at this image here on the left hand side, we have first angle projection. So we can see that the front view is the same front view as in third angle projection. Only the projections differ. So, for example, the top view appears beneath the front view, and the side view appears to the left, whereas it's the opposite for third angle projection. So that's a very simplistic way of trying to explain it. But by all means, please refer to the YouTube videos for a better explanation. So let's learn how to switch between the two infusion then. So I've drawn up a basic part here, and I want to check if I now start a drawing, what projection angle is going to be used. So to do this, we come up to our profile at the top, we're going to left click on this, and then we're going to go under preferences. Left click there. And then we have many, many tabs and options here. I'm going to close a few of these down. We want to come under General, and we are interested in the drawing section under General. And at the top of drawing, we'll see the standard. So in this case, I've got IO selected. And in terms of the projectiing angle, it's first angle. Now, we can't override these, okay, by ticking this box, and then we can adjust like so. But I'm going to leave that as the default for now. Click Apply, Okay. Going to go into design drawing. Let's go from design. Make sure this says IO, okay, create new from scratch. Okay? If I place the base view, click Okay, hit P on the keyboard and project. I'm going to project my base view. If I come down, we'll then see the top view. I come to the side. We'll see that side view and this view here. So this is first angle projection in accordance with what our preferences are currently. So to change this, we'll need to exit this. Okay? Don't save. Come back into our preferences. We're going to override this, and we're going to stake this as third angle, apply, okay. Going to repeat the same process, drawing from design. Make sure it's an ISO, okay. Put in the front view, P on the keyboard, and then give a top view, side view, and the ISO view. We can see now that we're working in third angle projection. So we can control this from coming into our preferences and overriding if we're working on ISO or we can conform with the ISO or ASM, depending if we want to work in first angle or third angle projections. So just a quick tip there. I'm sure that will help, and I'll see you in the next lecture. 76. View Styles, Labels, Leaders: In this lecture, we will take a look at views styles, labels, and leaders, and how they can be used to support us in the creation of two Di technical drawings. So to demonstrate this, I've drawn up quite a simple part here. I've just got a block with a taper extrusion, and in the center there, we have a countersunk tapped hole. So let's move over to the drawing of this. I've input a front view, a top view, and also an Io view, and this is in third angle projection. We've briefly covered the view styles already, but I just want to visit them in a bit more detail and see where they're more practical to be used. So, for example, if we take a look at the front view, if I double click on this, we have our styles here. So right now this is the visible edges style. So we just see the visible edges according to the orthographic perception of this view. We select visible with hidden edges, we'll see now that we're showing the hidden edges in dashed lines relating to the countersunk hole. And that can be really useful for indicating perhaps, in this case, the depth of the countersunk regardless that we would later dimension that within the details of this feature here. But in this particular drawing, this could just be that extra bit of help for communicating the full depth or in this case, a through countersunk hole. Double click on that again. And the next style we have is shaded. So that's as we see up here in the Io view. That's the shaded appearance. And this to demonstrate actually, I'll do it on this view here to demonstrate the shaded with hidden edges. It's very rare to see this, in fact, but doing this on the front view, we then see it shaded with the hidden edges there. And if we do that on the Io view, it will then see the hidden edges, so forming the remainder of the block and also the details as well of the countersunk hole. So I'm going to revert this back to shaded only. And I'm going to turn this one I'm going to keep on visible with hidden edges. I think it adds some extra value to show that detail and so those are the view styles. And we can use these as we like to better communicate about features that are hidden in any details that we need to get across. Next, let's move on to leaders. So here we're going to be looking at the text tools. So we've got generic text, shortcut T. We've got notes, leader notes, whole and thread notes, and bend notes. So let's start with text. We can hit T on the keyboard, perhaps we might want to label this view here. So drawing a box. I'm going to increase the font size there. Let's go for 4.5, and I'm going to type in front view, centralize there, and then we can move that around just holding down the left mouse button and dragging. I'm going to repeat that for the other two views. And it's quite common to use the text tool for notes as well. For example, if I make some text down here, add in some notes, let's say, tolerances, XY z, no sharp edges or burs, et cetera. And the next tool available to us is the note. So N on the keyboard, we can select onto any edge and identify some details there. So perhaps we might want to, let's say, click onto this edge there and identify the taper. So let's say taper, I think it's 15 degrees. Let's put the degrees simple there, press close. Give me an example of where we would use the note. Another common use for the note as well. So if we select that, we can then click, let's say this feature here, so the countersunk details. Instead of manually writing this out, we can just click on one of its edges and then click our leader there, and fusion will automatically pick up on the details of that feature and then add them in like so. So we've got our 18 mildiameter countersunk, 90 degree countersunk, and the tapped hole is 12. We've got our pitch thread, six H class, 21 depth. And if we want to edit this, can double left click and make any edits from there. And next, we have the leader note. So an example how the leader note difference from the general note is that it won't pick up on any features. So if I repeat the same process for this countersunk hole, we can just write empty text in there and it will not pick up on any features there. I very rarely use that. We've also got the hole and thread note, and this is only really useful for where we have some really complicated geometry, a lot of entities and a lot of lines to select. And in this particular case, notice that we cannot select any other edge or line here. We can only select existing holes or threads, nothing else. I cannot select any of these edges, but I can select these here. So yeah, likewise, we repeat the same. But in most cases, I would just do that with the note tool. And the same is also applicable for the bend note as well. So if we click this because we have no bends in this part, notice that we cannot select any of the existing lines here. So there's a quick overview of the notes and leaders. The most commonly used one is the note, unless we're working with something really complex where we might want to use the hole and thread note or the bend note. And I'll see you in the next lecture. 77. Adding Dimensions & Editing Drawing Preferences: In this lecture, we'll take a look at the various dimensions and how we can change our drawing preferences. So to demonstrate this, I'm going to be using this bracket here. And if you'd like to draw the same, then please refer to these dimensions here, and you can model that up. I think that's quite a good exercise at this point. And if we take a look at this part, it's fairly generic. We've just got one extrusion. We've got four threaded holes, and we've got the simple hole in the center with no thread, and then we have these two bosses on the outside. So let's create a two D drawing of this and apply some dimensions to it. So before we create a drawing, let's check, first of all, what our preferences are when it comes to drawings. Let's come up to our account at the top. I'm going to select preferences Left Quick once. Then in here, we want to come under general and then if I just hide all these to come down to drawing here, make sure that's selected, and we want to check that everything here is correct. So this is all good, and under the projection angle, I'm going to go, in this case, from third angle. So make sure you've got this tick box checked. They will let you overwrite the default ISO standards. Under linear precision, we can state there how many decimal places we want to show. And we can also adjust this independently for dimensions when we're in the two D drawing environment, which I'll show you in a bit. Also, in terms of the point, so I typically use a decimal point, you can change to comma, as well. I'm going to stay for decimal for now. Just click Okay. And now we can come over to the environments tab, hit the drop down, go on drawing from design. Then in our toolbox here, make sure we're under manual, to create a drawing from scratch. Going to go with the IO millimeters, A three sheet size, and landscape orientation. Click Okay. Let's go ahead and add a base view. So this is quite small for this sheet size. I'm gonna bump up the scale. Let's go for one to 1.5. Input the base view. Click Okay. G to hit P on the keyboard. So project, select this view here, put it in a top view, go to put it in a side view, and I'll put in a icer view as well. Hit the green tick, move this over here, double click on this. Put that in shaded, close. And on the top view, I want to show the center marks for all of these holes. Double left click under center marks, select hole. Then you'll see there that the four holes. I've used the hole feature, so they'll have center marks. And then also I want to include the round cuts as well, which is just the simple hole in the center. Click close. For the base view and the side view, I want to keep the hidden edges on. I think that's quite valuable detail to show, considering it shows that the holes here are through. We don't have to label that either in a leader or a note. So in terms of dimensions, if we come up to the top, we have the dimensions tab just here. We hit the drop down there, and we'll see there are many different dimensions available. However, in 95% of cases, we only need to use the general dimension tool, which is D, and that enables us to use the vast majority of different dimensions here, and we can change between them. But in some cases, we might want to use some specific dimensions here, such as the arc length dimension. So mostly, we're going to be using the dimension tool, and Fusion also has a auto dimension tool built in. So if I select this, let's see how it comes out. As this part is fairly simple, fusion, in this case, has done quite a good job of dimensioning this part, although it's very hectic. And definitely when we're working with more complex parts, if we're using auto dimension, it can look really messy on our sheet. But in this case, we're not going to go with auto dimension, but that feature is available if you want to use it. Let's jump in and apply some dimensions then. Let's hit D on the keyboard, so general dimension. And I'm going to apply a dimension for the total length of this part from this corner here to this corner. So very simple, just left click once on the corner and left click once on this corner. Fusion will identify the distance according to the pot we drew. Then we just quite simply left click once to input that dimension. Let's do the same for the extrusion height. So this point here to this point, put in the ten. Let's do the same as well from the total length from this corner to this corner. So that is essentially the distance from this face to the corresponding opposite face over here. So at this corner point, this corner point, click here. And as we see in this dimension, there is one decimal place. So we've got the 0.5, whereas we don't have that reflected over here. And that's because these dimensions don't have any decimal places, and so fusion will automatically pick up on that for us, which is quite handy. In this case, if we did want to remove the 0.5, I don't see why we would, but we can do that by double clicking on the dimension, and then we can make any changes here. So, for example, under linear dimension, if I put that to zero decimal places, we'll see now it's just 141 in this case, so it's rounded up. But I'm going to put that back to well, the default is two decimal places, but in this case, we only need 0.1. So I'm going to go with the default, press close, and then we have the dimension. Let's move over to the top view. So this is where most of our dimensions will be to D on the keyboard and have a look at this radius here. So what's great about the dimension tool we'll pick up this is a radius and therefore give it a radius. And so we don't need to then go into the dimension tool and select and specifically select the radius dimension. We can just use the general dimension tool, and fusion will pick up on that. We can left click once place that dimension where we want. Let's take a look at this circle in the center. So if I hit D on the keyboard, fusion will recognize it's a circle and apply a diameter. However, in the case that we did want to apply a radius, it wouldn't be possible to do so in the dimension tool. So instance like this where we might want to specifically select radius dimension, and then any item we select such as this here will be displayed then as a radius. I'm going to use the dimension tool, put in a diameter there. It's 25 mil. And then we can add the other dimensions to confirm the position of this. Let's go from the center point then. Let's go to this point here, add in this dimension. Again, from the center point, let's go to this point here. And you'll see here that the dimension tool is giving us an aligned dimension. And what's great about this tool is that as we move the mouse around, fusion will adjust the dimension accordingly, so we can put in this dimension here or this dimension, and we can move the mouse around like so. So I'm going to go with the dimension that we're after. In this case, 90, drop that in there. Let's also do a distance from this line here, so select that line to this line, draw that across, and then you'll see we've got the one decimal point there. We can go back and edit these dimensions as well. So let's say this one is 90, we've got no decimal places, right? We can double click on that. And then under the linear precision, we're showing two decimal places, there's no trailing zero selected. So if we select trailing zeros, perhaps close, we can then show those trailing zeros specifically for this dimension. And we would only use that if you wanted to highlight some fundamental information that was perhaps a unclear otherwise. Now if we move on to dimensioning up these threaded holes here, let's use the dimension tool, zoom in on one of these. As we bring the mouse over this arc here, we'll see it's giving us a radius, and we've got a diameter on the inside there. But that's not the detail that we want to get across about these threaded holes. So in this case, we wouldn't use the dimension tool and we would use a note. So we'll come back up to, in this case, we're going to use text. We're going to select note. We're going to click on to this hole here, drag that out. Left click once. That's o on the toolbar. Now you see we've got these four holes here, all ten by 1.5 thread class six H. So I'm going to go ahead now and add the rest of the dimensions for the part, very straightforward process, and I'll speed up the video for this. And we can also add in angles, as well. So, for example, where this boss sits off this line here, we can use the dimension tool by selecting this line and this line, and then you'll see it'll give us that angle to add there. We can drop that in. Or alternatively, we could come under the dimension, and we could add a angular dimension, which will only pick up on angles. So if I select these two lines here, we've got that angle there. So that's an overview of the dimension tool. It's nice and simple to use. Again, for very simple parts, we might want to use auto dimension, but as I say, 95% of cases, we end up using the dimension tool. And only if we had a lot of entities and perhaps complexity on our part, we might want to specifically identify the type of dimension that we want to give. And so I'll see you in the next lecture where we take a look at adding tolerances. 78. Adding Tolerances: In this lecture, we'll learn how to add tolerances to our dimensions. So in two D technical drawings, it's very common to see general tolerance stated. So I'm going to go ahead and add in a general tolerance guideline, and I do that in the title block. So here we have our general tolerances, which are applicable to every dimension within this drawing. So our linear has a tolerance of plus or minus not 0.2 and our angular plus or -1.5. But let's say, for example, that we had a dimension which was critical and differed from the general tolerances. We can state that specifically along with the dimension here. So, we're going to choose this one in this case. So this dimension is from this face here to the face on the other side. Let's go ahead and double click on that. And then in our toolbox, if we scroll down, then we'll get to the bottom where we have tolerances, select that. In fusion, we're offered three different options, symmetrical deviation and limit. Symmetrical is a simple plus or minus value. So in this case, the tolerance let's say a tolerance of 15 there differs from the general. So we've allowed here for a tolerance on this linear dimension of plus or minus, no 0.15. So in this case, the upper tolerance would be 140.65, and the lower would be 140.35. That would change that to deviation, and this is where the upper and lowers differ. So let's say the upper was, let's say we're allowed for 0.3, but the lower we would only allow down to 0.15. So in this case, we would have 140.8 as the upper tolerance, and then the lower would be 140.35. And the last option we have is limit, and this is where we just state the upper tolerance, so 140.8, and the lower is 140.35 as per the limits that we've input here. So that's how we add tolerances to our drawings. Nice and simple and really helpful for when we need to deviate from the general tolerance, and I'll see you in the next lecture. 79. Parts Lists & Ballons: In this lecture, we will learn how to add a parts list and also balloons to our two D technical drawings. So to demonstrate this, I'm going to use this assembly here from the creating assembly section, so feel free to do the same. And let's create a drawing. So come over to our environments, and we'll select drawing from design. I'll leave everything as default here, make sure that's manual. Coming of ISO, size 83 and a landscape orientation. Let's click Okay. Then as always, we need to enter in a base view. I don't particularly want to use the front view for this viewpoint. I want to use Near isometric. I'm quite happy with that, but we need to bump up the scale. Let's change that. Let's go for 0.75. Yeah, that's a good size. Okay, so left click once there. I'm also going to change the style as well to shade it. Click Okay. And there we have our full assembly. And now let's go ahead and add a parts list. So to do this, we'll come up to the tools at the top and where we have the section called tables. We can hit the dropdown. We've got the general table, custom parts list. Got the option to add balloons and various other tables in here as well. But to keep this simple, we're just going to select table. Then our toolbox pops up, and in terms of the type, we hit the drop down there, we can choose one of these. We're going to go for parts lists in this case. I leave the structure as first level. We can title that differently if you want, but I generally leave it as a parts list. Then left click anywhere in the environment. That will give us our table, and simultaneous to that, fusion will automatically add balloons, identifying each one of the parts, although these are very messy right now, so we'll definitely tidy those up. And if we look at the table, as fusion has input it, the information is kind of very cluttered and together. It's quite bunched up. So we definitely want to make some edits to this. There are two ways we can edit these tables. So if we hover the mouse over the parts list and then left click once, we have the option to adjust any of the columns and also to reposition it, as well, and notice that it will snap into corners like so. And another way to edit this is to hover over and double left click until we have our toolbox here. And here we can change the title structure table direction. So currently it's down. If I change it to up, have the titles at the bottom, and then item one, two, three, four, five, six, leave that as down typically how I work. I'm also going to add the description in. We can adjust the position of any one of these. For example, if we wanted the description to be before the parts number, we just select that and then move that above the parts number like so. But for me, I'm going to leave that after the part number, click Close. So I'm just going to drag that over here and let's look at the information we have. So in terms of item one, two, three, four, five, six, these item numbers here correspond with the balloon numbers. So item number one, have our part number here. That's the Pulley base plate and carbon steel material. Then we have that item number one here pointing to the base plate. We've got the quantity. So yeah, we've only got one base plate. Atom number two is the bracket arm, so two of those, one wheel, one pin, and four fasteners, the hex head bolts, and four of the washers as well. Then the part numbers here. So we did cover this in a previous lecture, but I'll just show you quickly how to add a part number. Let's take the base plate, for example, if we want to add or change the part number, come across, right click, go on properties. And then here we can adjust the part number. We can also change the description as well. We're going to leave that as it is for now. That's all good. Let's go back to our drawing. And then finally, we have the material. So again, to change this, if I jump back into the base plate, go and modify, come down to physical material. And then as we see here, I have carbon steel assigned to this base plate. So all of that information relating to each other parts will be brought from their part files and input into this table here. So now I will adjust some of the wicks of these columns and we'll position it in this corner here. So I'll left click once track this column out. Also same for this one slightly, make these ones slightly bigger. Track this one out, as well. There we go. Okay, quite happy with that. So I'm going to left click on it once, select the corner point. I'm going to track that over until I snap into the corner there. That's our parts list complete. And now let's focus on our assembly here. I'm going to track this over here. In terms of the balloons, so if we left click on one of these, we can track this, like so. I'm gonna put four, five, and six over here. I'm going to tidy all these up. Let's take a look at number one first. This is our base plate. Move this one over here. So again, just left click and dragging. And in terms of the arrowhead, again, same process, left click and drag, we need to make sure that it snaps on to the right part. So we don't want to snap onto this part, in which case, it will become number two. Snap that back to part number one base plate. That's correct. Part number two, let's leave that as the bracket. Then the wheel, bring that down slightly. Okay. But number four, we've got our pin, okay, bit of an awkward one to snap to. Let's try and move this arrow. Let's go to this edge here. That's good. Then five, we've got the hex head bolt. Let's bring this down somewhere here for now, and then six. Let's drag this one across to the washer to make sure that actually snaps on to the washer and not to the bolt. Okay, there we go. So that's how we add the parts list also to add the balloons, make any necessary adjustments or modifications, and I'll see you in the next lecture. 80. Example 2D Technical Drawing: In this lecture, I will use all of the tools learnt in previous lectures to create an entire two D technical drawing from this Pulley assembly that we drew in the creating assemblies section. So this is a five page document, and on the first page, we have our assembly model here with the parts list and the corresponding balloons labeled here. On the second page, we have the base plate all dimensioned up, and we've also got a tolerance there as the width of this base plate differs from the general tolerance. On the third page, we have the bracket arms, so two of these in total within the assembly. On the fourth page, we have the pulley wheel itself. We've also got a cross sectional view, which is titled AA. So that's referring to the base view here, section AA. And on the fifth page, we have the pin, nice and simple drawing for us there. So let's go through step by step and create this entire drawing. First of all, let's open up the assembly itself. And then from here, let's come over to the environments. We'll had the drop down, go down to drawing, and we'll select from design. In our toolbox here, I want to make sure we're under manual. Keep the contents as full assembly. We will include the fasteners, as well. Drawing, create new template from scratch. Gonna do an IO drawing, in this case, Units millimeters sheet size A three, and I'm going to do this in the landscape orientation for each page. Click Okay. Et's start by inputting a base view. So on our first sheet, we'll have the full assembly. So for this, I want to use a isoew. So I'm going to change the orientation here. I do this NI isometric. I think that's the correct view. Yeah, that's the correct view. Just need to bump up that scale. Let's put that. Let's try 1.75. I think that's a good size for this sheet. I'm also going to change the style to shade it, as well. Okay, I'm going to place that there. That's okay. That's looking nice. Now let's add a parts list. Come to tables, and I'm just going to hit table. And in terms of type, make sure parts list selected, leave everything else as default. Drop that in there. I to do some edits to this one. Let's double click on this, and we're going to insert the description. That's in the right location. I change the font of this come into document settings under our font. Let's change this too. Let's go for aerial. It's okay. It's looking better. Move this over here slightly. I'm just going to change the size of these columns, so I left click once. I pull out the material. Then let's drop that into the corner. So I'm going to choose the arrow point here, snap on to the corner. That's looking good. Let's hit T on the keyboard. Let's title this view. Let's good for ISerview, center there, press closes, trp positions okay. And now let's adjust these balloons. In order to align these balloons. So vertically, we pull out this one, for example. If we then pull out the two and bring that near to the one, it will snap to the one. And then if we bring that up, we can see we've got that alignment there. I'm going to do the same process for balloon number three, as well. Okay? Something like that. They're nicely aligned. Let's do this same for the other side and tidy this That's looking good, quite happy with that. Let's put in the general tolerances. So in terms of the title block, I'll be using the generic one associated with the ITO standard. But when creating the drawing, feel free to use your own. So I'm going to come over to the sheet settings, hit the drop down, right click on the title block. Then I'm going to select Edit Title Block. Let's click Okay. Let's T on the keyboard instead of textbox like so. Okay, so linear tornce plus or -0.2 mil, and angular tolerance, pussle -1.5 degrees. Let's finish the title block there. And we can later apply that to all of the other sheets as well. Double click the mirror mouse button. And let's go ahead and create the remaining sheets. So we've got five in total, so we're going to add four, one, two, three, four. And let's come back to the second sheet, which is our base plate so you can right click on these and rename them. I rename this base plate example. I'll do the same for the others as well. Assembly. Let's come under the base view then. So up here, let's click Base view. We want this to be the front view. We're going to bump up that scale. Let's go 0.75, left click once there, press Okay. We only want to be showing the base plate. So let's come over to our browser where we have the pulley wheel assembly here. We want the base plate to be showing. But the bracket, I'm going to select that hold down Shift and select the pin. I'll select all of them. Right click, suppress those. Same process for the fasteners as well. Left click, one of those, hold down shift left click the last one, right click, suppress. Now we're just left with the base plate. Pee on the keyboard, do a projection. Let's project this view, do a top view. Let's go for a side view and ISO view as well. Io let's make that shaded. And for the front view, I feel that it would add value just to clarify that these holes here are through holes. So for this, let's show the hidden dimensions. St close. Now this side view relates to the base view, but I don't want to show the hidden dimensions there. They don't add much value. So I just go visible edges only, rest close. That's looking good. I'm going to title these views up. And now let's start adding some dimensions. Let's hit D on the keyboard. Let's do the side view first. So this will go the overall height. Let's go this point here to this point here, but our ten mil. Let's come over to the side view and start defining these depths of the cutouts. Select this point here and this one, place that in there too. I'm just going to reposition that. So left click once, hold down on this pointer, drop that there, move the base view slightly. Let's D on the keyboard again, then from this height to this height to define this depression and going to bring this out there. Right click. Okay, that's good. Double click mirror mouse button. On this view here, we want to identify center marks for our holes, double click on them, under center marks, select hole, click Close. Let's press D on the keyboard, then give this a height. So this point here to this point, and this one has a tolerance that differs from the general tolerance, so we'll do that in a second. Also still in the dimension tool. Let's give the overall width of this. So this point to this point. We're going to bring this up here. And then we'll add a few other horizontal dimensions as well. Again, refer to this point. Let's go to the center point of this hole here, like so, bring that up there. Let's move the mouse, ten. Again, this point here to the point of this base, bring that up. Let's go 30 and this point here to the point of this boss. Bring that up 70, bring that 100 up as well. Bring that top view down slightly. Let's also add the other details. So in terms of this hole, press D on the keyboard. We're going to center point to the top vertical, put in that dimension there ten. We also need to identify these holes here. Now, we don't want to apply a dimension here, but rather a note. So hit escape on the keyboard, press N on the keyboard, and then select the hole here and bring that leader out left click once. Press okay. We've got identification here, so four holes, diameter eight through, simple, no thread. And then let's give this fillet a radius, as well. So we hit D on the keyboard, select the radius. Fusion will pick up that we want to define a radius here, just judging by a fillet. Looking good. Let's double click the mirror mouse button. And then we have our general tolerances down here in our title block like we added from the first sheet. And now we just need to add in the tolerance specific for the width, in this case, 50 mil. Let's double click on that. Let's select tolerance. And we're going to go with a symmetric tolerance of plus or minus. I think it's 150.15, quite close. Got that tolerance display there. That's and there we have the sheet for the base plate and feel free again to adjust the title block if you're using the default IO one. Before we continue, let's make sure that we hit Save and just double check the location. So that's in my project file while creating assemblies, which is the location of the pulley wheel itself. Let's click Save. Now let's move on to the bracket arms, so we'll select that sheet. Again, let's go with base view. And for the front view, I'd like this to be either from the right or the left. Let's go with the right. Bump that scale up as well, 0.75. Actually, no, let's drop that down to 0.1. Drop that in there. That's okay. Let's suppress the parts we don't need. So we want to keep the front bracket, which is this one, but select the others right click. Suppress. And that's the same for the fasteners as well. So left click once, hold down Shift, left click, right click, suppress. And then let's project some views. Pee on the keyboard, select this view. Let's do a top view. Let's do a side view and an ISO view as well. Might actually change that scale again. So I see how it looks 1.75. I think that's okay. Let's go with that. This in a corner. Let's go for a shaded appearance on that. Click close. Let's also show the hidden lines on this drawing. Show the through holes. Then, likewise, we can see them on the side view and also for the hole at the top, as well. 's double click this view. Let's have our center marks turned on for the whole features. And the same process for the top view, as well. Turn the center marks on, close. That's good. I'm gonna title up these views. Okay, let's start on the front you then, hit D on the keyboard. Let's first of all, dimension up this radius here, 15. I'm going to bring that dimension out slightly left l once, draw that out so hit D on the keyboard. Let's go for the WIC then. Let's go from this point here to this point. Got our 20 in there. Let's also go for the radii here. Ten. I'm going to bring that out slightly. And then as this as a hole feature, let's hit N on the keyboard, put in a note for this hole here, bring out the leader right click, diameter eight. And it's a through, in this case, or eight mil, which is the thickness of this body here. Let's move over to the side view. Let's hit D on the keyboard and define the depth. Let's go from this point to this one. Drop that dimension in there, and then a few vertical dimensions. I want to dimension this side here eight. Also the dimension here to the center point of this hole here. Let's go 58 and also this point here to the very top as well, 68. Let's also give the dimension as well for the width of this, eight mill, point to point. Looks good. Then let's define an angle here. Let's go from this line to this line. We could define it on the inside there, but it does conflict onto the model itself and it's generally advised to keep dimensions outside of the part. So I'm going to go with a 120 there then we can easily recognize that it's just a 60 degree remaining to make up the 180, giving us this angle here. Double click the middle mouse button. Now let's work on the top view. I'm going to adjust the front and the side view slightly. Okay, give the top view. So more space. Sit D on the keyboard then and go for the width, this point to this point. At 50 mil in there. We've already defined this thickness here is eight mill, so that's on the drawing there. We just need to go from this point to this point here and define this. So we got our 22 there, and then let's do the holes. So center point. Let's also reference this point, ten mil. And from this point here to the center point, we should have another ten. Let's give this fillet a radius, eight mill there, and then for the holes, we're going to use note, suppress N on the keyboard, select the hole, bring the leader out, two holes, both diameter eight, and they're both through or eight mill thickness, which is what we've defined down here. That will left click, the middle mouse button. Then just one more dimension that we need to add is the thickness of the rib. Move this top view out of the way. Let's move that over here, hit D on the keyboard, point to 0.6 mil. Put that identification back. Yeah, somewhere there, double cocking middle mouse button. That's looking good, quite happy with that. I adjust the base slightly. There we go. That's it, save. And let's move on now to the fourth page, which is the Pulewheel. It's the same process. Let's do a base view. And I'm going to flip the orientation of the base view to take a look at the left orientation. That's looking good. And again, let's bump that. Scale up. Try 0.75 again. That should be okay. Gonna left click on, okay? And then supress those parts I don't need. Same process. Go hold down Control. Select the parts we don't want to show, right click, suppress, and same for the fastens as well. Hold down, shift, right click and suppress. Let's now do some projections, hit P on the keyboard, select the base view. Move up to the top. Let's get a top view in there. Let's get an IO view in there as well. Green tick. Let's have the cross section as well. Come into the section view. First of all, select the base view as being our parent view. In terms of points, I want to select the very top quadrant and the very lower one here. Okay, on a right click, continue. Let's put that view just to the side here, okay? I'm just going to move these arrowheads. I don't like them so much conflicting with the part itself. So hold down on this point, they're here. Same process for the lower one. Looking nice. Move that. Let's take this icer view in the corner. Let's put that on shaded flows. Double click on our base view as well, let's get these center marks in on all of these holes here. Select that hole. Okay. We have our center marks there. That's good. Let's also put in a center line to define this hole here. So I'm going to use the centerline to under geometry. That's like my first edge here, second edge here. Looks good. Go to label these views up. Let's T on the keyboard. And for the cross section view, that's already labeled up as section AA. Now we can go ahead and start adding some dimensions. Let's do the top view first, fairly straightforward. D on the keyboard then. I want to come to the center point of this arc here, indicating that groove moving around the pulleys like this point here. So we know we'll to sketch that and then the overall height as well. It should be 30. Okay. We'll do it outer diameter, 60. Then let's radius, this arc here. So as we select this using the dimension tool, fusion will be using the diameter dimension. However, we want to be using the radius. So as in a case like this, we'll go to the dimensions, select the radius dimension, and we'll just select that radius there, put in the radius one, double click Middle mouse button. Okay. That looks good. Let's go ahead and define the pitch circle diameter for these holes here. So to do this, come under geometry. I like the center mark pattern. And we'll select this circle and this one. Okay, happy with that, leave everything as default. Press Okay. Actually, let's double click on that, and let's also add the center mark as well. This is a through hole here. Press Okay. And now let's dimension this up. Let's D on the keyboard. Give the PCD a dimension. So 41. And these holes here, let's hit N on the keyboard. I did these using the hole command. Let's select that edge there, bring that leader rout. So six holes in total, three mile diameter. And they're all through, as we can see in the cross sectional view here. It's also the center lines there whilst we're at it, center line. These two. Same process. These two. And finally, that's dimension the section view. D on the keyboard? We'll start from the center line of the through hole. And we're going to use a series of dimensions working our way Okay, there's a dimension there. So sent a line through hole, center line for these holes, as well. In the last two dimensions will be these guys, 27, it should be 30. Okay, that looks good. There we have our completed pulley. And last but certainly not least, we have the pin drawing. So let's come down to our fifth sheet. We'll select that. Let's go ahead and add a base view. And for the base view, I'm gonna leave the orientation as front. Put that scale up. Let's try zero pot 75. Yeah, that should be fine. Let's click Okay. And again, let's suppress the parts we don't need. So base plate, the brackets rotary, right, click, suppress. Same process fasteners, click once, hold down shift. Click again, right, click, suppress. Just have the pin. Let's do a side view of that, hit P on the keyboard. Select the base view. Do a side view. Also go for a projected ISO view, as well. Green tick. Go to bump that scale up, actually. Let's go for 0.5. That's good. Double click on this one, make it shaded. All these guys down. Got to label these views up. And now let's add some dimensions. D on the keyboard. I'm going to use this point here as a reference point. Select that point there. Let's go here first. Do this point to this one. Let's also add the thickness of this shaft as well, so this point to this point. And as for the diameter of this body and also the diameter of the end of the pin. We can do that on the side view. D on the keyboard then. So this one here is this body here, so diameter of 20, and this one here is the end of the pin diameter of 14. And there we have the technical drawing of the pin. Okay, and lastly, let's export this as a PDF. So let's come up to the top where our tours are. Let's go and export and select Export PDF. In terms of sheets, make sure we have all sheets selected. Let's open the PDF, as well, and keep the line weights turned on. It's okay. We could save this either into the Cloud or on the computer. I'm going to save this locally on my PC, save. And there we have the full PDF. So this is our assembly page. We got our base plate, side brackets, pulley wheel and the pin. So as a quick effort. I'm quite happy with that. There are a few things we could do, maybe to ti this up a bit, but all of the essential information is there. I hope that lecture was helpful, and I'll see you in the next one. 81. Additional Content Introduction: In this section, we'll take a look at some additional modeling tools. Now, these tools are not commonly used, but they are great to understand for the occasion when they are required. These include the coil command, which is commonly used for modeling springs or spirals, the loft command, which is Fusion's tool for creating complex geometries between different profiles. We'll also take a look at a technique for splitting bodies where required, and have also included a condensed summary of fusion for absolute beginners. And this was a lecture I made in 2024 for new entry level students as a kind of get started guide. Each tool and technique is presented step by step. And if you have any questions, please do send me a message, and I'll respond as soon as I can. I hope you enjoy this section, and I look forward to seeing you in the next lecture. So let's begin. 82. Coil Command: In this section, we'll learn how to use the coil command. This can be used to make springs or spirals with all sorts of customization tools. So I've got three examples here. On the left hand side, we have a spiral, and then we have three springs here, each one of them with a different cross section profile. So, let's learn how to use this tool. Let's jump into a new design. And instead of creating a two D sketch, we're going to jump straight into the creation tools and straightaway, click on Coil. Now within a coil command, we need to select a plane to do our circle on. This is a special type of circle that the coil command will reference in order to form a spiral or spring from that. So let's select let's go for the XY plane. Let's have a look at the top view. And now, although we're still in solid, we're in the coil command, we're actually about to draw a circle. So I'm going to left look at the origin and bring out a circle. I'm going to put a diameter there. Let's go for 150 mil. Press Enter. Then you'll see a preview there. In this case, it's a spiral, we have all sorts of parameters that we can change here. So feel free to have a good play around with these. I won't run through every single one. As we can see here, this type of coil is a spiral. So under the type, we can shift it to revolution and height. So these are the parameters we'll dictate. We could dictate pitch as well as revolution, and also height and pitch. But in this case, I'm just going to stick with the revolution and height and do a conventional spring. So in the preview mode, we've got several arrows we can play with here. This arrow relates to the cross section, so we can make that smaller, okay, like so. So we see essentially we're sweeping that profile around this coil path, or we can make it larger. We can control that in the diameter box, as well. Let's go 25 mill. We've also got the option here to increase. So in this case, it's the size of the circle, so the diameter. We can make that much bigger like so or make it smaller. Let's stick here. Let's go for the 150 that we said originally. We've got the height option here, so this is the arrow we see here. So total height will keep the number of revolutions and just adjust, the height accordingly, so we can have it quite compressed or like so. Let's go for a height of 400. We can also taper this, as well, okay? So taper like that, and then taper external as well. I'm going to keep that as zero for this example. And then for the profile down here, so the cross sectional profile right now is just a circle. So what we would have in a typical spring, we can change that to a square. You see this nice square profile appear there. And two other options we have is triangular, so external. So in this case, the triangle is kind of pointing outwards as it were, and then internal. So yeah, pointing inwards. I'm going to go with the circular section for now. And then in terms of the position. So this relates where this section here is in relation to the path here. So, for example, let's change the section position to outside. We'll see there that the section profile is on the outside of that line on center, okay, so and then inside is like this. Then section size, I'm going to leave a 25 mil. And then, in this case, definitely got it for a new body. Let's click Okay, got a home view. It's looking good. And of course, let's apply an appearance to this. Let's go. I'm gonna go for a paint, glossy paint, glossy red, click Close. And right now, I've got the visual style just turned to shaded. Turn visibility on. We'll see the path there. I'm going to keep that off for now just shaded. That's how we use the coil command, nice and simple, and I'll see you in the next lecture. 83. Loft Command: In this lecture, we'll take a look at loft modeling. So on the screen here are five examples of parts that were created using the loft command. And as you can see, the geometries are quite complex and not achievable by using either the extrude or the sweep tool. And this is where the loft tool can enable us to create these types of complex models. The loft tool essentially takes sketches from different sketch planes and calculates a three D body between them. There's a lot of maths going on behind the scenes to generate these faces, but we have the option with the loft tool to adjust certain parameters that will influence these calculations and create the geometries that we need. So in this lecture, we'll take a look at the three key types of loft modeling, which are profile loft modeling, centerline guide loft modeling, and rail guide loft modeling. So let's start with profile loft modeling. And to demonstrate this, we're going to be modeling this part here, which is an interesting looking vase. Let's go into a new design. Let's first of all, save this file, save call this profile loft modeling. Make sure it's in the right location. That's good. Safe. And to model this vase, we need to do four individual sketches on four different planes. Therefore, we're going to use the construction, and we're going to offset a plane, and we're going to offset, in this case, from the XY plane. We're going to come up vertical, and that's going to be a dimension of 75 mil. Let's enter. Let's put another plane then, let's offset from this one here. Let's go another 75 mil, and let's do one more as well from this one. Let's go up another 75 mil. So we've got our three added construction planes, and we've got the default X Y down here. So let's press C on the keyboard and start a sketch, and that's sketch on the XY plane. And it C on the keyboard again for a circle. And we want to start from the origin. So we just rotate that slightly. I've got the origin there. I'm going to drag that out. Let's go for a diameter of 75 mil. Just enter. Okay, that's nice, and let's finish that sketch there. And now let's create a new sketch. Hit C on the keyboard, and now we're going to sketch on this plane here. Okay? So we're sketching here. We've got our origin there. So let's start from there, bring out a circle, and let's go for 200 mil. Let's Enter. Okay, got our two sketches in there. Let's finish this sketch. Hit C on the keyboard. Let's go for the third plane this time. And we're going to start just at the origin there. I'm going to drag that out. Let's go 80 mil so I got our three sketches. Finish that sketch. Se on the keyboard, and we'll do a sketch on the top plane as well. And instead of a circle for this one, I'm going to come up to create going to go in a rectangle and I'm going to do eight center rectangle. I'm going to start that from this origin point here. In terms of the width, let's go 4150, press tab on the keyboard, let's do a height of 100, press Enter. Then we have our four different sketches there, and you can see how this will build the volume and the body of this vase. Let's finish that sketch then. Okay, everything there is looking good. Now let's come under the creation tools, and we're going to select loft. So from here, our toolbox pops up, and we need to identify profiles in which to loft from. One thing to note here that's very important is the order in which you select these profiles. For example, we'd either want to go from the bottom to the top or the top to the bottom. We wouldn't want to, say, start from this one, work our way down, and then select this one last. As per the calculations built into fusion, we must start, let's say, with this one here, and then in logical order, we'll go through the rest of the sketches. So this one here, we can start to see that preview form already. Now let's see how that preview changes when we select this profile here. Okay, we get that nice arc, nice curve coming in here. Then last but not least, we'll select this profile here. Everything in the preview is looking good, so we're just doing profile modeling here, so we're only concerned about this box. We're not concerned for the time being about guy types or rails, but we will cover these in a demonstration after. So we can click Okay there, let's have a look at this. That's looking good. It's the geometry that we're after. We can add to this as well. Let's do a shell command. Going to select this top face here. And in terms of thickness, let's go for a two mill. See how that comes out. That's okay. Yeah, that's looking nice. We've got our unique looking vase there. So let's see how we can edit some of these faces, then. We can understand here that by using the extrude tool or the sweep tool, this would be impossible to model, whereas with the loft tool, we're able to achieve this particular type of face here. You're going to turn off the grid. There we go. So let's come down to our timeline then and we can see we've got our added three construction planes. We've got all four of our sketches. We've got our loft there and also the shell command. We can edit any one of these. So we can edit these sketches. We can edit the distance of the plane. We can also edit the loft tool as well. So let's right click on the loft tool. Let's go edit feature. Let's take a closer look at the model. Now, you'll see on every profile, there are these circles, which essentially guides the faces of this feature. And we can adjust these. For example, left click, we can drag these down. We can see here how this guideline will alter depending on where we locate this point here. And likewise, if we do that to this one over here, okay, we can shift it around like so and start getting some really funky shapes coming out. Okay, let's see how that comes out. Press okay. There you can see our faces there are very I don't know how to describe that. We're going to skew whiff, and we've got these sharp bends in here. Okay, so these are points that we can adjust within the oftalEdit feature to achieve profiles that we want to achieve. So I'm gonna press Control Z, take that back, put the shell command back in. So that is the basics behind profile loft modeling, very straightforward. We just need to remember to go in logical order from one profile to the next. Now let's move on and take a look at center line guide lot modeling. So to do this, let's go on a new design. And let's press C on the keyboard, create a sketch. Let's go ahead with the Let's go for the XY plane again. Let's press C on the keyboard, and we're going to draw a circle out to the right of the origin. Let's go for a diameter of 50 mil. We're going to use the horizontal constraint between the origin and the center point of the circle. They're gonna press D on the keyboard and dimension these guys up. Let's go for a distance, yeah. Let's give a 100 mil. Finish that sketch there. That's one sketch we're going to loft from, and then let's do a corresponding face to loft two. Hit C on the keyboard again, and this time, I'll use a default plane, so we won't put in any construction planes. Let's go with the YZ plane. And for this, let's create let's go for a polygon. Let's go for circumscribed. Let's draw in a polygon here. Let's go for a ten mil. Constrain that vertically with the origin, and I'm going to put a dimension in there. Let's also go for 100 mil as well. I got a bit horizontal constraint on one of these lines here, and now that's fully constrained. Let's finish the sketch there, then. So we have these two profiles and loft between them. Let's come up to create. Let's go on loft, select our first profile, select our second. Okay, that preview is looking interesting, and we can just see a direct loft between these two profiles. So it's kind of like a diagonal. Not exactly what we want to achieve in this case, we want to have a nice arc coming in like so. And so to do this, we're going to use a guide, and in this case, we're going to use a center line guide. So this is something that we need to sketch in. So let's go back to the drawing board, press C on the keyboard, and let's do a new sketch this time on the X z plane. And let's go to create. Let's put it in an arc. Let's go for a Let's go for a center point arc, start from the origin. First point here to here. But notice we cannot snap on to the center points of either of these two profiles because they're not projected. So we're going to press P on the keyboard, and going to project to this point and this point, press O. Okay, now they're projected. We should be able to continue in our sketch. Let's go back to the arc center point, start from here, snap on to the first point, and then finish the arc at this point here. Okay, right click. Okay, let's finish that sketch. And now this arc here will act as arc center line for our lofting, so it should follow this guide here. Let's go and create. Let's go loft. Set our first profile and our second. Alright, not quite what we want to have. So here we're going to put in a guide type, and instead of rail, we're going to start with center line. And here we need to select our center line. So we're going to select this one here and see that big change there. So a nice guide to direct the loft. It's okay. There's one more thing I want to show you in here as well. So if we right click and edit this feature, I want to take away profile too. So I'm going to hit the cross here to remove that. And instead for my second profile, I'm actually going to select instead of this profile, I'm actually going to select this point here. If we press Okay. So we don't have to go to a profile, we can go to a point. We can see that nice kind of sharp end there looking very sharp, sort of like a wizard tap. Okay, so very simple. Let's just go right click Edit feature. And again, we just add in either a center line or a rail here. But in this particular example, we used a center line. Now that we've covered the center line guide, loft modeling, let's take a look now at the rail guide loft modeling. So let's jump into a new design. Let's do an example of this. So let's hit C on the keyboard, start a sketch. Let's go on the XY plane. And let's hit R on the keyboard. I'm going to use a rectangle to demonstrate this. Draw a a rectangle. Going to do 80 tab 60. Okay, and then we're going to constrain that. Let's go for the coincident constraint origin, hold down shift, like the midpoint of this line. That's fully constrained. Finish that sketch there. That's one of our profiles that we're left. Let's do another one now, but let's offset that from the XY plane. Let's offset that by let's go 4150. It's okay. C on the keyboard. Let's do a new sketch on this plane here. And I'm just going to project these lines here one, two, three, four. There we go. That's looking good in the preview. Click Okay. The finish the sketch there, and there we have Art two sketch profiles. So if we go ahead and loft between these now, it will just be as easy as doing an extrusion, nothing interesting. But if we now go ahead and add in some guides to guide the loft in its direction, will show us something quite unique. So let's hit C on the keyboard and let's do a sketch on let's go for the Z plane. And in this case, I'm going to us an arc. Now, let's use an arc, three point arc. One note about when we're using rails, they must be to some extent smooth. If we've got a really jagged line, fusion will not be able to carry out the loft as the faces will be too complex and perhaps conflict with one another. So I want to snap onto this line, but I need to project it. So I'm going to hit P on the keyboard, project this point here, press O. Okay? We've got that point there. That's nice. Let's go back into the arc tool then three point arc. Let's do the center point to this point here. And I'm just going to bring that out like, so let's put a rad on that. Let's press D on the keyboard, put it in a rad. Let's go for 90.'s finished sketch. Now let's go on create and loft. And this line here, instead of acting as a center line, we can sign this to act as a rail. So very similar to the concept of center line. First of all, let's select our two profiles. Let's go one and two, okay? Very basic extrusion there. And now let's go on the guy type, select the rail, and let's select our line that we've done here, the arc. And we'll see now that the loft kind of conforms to that rail guideline all on the external in the center of this face here. That's okay? And again, we can edit this. We can right click, edit feature, and we can adjust these points here, okay, so this will create some additional faces. We some rather crazy things, plus Okay. Okay? And then we've got quite a unique shape coming out there. So that covers the profile loft modeling, the rail guide type, and also the center line as well. I hope that was all clear, and I would recommend having a good play around with this tool depending on what you're trying to achieve. And if you have any comments or questions, please do send them to me, but aside from that, I'll see you in the next lecture. 84. Split Bodies: In this lecture, we will learn how to split a body and also learn how to split faces. So I've drawn up a basic part here, and I've also added in a construction line, which is this one here, and also a sketch, which is this sketch here. I'll turn off the construction line visibility for now. Just a note, we don't need to add this on a construction line. I've just done it for this lecture so we can better see the splitting line, but we can draw it, let's say, on this face here. So I've got my splitting line here, which is a spine, and we've got our part here. Let's come up to modify and we see we have the two commands here, split face and body. So we want to split faces, we'll choose this one or the entire body, this one. Let's have a go with split face first. And for this one, I'm going to select. Let's go for this one, this one, going to select my faces. Okay, so I've selected my five faces. And in terms of the splitting tool, I'm just going to select my spine I've drawn here, and we'll see a preview there, Okay what looks like a plane moving through this. Now will identify visually to us where this will intersect the faces I selected and create multiple faces. So split those in two. Let's press okay. As you can see now, of the faces that I've selected, they are now split into two, according to the intersection between those faces and the geometry of this spine that I drew here. So I noticed this face is not split, neither is this one. Whereas this one is here. Likewise it's here. And also, we've got the detail there like we have in our spine. So I'm going to hit Control Z, and I'm going to show you I'm going to show you one more example. Coming to modify, in this case, it's just body. So body to split, we've only got one body to choose from. And if we come into our bodies folder, we can select it there or select in the environment itself, and full of slidding tool's select the spine, press it o, and then we'll see there that every face is now split, and we now have two bodies in our tree. So body one, and in this case, it's body three. It A on the keyboard, apply an appearance. Now let's go for green, supply green here, and red here. And we can also assign different materials to both of these bodies as well. I'm going to go ahead and hide that sketch. That's looking good. And that's how we either split individual faces or split entire bodies. I'll see you in the next lecture. 85. Condensed Summary of Fusion 360: Welcome to this beginner friendly tutorial for Autodesk Fusion, or as it was previously called Fusion 360. In this video, we will go step by step and model a base plate, a bracket, some threaded hexkey fasteners, and with them, we will create an assembly, as we can see here. Overall, this video will guide you through the user interface, sketch tools, three D modeling tools, how to create three D assemblies, and we'll also take a look at materials and customization. So, let's get started. When we open fusion, straightaway, we are presented with the modeling environment. In the very center, we have the three D environment. This is where we will be sketching, three D modeling, and creating assemblies. It is the main focus of modeling infusion. At the bottom, we have a panel of display tools and viewing tools, such as pan, orbit, Zoom, et cetera, and we'll be covering each one of these and their shortcuts later. On the left, we have the browser. This organizes all of our design elements, such as parts, document settings, and also the default axis and default planes. At the top are our tabs, the main two of which are called solid and sketch, and under each tab is a series of tools associated with the tab title. On the right hand side in the corner, we have the view cube. This is used to help orbit and orientate parts or assemblies for better viewing angles, and we're using that a lot throughout this tutorial. First of all, let's start by creating a new project. I would always recommend creating a new project as it will keep each related part together, alongside any related assemblies and drawing files for quick and easy access. So let's go to the top left and let's select Save and let's call this first part base plate. And then when we come down to location, let's select the drop down here, and then we'll see a list of projects. So if you haven't used fusion before, you'll most likely just have the admin and the default projects available. That's absolutely fine. But in this case, let's go under new project. And then let's call this let's go for Fusion tutorial. And then if we click Save, we'll now see that a fusion tutorial project has been created. Let's click Save again. And now this part in any future parts that we make, we'll save into the same project so we can access them together. Now we have created our project, Let's start by creating the base plate. So to do this, we need to create a two dimensional sketch to which we will then turn into a three D model. As we can see on the screen now, these are the dimensions of the base plate. So let's go ahead and model this part. I will be modeling this part in millimeters, but if you want to change, you can come up to the document settings and then just click next to the Units to change. Got the option there to change to imperial, if you want. So if you want to jump into inches, for me, I typically draw in metric, so I'm going to stay in millimeters. Some people find that the grid in the background can be a bit distracting. If that's the case for you, feel free to turn it off. So if we come down to tours at the bottom, we hit grid and snaps, we can turn off the layout grid like so. I'm going to leave that on as the default, though. Also, if you want to change the color of the environment, we can come down to display settings, then we select environment. If you want to go, for example, a gray background, you can change like so, or, for example, a blue background. But for me, I'll stay with the default as photoboth have a white background. So let's begin modeling this part, then. Let's come up to the top where our tabs are. Make sure we're under solid. We want to come under the creation tools, and we want to hit the very first one, which is create sketch. And then we are presented with three planes. So this one here is the Z Y plane. This one here is the X Z, and this one here is the X Y. Need to select one of these planes to do our two dimensional sketch on. The more that you use fusion, you'll have a better understanding of which plane to draw on. But I would always recommend choosing the plane which orientates best your part. So in this case, we're drawing a base plate. So the best plane to draw, this one on is the XY plane. So we're going to left click once on this plane, and now we're looking at it perpendicularly, and we're ready to do a two dimensional sketch on this plane. Let's start with the footprint of this base plate. So if we come up to the top under the tabs, you'll see there's a new tab here, which is sketch, we have all our sketch tools, creation modify constraints, and so forth. Let's come under the creation tools, and let's select the two point rectangle left click here once, and we're going to start at the origin. So the origin is zero, 00 on the X, Y, and Z planes. So let's left click once here, and it should snap into place. Left click once, and as we draw the mouse out, we'll see a rectangle begin to form. Also see that the horizontal dimension is highlighted. Okay? So if we enter a dimension on the keyboard, it will become that. So as per the model, let's go for 90 millimeters. And then we're going to hit tab on the keyboard, and that will bring us to the vertical dimension. And this is also 90 millimeters. Enter that us enter on the keyboard. Then you can see we've got our square there. If you want to pan around, what we can do is to select the pan tool down here, and then we can left click and move around. An alternative to that is to hold down the middle mouse button, and then we can pan like so. So that's a shortcut. If you want to zoom in and out, we can use the mouse wheel to zoom in, zoom out. Now let's go ahead and add in this hamper. So we've got a 45 degree hamper at 20 mil. So to do this, let's come under the sketch tab again, and in this case, we're going to select the line tool. And I'm going to put the chamfer on this corner here to do this. I'm just going to left click on the vertical at any position, it doesn't matter for now, and then left click also any position on the horizontal. And they want to apply a dimension between this endpoint and the origin at 20 mil and likewise, for this endpoint. So let's come up to sketch dimension or shortcut D on the keyboard. Select the endpoint of our line, select the origin and left click once, I'm going to enter 20 mil on the keyboard, press Enter. I'm going to do the exact same process for the endpoint of this line here. Now if we notice this line is blue in color, that means it's not fully constrained. But we need to add this further dimension, select the origin, enter 20 mil, press Enter, and now we'll see it's black color, so it's fully constrained. It's not moving anywhere. It hasn't got the option to move. Also got this rough hole feature, which is roughly in the center of this square. Let's go ahead and select the circle tool. I'm going to input this circle anywhere for the time being. The diameter is 35 millimeters, let's enter. I'm going to use the dimension tool again to dimension this accordingly, so we'll see that it's blue in color now. We want that to be black, so it's not going to move anywhere. Left click wants on the circle. Let's go to the vertical. This dimension is 40 mil. Left click wants on the circle to the horizontal, left click and then 40 mils enter. Now I see the circles black in color, and it's positioned to where we want it to and we've also got some fillets around this corner here, this corner, and this corner. Let's come up to the modified tools, and we'll select fillet, and then we'll select this vertical line and this horizontal line, and you'll see a preview appear there. We've got an option to enter in the size of this fillet, which in this case, is 10 millimeters. Let's enter we'll do the same for this corner here. So left at the vertical, left put the horizontal and the vertical, ten on the keyboard. Same process, this corner here, horizontal vertical, ten on the keyboard, enter. And now I see that all of the entities here are black in color. Everything is fully constrained. Am I ready to finish the sketch there. So to do this, let's come up to the top right and select Finish Sketch. Okay. Everything's looking good. Let's go ahead and three D model this profile here. So let's come up to the top where our tabs are. Let's come under solid, and we're going to select this tool here, which is extrude or a shortcut E on the keyboard. Let's click that, and we've got a toolbox pop up. Now, first of all, we need to define what profile we want to extrude. There are three profiles here. There's this one, this one inside the circle, and then this one that's encompassed by the ShamfA. The profile we want is obviously this one here, so I'll select that. Everything else we'll leave as default, so the extrusion will start from the profile plane. The direction is just going in one direction. The extend type has a distance, and we're going to state that distance here. Now, as per the drawing, that's 10 millimeters into ten. We don't want that to be tapered, and the operation, we do want it to be a new body. So let's click Okay. Now let's come up to the ViewCube, let's click on the home view. Now we can see the three D model of that part. What we can do come down here. We can select orbit. And then if we left click, we can orbit around the part like so. Or a shortcut on your keyboard would be to hold down Shift, and then the middle mouse button, and then we can orbit like so. It's quite a useful shortcut. Way in which we can orbit is to use the view cube. So if we left click anywhere and hold down on the view cube, move the mouse around. We can orbit the part like so. We can also look at specific faces. So, for example, if I left click the front face, we're looking at it from the front view. I can then use these four arrows to rotate the part. That's rotated by 90. We can see the left view. Also click on the corner here. We can have a look at it from an ISO view. We can also reposition what we refer to as the home. So to do this, we can right click. We can select the current view as home bit to view. Then if I just move that to a random angle, and then we select the home view, you'll see the home view has changed to what we set it as. So that is the baseplate part complete. Let's just finish this off by giving it a color. Let's come up to modify. Let's click on the dropdown. If we come down, we'll just assign an appearance. Now you can apply a material as well. But for the purposes of this tutorial, we'll just go ahead and let's go for a red color. I'm just gonna go for a paint enamel gloss red. I'm going to hold down left mouse button and drag that appearance across and let go onto the part. I'm going to close my appearances. There we have our base plate. Okay, so the base plate is looking good. Now let's go ahead and model the bracket. So to do this, let's come up to the top. Let's come under File, and we'll click New design. And then we're going to go straight away and save that I want to call that racket. We want to make sure that its location is under our project. So fusion tutorial. That's good. Let's click Save. Now let's start to model this part. So we're going to do this in stages, and first of all, we're going to start with the footprint. So again, let's go ahead up to solid. Let's create a two D sketch, and let's select the XY plane. And then we're going to start with the rectangle tool. So two point rectangle, again, we'll start at the origin. We'll bring that out, and the horizontal dimension, we'll add in 80. We're going to hit tab on the keyboard, add in 80 on the vertical. Let's Enter. Looking good. Let's get that hampurin. So let's go the line tool. Roughly position that in. Now I'm going to select the dimension tool, endpoint of the line to the origin, 20, yes. Other endpoint of the line to origin. And then 20 press Enter. That's good. Let's go ahead and have this hole. So the center point circle, put that anywhere for the time being, and it has a diameter of 30 millimeters, and we'll sketch dimension there. So circle to vertical, going to be 40, then circle to the lower horizontal, it's going to be 40 as well. From here, we can finish the sketch, and we're ready to extrude this. So again, we'll come up to solid, select extrude, make sure that we select this profile here, not this one or this one. So let click once. Then for the distance here, we've got a distance of 10 millimeters. Leave everything else as the default. Yet new body is correct. Press okay? Take a look at that looking nice. Now the next feature we'll add is the side walls. That's the wall going along here and then down here. So to do this, we want to sketch on this face here. So we'll start. We'll create a sketch, and then we've got the three default planes there, which we don't want to select, but we can select faces of our three D body. So let's go ahead and select this face here. We'll look perpendicular at. Then let's go ahead and use the two point rectangle tool. We're drawing the wall at the back here to start in the corner. We're just going to snap anywhere onto the vertical line there. Then we go ahead and dimension that. So our dimension between this line here and this one, and it's got a wall thickness of 10 millimeters, there's ten, okay. Let's do exactly the same then for the other wall. So this corner here, bring that up anywhere for the time being. Let's dimension this line to this line. Again, wall thickness, 10 millimeters, press Enter. Good. Now, we do have a fillet here and also on the outside as well. But just to show you another way of adding fillets, we can do them in three D mode. So I'm going to leave this two D sketch as it is. I'm going to go ahead, come up to finish sketch, first of all, then solid extrude. I want just like three profiles. One, two, three, and I want these extruded a distance of 40 millimeters as per the drawing. Okay. Now, you see here under operation, we've now got the option to join to the existing body, which is what we want to do in this case. So let's stick with join. Okay, now, this is still one body here, okay? So these two walls are then joined to our original body. You got to hold down shift middle mouse button, just rotate around. Let's go ahead and add in this fillet on this edge here. So to do this, let's come under the solid tools. We'll come under modify, we'll select fillet, we'll select this corner here. Then our toolbox pops up. So we've selected one edge. Need to select the filllet radius, which in this case, is 5 millimeters. Okay, leave everything else as the default, constant radius, all looking good. Press okay. We've got that fillet up here there. That's looking nice. We've also got the fillet on the exterior here. So let's choose the filllet tool again. We'll select this edge here. This dimension is 15 millimeters as per the drawing. Press Okay. It's looking nice and we've got that uniform thickness running along the back wall. We've just got two features to add here. One is the hole on this wall and the other on this wall here. So to do this, we want to sketch on this wall. Let's create a sketch. Let's select this face here, okay? Looking perpendicular. Let's select the center diameter circle. Again, I'll just draw that in anywhere for the time being. That's got a diameter of 15 mil. Let's enter. A sketch dimension, circle to the vertical, that is 35 and then circle to this face here is 20 mil. Okay, the circles in black, fully constrained, looking good. Let's go ahead and finish that sketch. Now we need to extrude cut, so we need to remove the material. So again, we'll select the extrude tool, under here, we'll select our profile, which in this case, is this profile here. In a distance, we see the arrow here. So we can hold down the left mouse button and we can pull that out to extrude and add material, or in the other direction, we can remove material. So I'm going to put in a distance there going to be accurate, put it in a distance of -10 millimeters, rotate around. That's looking good. And the operation you'll see here is automatically selected cut, so we're removing material. It's okay. It's looking nice. Do exactly the same process for this face here. So create sketch, select the face, circle diameter, 15 mil sketch from the horizontal 20, sketch on the vertical 35, finished sketch, solid, extrude. I'll select that profile there. I'm going to actually just show you how to do this. So if we just go into operation and click cut and then we go ten mil, make sure we reverse that arrow. Oops, put in that ten mil again, minus ten, press Okay. Then we have our two whole features. It's looking good. That's all the features of this bracket, looking nice. Okay. Let's finish that up by adding an appearance. Let's go to modify appearance. I'm just gonna go for, let's go for green. Let's go for the powder coat rough green. Okay, looking nice. And we're just going to close that back to the home view. Okay, and there we go. That's looking nice. That is the bracket done. Okay, let's move on to the faster then. Let's come up to select a new design. Let's first of all, go on create sketch, okay? Now, in this case, I'm going to select the ZX plane. And this is purely because this will best orientate the part ready for our assembly. I'm going to select that plane, and you'll see what I mean when we come to the assembly file. Come up to our creation tours. So we're under the sketch tab. Let's go on the center diameter circle, start at the origin, drag that out, we'll apply a diameter there of 15 millimeters. Let's go ahead and extrude that. I'll come under solid, come under extrude, make sure that profile is selected. Okay, I'm going to put in a distance there. In our toolbox, we'll lab everything as the default, but for the distance, let's add in 30. And now we need to add the head of the bolt. So we've got the shank already. Let's come under create sketch. In this case, I'm going to choose this face here of the shank. Let's go under the center diameter circle tool again, start at the origin, and bring that out to a diameter, 25 mil let's come up to solid. Let's extrude that profile there. Now notice we have two profiles, the one which we've created there, and there's also an auto generated one coming from the shank. So we want to select both of those. We want to extrude those by a distance of five mil, looking nice. Let's go ahead and add in a Shampa then to this edge here and also this one. Come up to modify, select Shamfa going to select this edge here and this one and our toolbox for the shampa pops up. So we've got the two edges identified there. W these to be equal distance. Okay? So in this case, we only need to put in one dimension, which is 2 millimeters. You'll see both of these are now two. Leave everything else as default. It's okay. Then we've got that nice shamp on the head there just at the base of the shank. Let's now put in the thread on the shank come under create, then come down to thread. The following our toolbox, we need to select a face to apply the thread to. In this case, we'll select the shank. The thread type is automatically an isometric profile, but feel free to adjust according to your needs. Going to stay under the default there under size, so it'll automatically recognize the diameter of the shank. In this case, the designation is 15 by a nominal pitch thread of 1.5. Bass and direction leaves the same. But if you're doing a left hand thread, feel free to change. That's okay. And now we need to do one more feature, which is the keyway on this face here. Let's go under create sketch. We'll select the face. Then we'll come under our creation sketch tools. We'll select the polygon. In this case, going to use the circumscribed polygon, select that. We'll start the origin. And as you see as we drag this out, we're then going to add in a dimension from the origin to the flat. So flat to flat is ten mil. So origin to the flat will be five mils okay. Looking good, we just need to remove some material there that's come the solid, go and extrude, make sure that we select the right profile. So we want this one here. And let's make sure that's in the right direction. Okay. So it's a negative dimension. So in this case, it will be negative five. Leave everything else as default, operation, set to cut. That's okay. We've got our keyway, and there we have our fastener, and we're now ready to form our assembly. Let's go ahead and save that part, then. We'll call this fastener. We'll make sure that the location is under our project folder, Fusion tutorial. Look save. And now we're ready to move on to our assembly. Now, let's go ahead and make this assembly, and this is where things get interesting. So let's come up to the top. We'll go to file. We'll go on another new design, immediately, let's save that. And we'll call this. Let's go for assembly file. And then make sure the location is the project we created. So Fusion Tutorial. Big save. And now we're going to go back up to the top left, and we're going to select Show data panel. And within this, we'll see every part that we've created under our Fusion Tutorial project. And if you want to see any other projects that you're working on, just select home, and you'll have them all listed here. The one we're focusing on today is Fusion Tutorial double left click that one. And now you'll see, we've got our assembly file, base plate, bracket, and fastness. Let's go ahead and add in the base plate then. There are two ways to do this. Number one is to right click and select insert into current design. Or the method I like to do is just to hold down the left mouse button and drag that anywhere into the environment. The part will appear, and we've got our tour boox pop up. We've got some options to orientate the part. So we can use these wheels to rotate the part, or we can use these arrows to move them in linear directions. We've also got the center point of this part which we can just drag anywhere we want. So I'm just going to press Control Z and put that on zero on the XY and Z, and also the angle zero, as well. I'm quite happy with that being the position. I'm also going to rotate the view cube, have a look at the part from the corner, zoom out a little bit. Now let's go ahead and add in the bracket so that will sit on top of our base plate. We're going to hold down the left mouse button and drag that into the environment. That's not exactly where we want it as it's conflicting with the base plate, so we want to move that in a linear direction up. So we can move that up on the Zeraxis by ten mil, and that's where we want it to be. However, I do want to show you how to use the joint command. So for this, I'm actually going to raise it slightly higher and offset that we use the joint command to constrain and make these a rigid mate. So I'm going to leave that as 40 mil. That's okay. Now I'm going to go ahead and add in two fasteners. So let's throw in one. Roughly position this, so I hold down its center point, Bing that over here. I'm going to use this wheel to rotate that by 180 degrees. I just offset that slightly as well. I want to form a joint between this hole and this fastener. That's okay. Let's draw in another fastener, drag that over. Okay, use the center point, roughly position that. Rotate that by 90 I'm just going to move that in this direction, and we'll form that joint later. That's okay. Now, this base plate here is fixed. It was the first part we put in. The bracket. We can move. It's free to roam. It's not constrained to anything, and the same for the two fasteners as well. So now we need to go ahead and add in joints. So to do this, let's come under assemble. We can select joint, okay, or the shortcut J on the keyboard. Very straightforward to use. We've got the option to determine positions and motion. So motion is very typical to go with rigid unless you're doing moving parts, so feel free to have a play around with those. But for this particular assembly, we only want to have rigid joints. And under position, we need to snap two points together. Okay? So in this case, let's focus on the bracket and the base plate. So for the base plate, I want to select this point here, and I want to make sure that it's referenced from this face, not from this face. So for example, this is what we don't want to choose, and this is what we do want to choose. So that's left click on there. And just rotate the model, and then I'm going to choose the corresponding joint point for the bracket. So again, from this face here, we want to choose this point a left click once, you'll see we've got that mate there. It's not exactly the orientation that we want. So in this case, I'm going to use the wheel just to position that by in this case, -45 degrees. I'm going to press Okay. Now we cannot move this bracket. It's now got that rigid joint to the base plate and the base plate is fixed in place. So that's looking good. Now let's do these two fasteners. So still, these are both roaming around free. Let's go on assemble and joint. And in this case, I want to make a joint between the center point of this circle as we see is highlighted there. I'll just select that circle, rotate around. I come over to this circle here, and we can see its center point being identified there. So we select that circle. That is the mate that we want to have. That's looking good. Let's press Okay. And again, that's a rigid mate. So again, I cannot move that fastener, cannot move the bracket, cannot move the base plate. The only thing that's still in motion is this last fastener here. Let's add a joint to that then do the exact same process. Set the center point of this circle here, and I want to select the center point of this circle here. That's looking nice. And that's a rigid motion and position. That's all good. Press Okay. And there we have our complete assembly. Now in the next section, I want to cover on how we can edit assemblies and parts as well. So stay tuned for that. Et's now take a quick look at how we can edit assemblies or parts. So as an example, let's say that we wanted to increase the diameter of this hole by 5 millimeters. That hole is a feature as a part of this bracket, so we need to go into the bracket to edit it. So in our project folder, we right click on the bracket, select open. And once that's opened, there are two ways to do this. But I would recommend coming down to the bottom here where we've got the timeline, okay? And what you can do is move the arrowhead kind of back in time. Then we can go back in time and see where we were at that point. Each symbol here represents something. This symbol here is a sketch. This is an extrusion, then we can see we've got the fillets there. Also got another extrusion, and the last extrusion was the hole that we cut there. This hole here was a feature as a part of the very first sketch that we did, which is this one here. We can actually turn that sketch on under the browser where we have our sketches, it's sketch one. We can actually see that sketch there. So if we come down to the sketch at the bottom, right click on it, and if we edit that sketch, we can then make any changes here. Let's boost this up to 35 mil press Enter. Okay, finish that sketch. Then we can see visually the size of that hole is increased. Let's also go to measure that. So if we come up to the top, inspect measure so the shortcut there is I on the keyboard. Here, we need to select some geometry. We'll select this face here. And then under our toolbox, we can see the diameter is increased to 35 mil, which is correct. We just need to make sure from here that we save the file. Okay? So I just click, okay, save. And then if we come back into our assembly, so right click Okay. Then see that in a browser, we have these exclamation marks and also at the top here. Now, this indicates that there has been an update, and we need to activate that update to be reflected in our assembly. So to do that, we come up to the top, and we need to update that child component, which in this case, is the bracket, and then we can see visually that our hole is increased. And again, I'm just going to double check that. Click that geometry, and again, diameter of 35 mil, it's the same diameter now as the 35 mil, which was what we did for the base plate. Few edits that we can do in assemblies. So we see here we've got these symbols here. They indicate rigid joints. If we come over to our browser, we hit the drop down next to joints, we can actually turn the visibility of these off. So now you can no longer see those indications that there are joints there. We can turn them back on by selecting the eyes here here. And if we want to edit them, we can right click and then go to Edit joint. We can see where then referring to this joint here, and we can make any cordits that we like. One more example I'll show you, let's say that we wanted to increase the height of these walls here, and we need to go back into the bracket, right click, okay. Come down to our timeline and identify that feature. So if we jump back in time, we'll see it's this feature here, right click, select Edit the feature, and we can change that dimension. So from 40, let's boost that up to 60, press Okay. Then we're going to move our arrow head back to the end. Again, let's save that. That's okay. Let's right click on our assembly file. Click Open. And then, again, we're going to hit the update child component. So it's just going to follow along that update from the bracket, reflect that in the assembly. There we see now the walls have increased by 20 milli in height, and also the according joints are still relative as well. And so that is an overview of fusion or Fusion 360 as it was previously called. I hope you enjoyed that. It was of educational value. If you have any questions, please put them in the comment section and I'll reply as soon as I can. But aside from that, thank you very much, and I'll see you in the next tutorial. 86. Practise Exercise Introduction: This section of the course consists of a series of practice modeling exercises that will take advantage of all the tours and techniques covered in the two D sketching and three D modeling sections. Each exercise is provided with a dimension technical drawing. So feel free to have a girl at creating these models yourselves. But also, I will be demonstrating a complete methodology to model each part. And if you have any questions, please send me a message, and I will respond as soon as I can. Many of these parts can be three D printed and have included some cool desktop three D printed parts, including a smartphone and a Supermio stationary holder. So you're welcome to print these if you like. And if you do so, please send me a photo. Also included are two practice three D modeling exams. Now, these are based on the exams that are associated with becoming a certified fusion instructor and require you to utilize a range of sketch and modeling tools and techniques and also the ability to read complex technical drawings. I feel that these exercises are a good summary to this course, and I hope that you enjoy them too. So let's begin. 87. Flange & Piping Exercise: In this exercise, we will model this part here. So it looks fairly complicated. Aside from the base plate, that's very straightforward. Might be a bit challenging doing these two pipes here. Flange on the end should be simple. Let's go under inspect. Let's do a sect analysis, have a look internally, what's going on here, draw that back. Okay, so we've got some fillets internally there, okay? So all lamina fluid flow. Okay, looking nice. Okay, and these shelled out pipes. I think in a case like this, it would be best to start from the base plate and then we'll build up two sweep profiles for these two pipes here, and then it's quite simple to add the flange, although the flange is offset from this face here. So we'll be using quite a lot of construction tools to help us make this. So let's begin. Let's jump into a new design. These are the dimensions of the base plate. So if you'd like to draw this yourself, please feel free to do so. Aside from that, I'll have to go at this myself now. So let's sit C on the keyboard, start a new sketch. Let's go on the XY plane. Set C on the keyboard again, let's start from the right hand side at the origin, and let's put in the 30 mill circle here, press C again. Let's put in the PCD. So I'm going to put this as a construction line. It's got 91 mil diameter. Help us position those eight holes. Let's add another circle as well. Turn construction off, start at the origin, and this will be the outer circle. So one oh five it's looking good. Let's see again. I go to snap on coincident to the PCD and add in one of these holes mile diameter. I'm going to use the vertical constraint from the center of that hole to the origin. That's fully constrained. We're going to create circular pattern, select the circle. And the point that we're patterning around is the origin here. Okay? We want to have eight instances. Okay, equa spaced around 360 plus okay. It's looking good. I just tidy up these dimensions at. Et's continue on the left hand side then. So hit C on the keyboard again. I'm going to draw this anywhere for the time being. So we got the same circle here, 30 mill and we put a PCD put on construction. PCD, in this case, is 66. Then one more circle. Turn off construction. This is the outer circle. It's 80. Press you on the keyboard again. Let's input one of these holes coincident to the PCD. And this has a diameter of eight. Again, vertical constraint, center point of this circle to the center point of this one. And then I'm going to create circular pattern this circle here and that around the center point here. And again, on this parameter box we've got here, let's put in eight it's okay. It's looking good. And now we need to define where this is in relation to this one. So we can see us for the drawing. We've got a dimension from the center point here to this center point. That is a aligned dimension. So 91 mil. Move that dimension out of the way. Okay, there's still some movement going on here. But we can see in the drawing that there's a relationship of 30 degrees between these two center points here. So I'm going to add in a line. I do a construction line, centerpoint of this circle, center point of this one. I do one more construction line as well. Center point of this one. I'm just going to bring this out here, press D on the keyboard, and then we can input this 30 degree angle 30, okay. And there we are. That's fully constrained. Let's finish off the profile so we can form our extrusion. Let's go L on the keyboard line tool, turn off construction. I'm just going to put in a line in between these two circles here and then make that line tangential to this line here, tangential this circle, and likewise to this circle. Then down here, we've got this arc. So to do this, I'm going to hit C on the keyboard. I'm going to draw a a circle. It's got a rod of eight, so diameter of 16, and I'm going to make this one tangential to this circle and likewise here. And at this point, we do have the option to trim away the lines that we don't need. But infusion, I do find that that removes the fully constrained feature of this sketch, and so I'd rather just select the individual profiles. So I'm going to finish the sketch there. E on the keyboard extrude. Let's select this profile, this one, this one, like this one in here, and also this one. Let's have a look at a preview then that's looking good. Okay. And the extrusion, in this case, it's ten mil thickness.'s enter. G on the home view. And there we have our base plate that's looking good. And then next, let's do one of the sweep profile and paths of one of these pipes. Let's go for this one here, and then we can form the flange after that and just tight it up with the fillets holes, and also this fillet here. So this starts from this hole here on our base plate. So let's go back to our model. Okay? So we're starting in here. These are the dimensions of the sweep path. So if you'd like to model these yourself, feel free to do so. First of all, let's do the path then. So we want to sketch that on. Let's look at what planes we've got available to us. Okay, in this case, it would be the X Z plane. So let's create sketch hit C on the keyboard, and let's select the default z plane. Now for this, I want to start at the center point of this circle here, so I need to project this geometry. So I'm going to hit P on the keyboard, select this circle here, press Okay. Then we've got this line projected, and we do have a midpoint in there as well. Let's go on the line to then. Let's go on the front view for this and we see our projected line, snap onto the midpoint, as we can see there. I'm just going to roughly draw in the entities here, so we've got a straight line, hold down left mouse bottom, draw out that tangential arc, and then we're going to come across a certain distance. Want to put a tangential constraint between this arc and this line here. Now we can go ahead and dimension this up. So as for the drawing, we've got a dimension of from this line here to the origin. We've got 60 60? Sorry, 80 mill. Got a ad here. So this radius is 40 mil. We've got a total distance. So from this endpoint here to the origin, we've got there a distance. We have one, four, three. Let's enter. Let's finish the sketch there. Okay, that's our sweet path. Now we just need to enter the profile. Let's C on the keyboard, and this sketch, we're going to profile from this face here. So I'll select that face. Let's C on the keyboard, from the origin here. We're going to expand this out by 40 mil. Okay. And here we have our profile and then it'll follow this path here. Let's finish the sketch. Let's come up to our tool. Let's go and create and let's choose the sweep tool. In terms of the profile, profile here. We're going to select this one, and in terms of our path, we'll select this line here. Okay, previews looking good, already shelled out. That's nice. How does the join look down here. That's looking fine. Okay? And the operation, we want to make sure this is a join. Okay, that's looking good. Let's press Okay. And for the next feature, now that we've swept our pipe here, let's go ahead and add in this flange feature. So to do this, first of all, I'm just going to change the home view. I click on this corner here, right click on the ViewCube and select the current viewer's home fit to view. Now, if we look at where this flame sits, it sits off of this face here. Let's inspect that face to face. So I've hit I on the keyboard, at a distance there of four mil. So offset a four mil. Let's do that with a construction line. Let's goingto construct, offset a plane, select this face here. And we're going to go in this direction, so the minus. In this case, we want minus four. Okay. Now let's hit C on the keyboard and let's do a sketch on our new construction plane. We're now sketching on our plane. Let's come under Create. Let's go on rectangle. Start the centerpoint rectangle. I'm hoping that we can snap to the center point of this circle, but we can't. So let's press P on the keyboard, and then we're going to project this circle onto our plane. Let's press Okay. We can see the projection there and the center point. Let's go back to the left view. Go on create rectangle. Let's do centerpoint rectangle. We'll start from the center point here, we're going to bring that out. I'm going to type in 60, press Tab 60, Enter. Looking good. Let's get some of these holes in as well. That's a C on the keyboard. Snap coincident to this construction line here. Diameter, eight mill, repeat the same process down here, eight mill then we can mirror these lines across. We can mirror these circles across. Let's go on the vertical constraint between these two, and that's sort of distance between them. So D on the keyboard, center point to center point. We put that dimension in as per the drawing, 44 mil Go ahead and add a construction line that we can mirror over construction center point of this line, doing that down, center point of this line. Select the mirror tool, select these two circles as our objects. And in terms of mirror line, we'll go with this construction line plus o. It's looking nice. Let's finish the sketch there, Let's go back to the home view. P E on the keyboard and we'll extrude this profile here. So we don't want to go in this direction, but rather this direction. We don't want this to be a cutting operation. So let's change the operation to join. And in this case, we can go four minus ten mil, plus o. It's looking good. You're heading out some fillets to these corners. It's like the fillet command. Choose this edge here, this edge, also this one and this one as well. As for the model, we're doing eight mill fillets. Let's enter. Let's go on the home view again. Okay, that's looking good, like that. Okay, next feature, we need to add in this other pipe which sits around here, which is this one here. Okay, so to do this, we need to create a sketch plane that we can model the sweep path on. It's a little bit tricky in this case, because we can't use any of the default planes, so we're going to have to construct a plane. But to do this, we need some geometries to reference from for that plane to be in the correct place. But what we can use is the axis of these three circles here. So I'm going to come under construct and select axis, enter and axis there, press okay, right click and then select repeat axis, this one, press Enter, right click, repeat, this one, Enter. Got a three axis there. These act as edges. So let's come under construct. We're going to a plane through two edges. Okay? So we can only select two of these, so we just go one, two. That's okay. I'm just going to make that plane a bit bigger. Do you want to drag that across. Okay, yet, that is the correct angle. That's parallel with this face here. These are the dimensions of the sweet path. So again, if you want to draw these, feel free to do so. Let's hit C on the keyboard then and select this plane here. And I want to start at the center point of this circle. So I'm going to hit P on the keyboard and project this circle here, preso. We see what our projection line at a midpoint in there. From here, let's look at the left view. Let's hit L on the keyboard, find that midpoint, which is just there. We're going to roughly draw this in. So we've got a straight line coming up, hold down left mouse button, drawing that tangential arc. Let that go around there. Let's use the horizontal constraint then end point of this arc to the start point of this arc. Then it's dimension this up. So as per the drawing, this dimension here of this line is 95. And the route of this arc is 22.75. That will take us to the top quadrant of this circle here or at least a distance away from. That's our path complete. Now let's put in our profile. So I'll finish that sketch. We'll start a new sketch. But this time, we're going to sketch on this face here. Same process like before. Gonna hit C on the keyboard, start at the center point of this circle. Take that out 240, finish that sketch. There we've got our profile and our path. So let's go create, go sweep, select this profile. In terms of path, select this one. Okay, previews looking good. Okay, let's shell down. That's all correct. Let's go with the joint operation and press Okay. Then from here, we don't need these axis anymore. So if we hit the drop down next to construction, we're going to turn off their visibility. And the next feature we're going to add is the continuation of this shelling feature through this body here. So to do this, I'm going to create a sketch on this plane here. And what I'm going to do is I'm going to hit pee on the keyboard and project this circle here. So that's the profile I want to extrude cut through this material. Was press okay? Okay, let's finish the sketch there. Hit E on the keyboard extrude. We're going to select that profile we've just created. Going to bring this down a cutting operation that's nice. Now, in terms of the distance, we need to be a bit careful here because we don't want that going through the entire body. So what we're going to do is we're going to go to object, and then I'm going to select this face here. And as you'll see the preview shows, it will only cut up to this face. Let's press Okay. That's what we're looking for. Nice. And now we just need to make that join between this profile here and this body. So it's a E on the keyboard. That profile is available to us already. So we're going to do a continuation. We don't want to cut, though. I want to go for a join operation. And in terms of the extent type, let's go to object and select this object here. A preview is looking good, make sure that's a join, okay. It's looking nice. We've got our connection there, okay? So almost there, we need to tidy this up with a few fillets. So let's select the fillet command. And let's select the edges about all of the joins. Let's go this one, this one. Let's go for this one, as well. So this one down here, this one, and also internally. You know, we don't want any possibility of increased turbulent fluid flow, okay? We'd like to have laminar fluid flow. Let's get a radius there. Let's go a four mill. See how that comes out. Looking nice. Let's also select this one here as well. It's four mil or so. And let's give it overall radius as well to the base plate. So let's put a fillet on. Make sure we've got tangent chain turned on. This one here, let's go for one mill. And let's press Okay and see how that comes out. Looking nice, okay? Got our fillets in there. Go back to the home view, and let's do a section analysis, to double check. Everything is in order. I'll select this face here, and let's just work our way through. Okay, nice and smooth joins there. That's looking good. Continue. Yeah, perfect. There we go. It's okay. Back to a little home view. Then we have our complete part. Let's definitely apply an appearance to this one then. I said, A on the keyboard. In this case, I'm gonna go for a let's go into the metals. And yeah, let's go for stainless. Let's go for stainless, seal polished. I'm gonna drag that up. Drop that here, press close. There we have our completed part looking really nice. If you were able to model this yourself, a big, well done. It is quite a challenge. I hope you enjoyed that lecture. Look forward to seeing you in the next one. 88. Door Hinge Exercise: In this example, we will model a simple door hinge, as we can see here. And in the assembly, we're going to assign a joint with limitations. Okay, so this will be a revolute joint, and it's only limited to these motions that we see here. If you'd like to model this yourself, I created a drawing here. So please refer to this, and you can model up the pin and also the sheet metal part and then form the assembly. Aside from that, I will continue and have a go at this myself. So let's jump into a new design. And let's hit C on the keyboard, create sketch. Let's go on the XY plane. Hit R on the keyboard rectangle. We'll start at the origin. We'll give this a width as per the drawing 40 mil. Press tab on the keyboard, height 100, okay. And we're just going to hit E on the keyboard, and let's extrude this by the thickness, 1.5 mil. Press Enter. Okay, looking good. Let's get those fillets in there, then. Let's press F on the keyboard and just go to drag select to capture that edge there, and also this one here. And that's got a rat five mil. Press Okay. Next up, let's put in these countersunk holes. Let's see on the keyboard and select this face. And we're going to input some points that's coming out of the creation tools points. I go to roughly place these, something like that. And then I'm going to hit the vertical constraint, apply it between these two, and apply the same vertical between these two. And then we can go ahead and start dimensioning this up. So this point from this vertical line here is 20 mil, and this point from this vertical is ten mil. This point from this line here, we've got 12 mill. Then we've got 36 from this point to this point. Then we've got 65 from this one to this one. And last, we've got 88 from this point to this line here, 88. Let's finish the sketch there, then. These are our four points fully constrained. Let's go on the whole command, and we'll select these four here. So one, two, three, four, and in terms of the extents, we want that to be all hole type. Let's go the counter sunk, and they're simple. There's no threads. So as for the drawing, we've got, yeah, four holes, diameter eight on the counter sunk by 90 degree, and then the through hole is five mil. Okay? So all these figures are correct? Let's preso, okay. Looking good. And now let's get the housing in for the pin. So I'm going to hit C on the keyboard. Let's do a sketch on this plane here. And I'm just going to sketch this in in the environment. So let's go over circle, and let's draw in. So we've got a radius of five on the outside. So ten, it's circle again. So from the center point, and we've got a diameter of six there. We've then got a cut out, so I'm going to use a line tool here. We're going to draw in two lines, one, two, and that's usually the dimension tool. We can dimension between those. That's got a distance of 1.5. Then we can also see that from the center point to this line here, we've got a dimension of 0.5 mil. And we've also got a fillet between this line and this line to do this, going to hit C on the keyboard, drawing a circle. So it's got a rod of one, diameter two. Okay, so the fillet will sit, something like that. Let's use the tangent tool. Let's go circle to circle and circle to line. I got that nice, fill it in there. Let's start to position this then. So you know this line here is collinear with this one, so we can apply that as a constraint, go collinear constraint, this one, to this one, and also let's choose the coincident constraint, this point to this one. And then all we need to do is to join up from the origin to this line here. Make sure that line, we've got a complete profile there. Let's finish that sketch. Put it E on the keyboard and select the profiles we need. So we need this one. We're going to choose this one, this one, and this one as well. Just have a look at a preview of that we track that out. Yeah, that looks good. Okay, and we've got a distance there of about 25 mills, so -25 in this direction. Okay, that's looking nice. Now I want to pattern this over, instead of drawing it again. So I'm actually going to make this a new body. So I'm going to edit that feature and go to make this instead of a join. Go to get a new body. Press Okay. Make sure in our body's folder, hit the drop down. We've got our first body and second one, that's correct. So let's go of the creation tools. Let's go on pattern, rectangular pattern, and we're going to select the body, in this case, this one here, and the axis, we'll choose this line here and bring this across. We only need a quantity. So only two instances in terms of the distance. So as per the drawing, we want to go 25 plus 25. Let's do 50. That's okay. There we go. There we have our sheet metal part. That's looking nice. Make sure we save that part. So let's call it sheet metal part. Say that in the right location, save. Okay, let's start a new design and model up the pin. Got a new design. It's a great sketch. And we're going to do this on the XZ plane. Start with C on the keyboard circle, start at the origin. And for this, we'll do the inner diameter. So that's six mil. Okay, then hit E on the keyboard, and we'll extrude that by a distance of, so 100 up until the head. That's okay. Over here. Let's press E on the keyboard, sketch on this plane. Hit C again, circle, do the outer diameter of the head, which is ten mil. It's okay. E on the keyboard extrude. I want to select this profile and also this one. Distance here is as per the drawing two mill. Okay, let's go on the home view. That's our pin. Let's now save that part. And we'll just call this pin. Call it Pin tutorial, save. Now we've drawn up our sheet metal part and our pin, we have one of these in the assembly and two of these. Let's go ahead now and make the assembly. Let's go on a new design. And let's come into our data panel under our project, if you find the cording parts here, we've got the sheet metal part and Pin tutorial, right click Insert into current design. You're quite happy with that. Go to leave that there. I go to insert another one. So right click insert. I'm going to slightly move this one over here, and let's rotate that 180 as well. Like so. Okay, let's also get the pin in there, right click insert into carret design. Yeah, happy with the orientation of that. Let's leave that there, okay? Let's go ahead now and add in some joints. So let's put the pin in place first. Let's go J on the keyboard, and we'll hover over the circle here and we'll see it selects this joint here. This point here. That's correct. And we want that to be corresponding with this point here. So left click there once. It's okay. Review looks good. Now we just need to place this sheet metal part. Let's get J on the keyboard again. And in this case, many to choose from. But let's go this point here, and we'll join that to this join here. Okay, that's nice. Under motion. So we don't want this to be a rigid joint. We'd rather have it as a revolute joint. However, that's not exactly the type of revolution that we want. So in this case, we're going to input some limits. So this will take some playing around with, but let's put it in a minimum and a maximum. And I'm going to do this manually using the pointers here. Okay? So if we bring this around like so, let's just see how that comes out there. Okay, that's looking pretty good to me. I got 150 on the minimum, 30 on the max. Have a look at that again. Okay, and feel free to change those how you like, but I'm going to leave those as they are for the time being. Let's go back to the home view, exit out of the data panel. And let's go ahead and apply some appearances then. Let's make this look pretty. Let's press A on the keyboard. And for these sheet metal parts, I'm going to come under metal, and I'm going to choose a brass. Let's go for a polished brass. Make sure that we're under bodies at the top and not faces. So polished brass. I'm gonna go for this this face here and this face here. And then for the pin, I'm just simply going to go on. Let's go for a paint glossy and black. Body there. Press close, back to the home view. And let's just have a look at that joint one more time. Motion, preview. Yeah, that's looking nice. Okay. And then we'll finish up there. Just go to tidy up this by coming under the object visibility, turning off the joints. There we have our complete part. Yeah, I hope you were able to follow along okay. And again, if you do that yourself, big, well done, I'll look forward to seeing you in the next lecture. 89. Elbow Pipe Bend: In this exercise, we will model this part here. So we've got a nice pipe, 90 degree bend, and then two flanges either side with a chamfer and some mounting holes. If you want to have a go at this yourself, I've done a drawing here, so feel free to use these dimensions and have it go. Aside from that, I will continue and model this myself. So let's go on a new design. And let's hit C on the keyboard, start a two D sketch. And we're going to start off, in this case. I go to start off with one of the flanges. Then we'll do the sweep profile and path. We'll sweep that 90 degree bend, and then we'll add in the other flange at the end. So let's do our first flange on the Y Z plane. Let's go for the creation tools. And let's go on a let's go on a center rectangle. Let's go from the origin and draw this out. We're gonna go 360 by 360. Then we're going to input this through hole there. So E on the keyboard, star the origin. We'll bring that out by 210 mil. Let's Enter. That's fully constrained. Let's E on the keyboard. Straightaway. Let's extrude that. And the distance there is 50 mil. This is a very big flange. Let's go ahead and put these fillets in. Let's F on the keyboard. Select this edge, this one, this one, and this one give that a radius of 20 mil. Let's enter. Now let's go ahead and add these holes in here. So these are just simple through holes. Going to use the whole tool for these. So let's hit C on the keyboard, create a new sketch. Let's go on this face here and let's insert some points, identify the center of these holes. So four points there. Use a horizontal constrain between these two. Vertical constrain these ones, and horizontal constrain these ones and vertical these ones. Now we can go ahead and put in some dimensions, D on the keyboard, center point of this one to the top horizontal line. It's 50 mile top horizontal line to this one here is 310. Then this one to the vertical line. We've got 50 and this one to this point here. We've got 310 -50, so that's 260 center. There we are fully constrained. Let's finish that sketch there. Got all our center point to our holes. Let's go on the hole command, then, we'll select one, two, three, four. And as per the drawing, again, simple holes. In terms of distance, let's go through all, and we've got a diameter of yet 40 mil, Okay, all these parameters are correct, let's press okay. There we have our first flange. That's our very first feature. And now we need to go ahead and input a profile and path for this swept bend. So let's go ahead and put in the profile first, set C on the keyboard, select this face here. We've already got this circle here, but we want to add in the outer diameter of this bend, which in this case, is 290. Okay. We have our profile there. Let's finish that sketch. Now we need to put in our path. Let's see what default planes we have available. Hit the drop down here, and we want to choose, in this case, yeah. It's the X Z plane, we'll right click on that, create sketch. Start with the line tool, start from the origin. I'm going to come out horizontally distance off. So it's 150 -50. That's 100. You're going to click there, and then I'm going to hold down the left mouse button and drag out a tangential curve. To finish somewhere there, and then bring a line up 100 and press Enter. Let's go ahead and add a tangential constraint between this arc here and this line. And then following that, let's give a dimension to this arc here. That dimension is 405 minus one, 15. Let's enter. You go, that's looking good, that should be all fully constrained. Yeah, we've got the red padlock there, okay? So we've got our path. Let's finish the sketch. Now let's go on our creation tours. Go on sweep. We're going to select this profile here. And under the path, let's select our path here. Okay, previews looking good. Okay, let's press Okay. And just one last feature to add, and that is the exact same flange as per its dimensions on this face here. So first of all, let's add the Shampa and finish off this flash. So let's come to modify Shamfa. We've got a 45 degree Shamfa like this one here, so equidistance. And this is ten mils per the drawing. But Okay. And then we have different options available to us to put this flange on top of this face here. So what we could do is essentially repeat all of these sketching and three D modeling operations on top of this face here, which is very time consuming or a much quicker way to do it, which is what we're going to do here is to just copy this feature over here. So if we're going to copy this, we need to check how many bodies that we have. We only have the one body available to us. So let's make this one a separate body. So let's find our sweep, which is as we can see, it's highlighted in our timeline here. Let's right click on this, go and edit feature. Then under the operation, let's change that instead of join, so just be one body. Let's go on a new body. Click Okay. Make sure that's come out right. So body one, in this case, is the flange, and body two is a sweat profile here. So we are interested in copying body one and repositioning here. So let's right click on that. Move Copy. And in our toolbox, let's drag this over here. Let's go on a free move. And let's just well, we need to make sure that we create copy here. We don't want to be moving the original. Just go to move this up, like so. I'm going to rotate that by 90 degrees. Okay, and they're going to press Okay there. Then from here, we're going to do one more move operation on this body here. If you look at our bodies folder, we now have a third body created one we copied here. Right click on that, move copy. In this case, we're going to choose point to point as a move type. Want to make sure we got body selected, and this one's already selected for us. Needed to create the origin point and the target point, and we don't want to create a copy in this case. So it's very similar to the joint command in that if we actually highlight, let's say this circle here, we can see the point highlight in the center. So we select that circle. That points now chosen for us. Then we repeat the exact same here, and we can see this blue kind of diagonal line showing the point to point met. So let's left click there once. And let's click Okay. That preview looks good. Let's go on the home view. And there we have our completed parts, so comprise of three bodies, the first flange there, swept profile, and the third flange up there, which we copied across. Everything there is looking good. Let's go ahead and apply an appearance to this, of course. Let's A on the keyboard. And let's go let's go for a metal, and let's go for a stainless. And I've got to stainle's polished again. That's quite a nice one. Que close. And that is our complete part. So we can save the part from there. And I look forward to seeing you in the next lecture. 90. Flange Coupling Assembly: In this exercise, we will model this part here. So this is an assembly made up of a flange component with a neck corresponding on the other side as well. And also, if I hid one of them, we'll see inside there right in the center, we have a gasket, and then external mating these together, we have a series of fasteners, which are brought in from the fusion content library. So this is an interesting assembly to make. If you want to have a goat with this to yourself, I have a drawing here of the flange and neck so feel free to take those dimensions, and then have another drawing here, which is off the gasket. So we've got the OD, PCD, size of the holes, and then the internal hole, as well. So let's begin to model this assembly here. Let's start off with the flange on its neck. Let's go on a new design. And let's hit C on the keyboard, create sketch, and we're going to sketch this on. Let's go for the exit plane and start the origin with the circle tool. Draw that out, and let's go for the OD, which in this case, is 175 mil. And let's go for the through hole as well. So C on the keyboard, put in the other circle here, which is 64 mil. And then we can hit E on the keyboard and select our profile. We want to extrude that. So that's got a width of 18 mil. It's okay. Now let's get these holes in position around the flange. Let's C on the keyboard, select this space here. Let's put it in a series of points again at one point in there. Let's put C on the keyboard and put in the PCD, so put circle diameter, make that a construction line. That has a dimension of 140. Want to use the coincident constraint between this point and the PCD, and then the vertical constraint between this point here and the origin. Come and create, do a circular pattern, select the center point of one hole, and the center of our circular pattern will be the origin here. Total number of holes. We've got three, six, eight. Okay, there we go. Finish the sketch. Let's use the whole tool, press H on the keyboard, and let's select the multiple holes. And then gonna drag select these three here, these two. Go for these two, as well. And this one here at eight in total. In terms of extense, let's go through all, and the whole type is simple, and there's no tap, just a simple hole. And the diameter of this hole as per the drawing is 15 mil. Press Enter. It's looking good. And now let's get the neck in place. Let's C on the keyboard. We'll select this face here. Again, C, and we'll start at the origin. We're going to bring this out by 80. Let's hit E on the keyboard extrude. That profile is already there for us. Fantastic. Let's draw all this out. Previews looking good, total distance we've got there is 118 -18. Enter. Okay, that's looking nice. Let's get that champa in there as well. So let's go modify hamper. Select this edge here. This is an equal champa so it'll stay equal distance. And in terms of the dimension there is ten, so ten by ten, press Enter. And let's also right click in our timeline. Let's go Edit feature. Let's add in two more hampers, this edge here, and this one. These will both be equal as well. Let's go for one mil. Press Okay. Go on the home view. It's looking good. Okay, let's save that part. Let's call that flange Nick. Lange coupling, save. And now let's go ahead and create a new design, which in this case, will be the gasket. Let's it S on the keyboard. Let's do a sketch. We're going to do this again on the same default plane, Ed, S on the keyboard again, start from the origin, and we'll do the outer diameter here, which is 170. Put in the PCD, so make that a construction line type from the origin. That is 140. Then we've got the through hole there. So C once again, turn off construction. And Alan one last circle here, which will be 70 mil. And in terms of the holes, we could either do these using the whole command using points or we could do them in sketch. So I'm going to do these in sketch at C on the keyboard, draw that out. We've got a diameter of 15 mil. Again, vertical constraint, center point to the origin, and then create circular pattern, choose the circle, point of reference will be the center here and a total of eight. That's okay. Finish the sketch there. E on the keyboard, let's extrude this profile here. We've got a thickness as per the drawing, 1.5 mil let's go ahead and save our gasket. Call it gasket. We're going to call it two for me. Save. And now let's go ahead and create our assembly. So let's go on a new design. Let's come into our data panel. And we have here our flange eneck in our gasket. Let's go ahead and insert the flange Neck first, right click insert into current design. Looking nice, I'm going to leave that there grounded to the parent. And let's input one more. So right click insert in current design again. And this one I want to move. Move that up there, rotate that 180 degrees. Like so just go to leave that floating there for the time being. Let's put in our gasket, right click insert. Definitely want to move this over here, press okay. We can start using the joint command and making up our assembly. So you need to be a bit careful about where we select. I want to choose the center point of this circle here, so left click there once. I want that to join to the corresponding point, which is the center point here of this circle. Looking good. I want it to be a rigid constraint, make sure that those holes are all aligned. That's looking good, okay. Then last we can put in this part here. So J on the keyboard. And let's go for the same point. So this circle here. And I want the outer gasket circle center point, which is this one. It's Okay. Make sure that's good. Yeah, looking good. We've got our gasket sandwiched in there. Nice through holes there. That'll be for the 14 fasteners. Let's go on the home view. Close down the data panel now, and now we can go on Insert fastn. Okay, so let's start off. Let's get some bolts in there first. I'm gonna go for flanged hex bolts. I've got a filter on here for ISO standard and metric measurements. So in this case, I'm just going to go out with the default here. Left click on that once, and make sure select similar is turned on. Then as we move over here, we should see that they will pattern throughout the flange. Left click once. Just double check these parameters here M 14, yet, that's good. We've got 15 mile holes. Nominal length 60. Yeah, we're going to have a nut on the end of there. There should be enough thread leftover. Let's stick with 60. Material is good, finish. Okay. Actually, let's change the finish. Let's go for black. Let's press Okay. Right, that's looking nice. I'm just going to hide these joint symbols. So display settings object visibility, turn off the joints. There we go. They're looking nice. And now let's repeat the process for some nuts on the other side. It's going to insert fastener. We're gonna go four nuts, and I'm just going to choose a flanged hex nut. Again, I've got IO and metric, and I'm just going to use the first one here. Bring this over roughly put this in position, and hopefully fusion will recognize where we want that to sit, which is here, and then it will pattern over and select similar like so. Preview looks good there. Let's click Okay. I'm going to make these black as well. G to right click on that. Edit the fastener. Finish black. That's okay. There we go. There we have our complete assembly. That's looking really nice. We've got our Gascon sandwiched in there. We've got our fasteners, and we've got our flange neck, as well. Looking really nice. If you did that yourself, Big well done, and I look forward to seeing you in the next exercise. 91. Paperclip Sweep Exercise: In this exercise, we will model this paper clip as we can see here. If you'd like to have a go at modeling this yourself, you can refer to the drawing, which I'm just showing here. So feel free to use these dimensions, and we've got a profile down here of 0.4 mil. But aside from that, I'll continue to model this part myself. So let's go into a new design. Sit C on the keyboard, create a sketch. And for this, let's start with the path on the XY plane. Sit L on the keyboard, start of the origin, and we're going to come up by ten mil. Zoom in a bit. Left click there once. Hold down the left mouse button and do a tangential arc. And this has a radius of three, so I'm going to roughly position that, something like that. And then come down, B 15 Left click once. Same process with the tangential arc. And this one here is 2.5, so roughly put that in position. Then we're going to come up again by 13 mill. Left click to another tangential arc, something like that. Then we'll finish off the line tool there. Then we'll use some constraints and dimensions and have this fully constrained. So first of all, let's go on the horizontal constraint. Let's start with the origin at this point here. Let's then hit D on the keyboard. Let's put in the ad for this arcuate got a radius. We've got between 3.2 and 2.8, so that's 3.0. And this AD down here, we've got 2.7, 2.3, so 2.5, this rat up here, we've got 2.21 0.8, so 2.0, then that should be fully constrained. That's how I look at my sketches yet. We've got the red padlock there, and that is our sketch path. Let's finish that sketch there then. And now we need to sketch in the profile. So let's hit C on the keyboard once again. And for the profile, we'll go on the Zplane and C on the keyboard. Let's do a circle. And this is our 0.4 mil. Finish that sketch. We've got our profile, and we've got our sweep path here. It's come up to create, select the sweep tool. And in terms of a profile, select this one here. And in terms of a path, let's go for this one here. Make sure that we have change selection turned on. The other parameters, yet, we want the full distance of the path. So leave that as one. Don't need a taper or a twist orientation. So yeah, the profile is perpendicular to the path. So leave that as it is. And operation. New body, press Okay. We have our paper clip, and of course, let's apply and appearance. Hit A on the keyboard. And for this, I applied I went into metal brass, and I went for brass polished. We'll drop this one in the appearances here, close. And there we have our paper clip, nice and simple exercise, a really effective way of using the sweep tool to generate nice paper clip profile as we see here. I'll see you in the next exercise. 92. Mug and Coaster 3D Printing Exercise: If you're into three D printing, one of the parts that I see regularly online that's very common for people who are getting into three D printing is custom design coasters. So I have a design here. It's very generic, simple sketch using the extrusion, a few different sketch techniques. So we've got a revolve there. I'm using splines to create the profile of the fusion logo, and then of course, you can insert anything that you like in here. We can also model up the coaster holder as well, which can be three D printed also. So let's see how this looks if we put a glass on top. We hide these and let's have a look with a glass on top. Yeah, that looks fairly nice, okay? Good sizing generic coaster there. For this part here, I've created a drawing. So if you want to model specifically this part, feel free to do so. As for the fusion logo, we'll learn to use the spline tool in this example and also insert the text there. Well, let's begin to model this part, then. Let's go into a new design. Let's at C on the keyboard, created sketch, and let's go with the XY plane. That's the one we want for a coaster. Within the circle tool, let's start at the origin, and we'll bring out this diameter at 80 mil as per the drawing. And then we'll put in one arrowhead and more circular pattern that around this circle here. So I'm going to roughly draw this in place. G to draw a line angle like so, and then roughly like that. Let's use the perpendicular constraint between these two lines. Let's also use the equal constraint between these two, as well. And then we can apply a dimension to one of these lines, which as per the drawing, it's eight mill. Okay, that's looking nice. Let's continue. Press L on the keyboard line tool. Come across here perpendicular by a distance of two mill. Click on. G to bring this up something like that, again, over perpendicular. I'm going to join off finish off this line just here. Let's go on the perpendicular constraint between these guys. And let's put in an equal constraint between this line and this one, so they'll both become two. And let's use a vertical constraint between this point and this point. Okay, I think that's looking good. Go ahead and apply one more vertical constraint, this endpoint to the origin. And that's applied dimension between the origin and this point here. And in the drawing, that's 28 mill and hopefully, that should be fully constrained. Let's go in our sketches. We've got the red padlock. That's perfect. We're now ready to circular pattern this around this circle here. It's going to create circular pattern. A drag select around the arrowhead. And for the center point, let's go with the origin and for quantity, thrown to 16, up to you, whatever shape you're drawing, feel free to insert as you like. Lets go for 16, press Okay. Finish that sketch there. Okay? I think that's looking quite nice. And let's E on the keyboard, then. Let's extrude this. And in my design, I'm extruding by four mill. So if a three D printed, that should be fairly strong. Let's press okay. It's looking nice so far. Let's go ahead and add a border for our coaster, then. Set C on the keyboard. And for this, we'd want to sketch on the base of our coaster. Okay. And I'm going to offset the outer circle here. I go to bring this out. We're going to offset this by three mil. That's okay. If we look at that from the top, then simply go to hit E on the keyboard. I want to do an extrude. It's going to be a joining operation. I want to go in this direction here. So that's the negative. Let's go negative five. Let's enter. We should have a one mil offset between these two faces. Let's hit E on the keyboard and just double check that. This face, this face. Yeah, we've got the distance there of one mil offset. That's good. Let's go ahead and apply some radian into this, then we don't want to have any sharp edges. Let's apply some fillets, and let's like this face here. And I got to like this face here. So I got two edges. Let's go for a one mill. That's looking nice. That's okay. I think that's a good border to have for our coaster. Let's add the next feature then. So for this, I'm going to do the fusion logo just at the side, I'm going to extrude cut that. So to do this, I'm actually going to insert the decal. I'm going to use the spline tool to model around that part to generate a profile, and then I can extrude that. So let me find that that's in my three D modeling section, fusion logo insert. Okay, let's go on the top view. And let's insert it on this face here. All right. I'm going to rotate that. May put that around 90 degrees. I'm going to scale that down slightly as well, something like this. And I'm going to position that here. Let's go. Okay. And now let's start a sketch. Let's go S on the keyboard. We're going to select this face here, rotate that back. And then I'm going to use the creation tools, but here I'm going to use spine. I'm going to use Control Point spline. Select this once. And now I'm going to start at this corner here, and I'm just going to follow the logo up. I want to try and follow as best I can the outline of this F. A and I'm going to finish that there. So I just did that roughly, I didn't spend too much time, but as you can see, we've got a profile that's conforming to the fusion logo. Let's finish that sketch then. Let's go on E for Extrude. Let's select this profile here. We don't need the deco there, so we can hide that. So come into our folder, just turn off the decals. And then let's extrude that profile in this direction. And then the distance, let's go through all, make sure it's cutting operation, press okay. How I look at that from the top view. Yeah, quite happy with that for a rough use of the spine tool, that's come out, okay? Let's insert one more. Sketch as well. Let's go see on the keyboard. This face here, rotate that back. Let's come up to the creation tools and use text, roughly drawing a border there. I'm just going to put in insert logo here. Take that down in size. Let's go to three mill. Okay, maybe four mill. And I want to change the font. I'm going to go in this case, for stentil That's okay. I go to reposition that slightly. Let's finish the sketch. E or extrude again, select our text there, make sure we're going in the cutting direction and under distance. Let's select all. That's okay. There we go. That is a very basic design for a three D printed coaster. Of course, let's apply an appearance for this. Gonna go for a generic glossy paint. Gonna go for enamel glossy green. Drop that there, press close. Back on the home view. That's looking quite nice. And moving on now that we have modeled up the coaster, let's go ahead and model up the coaster holder. So this is a very simple design with dimensions that are suited for the design of coaster. We just modeled, but feel free to adapt this how you like. So let's go on a new design, and let's press E on the keyboard, so circle tool, and we'll do this sketch on the XY plane, select this one. Start the origin, and we'll bring this out the larger diameter. So 96 mil Enter, press E on the keyboard. Let's extrude that by. We've got a thickness of three mil. C on the keyboard again. And in this case, we want to sketch on this plane here. Okay? So from the origin, we'll bring that out 90 mill, so this is the inner diameter, and then we can extrude out these walls here, set E on the keyboard. So like this profile, and we're going to extrude this one by we've got 50 minus three, so 47 gives us a total height of 50 mil. That's nice. Okay. And then from here, we want to create these cut out sections here. So we use the extrude cut tool for that. So let's create a sketch, and let's select this face here. And I'm going to hit L on the keyboard. Let's do some lines. Let's start coincident to this outer circle. Just go to draw this anywhere and make it coincident to the same circle, put it on the other side. Same process here. Then we can add some constraints and tidy this up. Let's go on a coincident constraint. So like this line here and the origin. Same process for this one and this one. I'm going to draw in a center line in which I can use the symmetry constraint between these two lines to on the keyboard, choose construction origin to the top. Make sure that's got the vertical constrain on. That's nice. Select symmetry, select my two lines. And we're going to select our construction line as the symmetry line. Okay, that's looking good. So still quite a lot of motion here. Let's get a dimension in there, D on the keyboard, endpoint of this line, endpoint of this line, place that there. I put 20 milwas per the design that I did. To finish that sketch, we should have a profile here and a profile here. That's perfect. Let's a E on the keyboard, select those two profiles that we created. And we're going to be cut and extruding these. And we're going to go -45. Enter. Now we can apply some fillets and tidy this up. Sit F on the keyboard, then. Let's apply the larger fillets, first of all. So we've got this edge here, this one, this one, this one, same on the other side. Let's go back to the home view, and let's apply Let's go for five mil. See how that looks. Let's click Okay there. Looking good. Let's press F on the keyboard again, apply one more fillet. Make sure we got tangent chain turned on here. Let's select this edge and this one, and that will chain all of these edges together. And let's just apply a small fillet there. Let's go for one mil. Press Enter. That's looking nice, okay? Let's save that part. We call that holder tutorial, save that. And let's just make an assembly and make sure that these dimensions work. Let's go on a new design. Let's go on our data panel. Let's insert the coaster holder. So I call it holder tutorial, insert into current design. Let's go ahead and put one coaster here, insert into current design. Let's go to position this somewhere up here, although actually, it looks like a perfect fit. Okay, let's just chuck that up here. We can apply a joint there. Let's it J on the keyboard, and then we want to select the center of this circle here. So at that point there, we want that corresponding to the center of this circle here. Okay, that's looking nice. And let's see how that looks with our glass as well. Right click. So this is a part that I modeled up separately, but feel free to draw your own mug or glasses you need. And just kind of check that in there. Roughly like so. Let's go okay. See how that looks. That needs to come down a bit. Yeah, something like that. Yeah, that looks good to me. Okay, and there we have our coaster and our coaster holder. Hope you enjoy the exercise. And if you are three D printing, please feel free to print off this design, and I'll see you in the next exercise. 93. Mario Stationary Holder 3D Printing Exercise: In this exercise, we will model a desktop stationary holder. So I've input these pens here. This is where you store, pens, pencils, rulers, and such. And it's quite a cool little piece to go on someone's desktop. This can all be three D printed, by the way. How you three D print this would be up to you if that would be one piece, or most likely you'll be going for individual pieces here. But that's up to you and how you command that in the splicing software. If you do go ahead and three D print this, please do send me a picture I very much like to see, and I hope one day that I will three D print this as well. You want to model this part yourself, I've done some rough dimensions here. That should be enough to enable you to model this. But aside from that, for the remainder of this lecture, I will continue to model this myself. So let's go into a new design. Instead of doing this as an assembly, so drawing all individual parts and then bringing them together, I'm just going to do this in one design. So first of all, I'm going to start with the base. Let's set R on the keyboard then rectangle tool, and let's do this on the XY plane. I'm going to start at the origin. So two point rectangle, bring that out. The dimensions are 150 width, press tab, and 80 on the height. Let's finish that sketch. E on the keyboard extrude, and let's bring that up by, let's say ten mil. And let's add some fillets to that, press F on the keyboard. Going to drag select one, drag select two, three, and let's get that fourth one in there as well. Fillet dimension, five mil, press Enter. It's looking good, we can apply an appearance to that later. So we'll give that A an earth like appearance. Moving on, let's do the grass layer. So that, in this case, is the green layer here. Let's go let's go create sketch and then select this face here. And to do this, we can just simply offset the perimeter of this box here. So come in to modify offset, make sure we've got chain selection turned on and select the edge there. We can bring that out, but not that big, let's offset that by two mil. Press Enter. Looking good. Let's finish that sketch. Let's hit E on the keyboard and extrude. And we want to select two profiles, the one we generated here and the original one of the body down there. And we want to extrude that like so, but let's go for a distance of five mil. Now, this is going to have a different appearance to the kind of earth block below. Therefore, for the operation, I'm going to go new body. I just simply assign a green appearance to this new body. Come into our bodies folder. Yeah, we've got body one, which will give the earth appearance, and body two will go for the kind of green grass appearance. Next, let's model in the let's go for the actual stationary holder itself. So I'm going to hit C on the keyboard circle tool and I'm going to select this face here. I'm going to put that circle anywhere for the time being, and I'm going to give a diameter of 50 mil enter, and then I'm going to offset that to modify, offset, select that circle, pull that in. That should be the negative, yeah, negative distance. Let's go for a wall thickness of let's go for a four mill for three D printing that will be strong. Row D on the keyboard and place this center point. Let's go centerpoint then to the vertical on the left. And that dimension there is let's go for 38 mill, and then centerpoint to the top horizontal. Let's go. So let's go for halfway. So 42 mil. Let's it E on the keyboard, and let's extrude that profile we made there. Let's bring that up. And we'll extrude that by a distance of 80 mil. And operation, we could go for a new body as well as this will be a different green appearance to the grass layer here. So. We've got our three bodies in our bodies folder there. Let's create the head of this tube, then. Let's go C on the keyboard, and let's do that on this face here. And let's snap to the center point of this circle. Yeah, so it should appear there. Blue circle. Click there once, so we snap there, bring that out. Let's go over 60 mill. It looks okay to me. Yeah, let's finish that sketch. And that's at E on the keyboard, and we'll select this profile here. We want to extrude down, okay? Something like that, except not too much. So this is a negative, so negative 15. Press Enter. It's looking nice, okay? We've got a holder there for our stationary. And feel free to change any of these dimensions if you want this diameter to be bigger or positioned elsewhere. Yeah, please feel free to do so. Let's tidy this up by applying some fillets, Let's it F on the keyboard. Let's go for one, two. Let's go for three and four, as well. For a fillet, let's make this quite discrete. Let's go for one mil. Tidy that up. I'm just going to turn off the edges. So it just looks shaded. There we go. Yeah, that's looking nice. Here, let's put those edges back on, then. Let's do the next feature then, which will be this cube and also the flagpole flag itself. So let's do this on this face here. We're going to press R on the keyboard and select this face here. So we're in the rectangle tool, go to draw in a rectangle, and I'm going to enter a width of 30 and a height 30, as well. So square. D on the keyboard, put this in position, select this line. Let's go to the right to vertical. But that's 20 mil. And let's put in a constraint to lock this in place. Let's go for a horizontal constraint between this point here and snap on to the endpoint of this arc. This one here. There you go. That's fully constrained. Let's finish that sketch. Put E on the keyboard, then, select that profile. We're going to bring this guy up. And let's make this a cube. So let's go for 30, enter, and maybe we could make this a different appearance as well. So if we right click on that feature, edit. Let's go new body or so. Press Okay. Let's go ahead and do the flagpole, then. So let's see on the keyboard circle tool, select this face here. And I'm just want to put a circle in anywhere, and we can constrain that in position. Diameter six, Enter. Let's use the horizontal constraint between the center point here. And hopefully we can get the midpoint here. Yeah, so as you see we snap on there, hold down shift on the keyboard. Click once. That's good. And now it's constrained, so we cannot move it up and down, only side to side. So let's get this in the middle. Let's use the vertical constraint, center point, hover over, hod down shift, snap onto the center point, fully constrained, looking good. Let's finish that sketch to E on the keyboard. Let's extrude this profile here. And let's bring that up by 100 Mill. That's for maturing. Press Enter. That's our flagpole. But again, I want to right click edit feature, and make that a new body as well. Assign its own appearance. And the next up, we need to add the ball at the top of the flagpole and also the flag itself. So to do this, we need to sketch on a plane that's currently not there in our original, so the default planes. We've got the XY, Xs and the Ys, then not in position we need. So we need to construct a plane, set the drop down under construction, and let's go on a mid plane, and let's select this point sorry this face here. And this face here, we see that plane appear as a preview. That's correct. That's okay. I'm going to draw that out so you can see it a bit better. I go to make sure that is halfway. Yeah, perfect. Let's go on create sketch, then, and let's select this plane here. And to do this, let's do the ball first. So I'm going to come under Create. Let's do an arc and a three point arc and hopefully we can snap on to the endpoints, but we can't. So let's hit P on the keyboard to project. And what we're going to do is we're going to project this circle here, okay? So we have that projection line up here. That's okay. We should have a midpoint on there as well. Let's go back on the front view then. And let's come up to create arc, three point arc. We can see the two points. So this is the start of our arc. This is the end of the arc. Then we can bring that up. As for a dimension, up to you. I'm going to go for something like this. And I'm going to go for a L on the keyboard line tool. I'm going to snap on to the upper quadrant here, snap on to the midpoint of our projected line, okay, like so. And then we've got a profile here, which we can revolve. Let's finish that sketch. Let's go on revolve. We'll select this profile here. In terms of axis, we'll select this line we drew here. It's looking good. Definitely going on a new body here to make this like a yellow color. It's okay. It's looking nice. Let's go on the home view again. Yeah, we're getting there, okay. And now let's go ahead and model in the flag. So it's up to you how you do this. You could create an extrude cut like a slot or a slit in the flag pole here, and then you could mount in the three D printed flagpiece. But for the purposes of this exercise, I'm just going to draw in the flag, but up to you how you choose to assemble it. Let's create a sketch. And let's go on the same plane, which is no longer visible. So let's go drop down next to construction, and let's select plane one. Drawing on the same plane again. I'm going to use the line tool, and I'm going to select 1.2 0.3 0.4. Okay, that's looking good. Let's apply a vertical constraint to this line here. It's also hit D on the keyboard to mention this line here. Let's go 25. And let's do on the keyboard and from this point to this point, let's do a distance on the axis. Let's go with 34 mil should work. Then we've still got some movement here. So we just need to tidy up these angles. Let's go for an equal constraint between this slin and this line. I'll tidy that up nicely. I'm just going to position this here. But again, if you create a slot in this flag ball here, and then what you can do is, after that's three D printed, you could just insert it, yeah, something like that. But again, for this example, I'm just going to roughly position that here. Let's finish the sketch. And I said E on the keyboard. Let's extrude this profile. You want to extrude in both directions. So direction, let's go symmetric. And let's do a whole length of, let's try two mil. It's a bit too thick. Let's go 1.5. Actually, let's knock that down to one. Okay. So just going to one mil. Press Okay there. Okay, I think that's sufficient as a flag. Now we can go ahead and tidy this up by applying a decal. So it's come under insert. Can hit the drop down, select decal. And then you can insert the Mario flag decal. So I will add this as a downloadable resource, so I feel for you to download it and you can use it as you like. So I'm going to select that. It's under my project folder, press Insert. In terms of face, this one here. I don't want it to be chain faces, so we just want it on the one face, and I'm just going to tidy this up, rotate that 90. Let's go on the front view. And I'm going to scale this up and position there. Okay. That looks good. Press okay. Yeah, preview looks fine. I feel free to do the same on the other face, as well. And next, let's add in the Piranha plant, which I've got in my design just sitting down here. So I've drawn this in another software. It is available as a step file as a downloadable resource, so feel free to download and use that. And to insert that into this design, let's come into our data panel. And where you store that within your project. So here I've got it called Mario, well, it should be piranha plant, but Mario flycatcher, right clerk, insert into current design, just like in an assembly. And there we have that part there. I'm just going to check that roughly there for now and rotate that. Go for 90 degrees plus okay. I'm also going to chuck in a pen in there as well. So I've called this CO Pen, insert into current design. And just go to lift that up. And let's rotate this slightly as well. Let's go 90 degrees. It's okay. Close down the data panel. We can just tidy this up. So we could apply a joint here. Let's go J on the keyboard, and let's select the center point of this circle here, left click once. And let's select this point here, then we can adjust it manually. So I'm just going to roughly place this into position, something, something like that. Let's press okay there. And for the pen, I'm not going to do a joint for this, but I'm going to come into my browser where we've got the part, right click and then we're going to select move copy. Then we can just roughly move that into position. Let's go on the top view. Okay, something like that. So yeah, I've included both these as downloadable resources, so feel free to download both stephls and you can insert them. And then the only thing left to do is to apply some appearances. So let's start off with the sphere at the top here. Sit A on the keyboard. And for this, I'm going to come under paint glossy, and then just going to apply yellow, enamel glossy yellow and just bring that over, make sure we got bodies selected. Okay, select that body there. That's looking good. Let's also do the flagpole as well, so I'm going to stay and paint go for the white here. Select that body there. That's looking good. Let's do the tube here. So for this, I'm going to type it in LED. Then if we come down, we've got our LEDs here. I'm going to go for green in this case, okay. Drop that on that body there. And then for the grass layer here, let's go ahead and let's just apply a paint green. But this is too dark for my liking, so we can change that. Feel free if you like. Gonna right click on that. I'm going to select Edit. And then within my options here, I'm going to move the shader slightly more towards the yellow, something I think something like that's quite nice. More of a green grass appearance, press done. And then for the Earth like color, which will go on the lower block there and also this cube here, let's go let's assign another color here. So let's add blue up here, and then apply this to the block and also to the earthy compound below. Let's right click on that and edit. And that's the justice. So more of an earthy kind of brown color somewhere over here, that over here. Yeah, something like that. I think that's okay. Feel free to play around with those as much as you like. And there we have our complete model. That looks quite nice. Let's turn off the lines, then. Let's just go shaded. I think that looks really nice. I hope you enjoyed that lecture, and I look forward to seeing you in the next one. 94. Wall Mounted Hook Exercise: In this exercise, we will model this wall mounted hook. So for the base plate, the sheet metal part here, that's very simple, basic extrusion. We can use the whole tool for these counter sunks. The sphere on top, very simple. Use the revolve tool. But the only difficulty is the arm. And for this, we're going to be using the loft tool. So if you want to have a modeling this part yourself, I have created a drawing for this with the dimensions here, so feel free to capture this and have it go yourself. But for the remainder of this lecture, I'm going to model up this part. So let's go on a new design. Let's all start off with the base plate then. Let's it R on the keyboard, rectangle tool. And let's select the Let's go for the Y Z plane. That's the most logical for this part. Start of the origin, and let's drag that out. Wick through the part. We've got 60, tab on the keyboard, and the height. We've got 20. Let's Enter. Let's go ahead, press E on the keyboard. Let's extrude this. Let's come out in this direction. Definitely not by that much. Let's go for three mill. Let's Enter. And let's it F on the keyboard. Let's put in our fillets on this edge here, and we also want this edge here. This fillets have a radius of ten. Okay, looking good. Just go to turn off the edges, visual style shaded with edges. Now, let's go ahead and put in some points, and we use the whole command to put the counter sunks in. So let's create a sketch and we'll do them on this face here. Let's come to create point. And let's put in these roughly one, two, three, four, something like that. Use the horizontal constraint between these two, and horizontal between these two, as well. And let's go ahead and press D on the keyboard. Let's come from the center point of the first hole to the top horizontal line. That's five mil. And then we've got the center point there to this line here, which is 45 mil. And this one here to this one, 15, and this one from the top here is also 15. Could mirror those across. But in this case, I'm just going to add the one dimension. So I'm just going to select instead of entering a value in the parameter box, I'm just going to select this dimension here. So if we do change it, that change will be reflected in the opposing one as well. Likewise it's going to do the same for this guy. Select 15. Enter, that's fully constrained. Let's finish that sketch. Use the hole tool and make sure we have multi hole selected, coming in for one, two, three, four. Okay, those holes are particularly big. In terms of distance, we're definitely going through all. Want to go for a counter sunk and we just want a simple hole. So as for the drawing, we got four holes. The countersunk is six mill, angle is 90, and the diameter of the hole is three mill. Let's enter. That's looking pretty good, okay? Now let's go ahead and add in the sphere, which will be sitting somewhere up here. So we don't have a sketch plane up there currently. We're going to have to insert one. So to do this, I'm going to select a mid plane between this face here and this face. Okay, I'm going to press Okay there, bring this up roughly so we can see looking good. Let's press Let's have a C on the keyboard circle tool, and we'll select the plane that we drew. I'm just going to drawing the sphere here. So it's got a diameter at 15 mil. Hit D on the keyboard, and let's position this. So we know that the center point to this corner point here that's got a dimension of 25 Then we've got a height of 40, and that's also from this corner point here. It's 40. Okay, it's looking nice. Let's go for the line tool then so we can select a revolution line. Okay? I'm going to put in a straight line there from the top quadrant, let's finish that sketch. It's gone the revolve tool, select one of these profiles here, and under the axis, we'll select that line we threw in. Okay. So there we've got our sphere and our wall mounted bracket. We just need to put in this arm. So I'm going to use the loft command for this. So I need to draw two profiles, one on this face here, and then one somewhere within the sphere. So let's go let's go for the line to then, press L on the keyboard, and we'll model on this face here or sketch. I'm just going to roughly draw it in a triangle, something like that, and that should be a complete profile. That's good. Let's go on the dimension tool then between these two points here. And that's got a dimension of 16 mill. And I want these two angles to be the same. So I'm going to use the equal constraint between these two lines. That's looking nice. And now we just need to define where this goes. So let's use the coincident constraint on this point here. Then if we can find the midpoint line by holding down Shift, it's just there. That's perfect. That's fully constrained. Let's finish that sketch. So that's one of our profiles there. And then we just need to insert the other profile, which will be in the center here. So to do this, we need a plane to draw on in the center of this sphere. So let's go and construct and offset a plane. Let's select this face here, we can bring that plane up. That's got a distance as per the drawing. It's 40 mil. Let's enter. Let's make sure that does intersect where we want it to go on the front view. Yeah, perfect. Alright, let's get a sketch on this plane then. Let's go and create sketch. Let's select this plane here. I want to project this sphere onto that plane. Let's hit P on the keyboard, then. In terms of geometry, we want to make sure here that we have bodies selected because this is a different body from this one. We know that from the two bodies in the body's folder. So make sure we have body selected, select this body here, presso. Then we should have a center point there and also the exterior of the sphere has been projected. That's great. We can see it there. For the circle tool then, and let's start at the center of this circle. And let's bring this out. I'm just going to go for eight mil, but feel free to adjust this. How like it. I just chose eight Mil, and that's going to be my profile in the center there and this one here for the loft command. Let's go and finish that sketch then. Let's see if this will work. Let's go and create Loft. Okay? So we want to select two profiles here. Let's go one. Let's go two. Alright, interesting. Okay. So as in the preview, it's not exactly what we're after. So what we can do is just come up to our profiles here. I'm going to change the connected to direction. Okay? And then we can adjust that, right? So we can do something funky like this. I bring that out roughly like so. Let's go direction on the second profile, as well. Okay? Actually, that's looking quite good. But again, you can adjust this how we like, so it can move it around. Gonna go for ten on the top, then profile one. Got it it's eight of the minute. Okay, so I'm quite happy with that preview, but right now it's doing a cutting operation, which is not what we want. So let's change that too. Let's go for a join. Looking much better. Press okay. I think that's come out quite nice. Then, of course, let's apply an appearance to this. So press A on the keyboard. And for this, I chose a brass. So let's go into metal. Going to brass, and I went with brass polish. So I'm just going to drop this here. That should be on all the bodies, as we can see. But clothes there. Looking nice. Let's turn off those edges. Visual star shaded. There we have the complete part. That's looking good. If you managed to do that yourself, especially with the loft command, big, well done, and hope you enjoyed that exercise, and I look forward to seeing you in the next one. 95. 3D Modelling Exam 1: In this exercise, we will model this part here. And this is quite an interesting part because it takes advantage of a lot of different sketch techniques and also modeling as well, particularly using construction planes. If you'd like to model this part yourself, do have a drawing that's fully dimensioned, which is here. So feel free to use this, but aside from that, for the remainder of this lecture, I'm going to model this part myself. So where to begin, I would recommend starting off with the base plate here. That's just a simple extrusion, we could include a number of these features here, and then we can move on to the remaining bodies here, and then finally we can finish off with the flange just here. So let's start a new design. And let's press R on the keyboard. So rectangle tool, we're going to start on the plane. Let's start from the origin, and we'll give this rectangle. So we're just doing the base plate here. We've got a Wik has Poller drawing, 64 mill, press tab on the keyboard, total height, 15 mil. Then we can use the line tool and add in some of the other features. So I'm just going to draw these in roughly. So we're going to come down, something like that. Come across. We've then got a circle here, so I'm going to hit C. Gonna give that a diameter. So it's an arc, in this case, five mil, so diameter ten you can use a horizontal constraint, not midpoint of the circle, coincident constraint, endpoint to the circle. Continue with the line tool then. Let's snap on to the right quadrant of this circle. Come down, bring that across. And we just want to extend this line here to be in contact with the circle. So just bring that up slightly. Going to modify, extend, hover over this line. We see the preview. That's good to me. Let's finish that there. Press C on the keyboard and put in the through hole. So concentric with this circle. Let's start at the center point. And that's got a diameter of four mil. Now we can go ahead and start adding some more dimensions. So from this line here to this one, we have a distance there eight mil. And then from the origin to the center point of these circles, we have a dimension 36. From this line here to our origin, the dimension there is nine mil. And last dimension should be these two, which is five mil. That should be fully constrained. Let's just check in our sketches folder. Yet, we've got the red padlock. That's perfect. Another thing we can do here is to add in the fillets. So we could do those in three D mode. I'm going to do them in sketching for now. So I put in a circle here, so it's got a filllet of two, so rod of four, same for here, four, and the same down here, four. Let's use the tangential constraint now. So circle to vertical, circle to horizontal, circle horizontal, circle circle, and circle. Let's go for the horizontal and circle circle. That should be all the profiles that we need. L's finish that sketch then, E on the keyboard. So like this profile. Let's get our fillet in there as well. Also, this fillet this circle. We want to have this fill it here and also this one. I think that's all that we need. Let's bring the arrow out. Have a look at that. Yeah, that's looking good to me, okay? So the depth of this part is 50 mil. Let's press Enter. That's looking nice. Let's go ahead and add the fillets then on each of the four corner edges. Let's press F on the keyboard, select this edge, this one, drag select this one. And we need this one as well. So four edges, and these have a rat four mill. Let's go back to the home view. Now we can start to add in our through holes. So one in each corner, I suggest that we sketch them on this face here, and we can mirror these across to the other side here so we can extrude cut through all. So let's hit C on the keyboard, then. I want to make sure that we select this space here. And we're going to start our first circle from the center point of this arc. So if we just drag down, we'll see that blue circle appear there. So we've got four holes at three mil each. That's our first one. Let's add in another one, then again, find the center point of this arc. Okay, three mill. And in this case, we're going to project this entity here, and this entity here, that's okay. Let's go on the circle tall again. Then from the center points three and one more here three. You could mirror those across if you like. So our four profiles there. Let's finish the sketch. Let's go on E extrude, and select the first profile, second, the and the fourth. Let's pull the arrow down then. So yeah, we've got the operation cut. In terms of the extent type, we want to change that to all presser. Okay. Then we have our four hole features. That's nice. Okay, so that's all the features for the base plate. Let's go back to our model then. And now we've just got this feature, this one, this one, and the flange. Let's now move on and input this kind of pipe feature here. So to do this, let's put the sketch. We're going to start at the top of this feature and then extrude that down to these bodies here. So to do that, we need to construct a plane. We need to offset that offset that from the bottom here, actually. And we can use the dimension 40 mil. So in this case, it'll be -40 mil to get to the top of this circular feature. Press C on the keyboard, and let's select this plane here. And just going to draw these two circles in anywhere. So outer has a rad of 11. So let's go 22 diameter and C on the keyboard. Let's do the inner. So inner is nine, so diameter 18. To position these, we need to refer to some of the entities here. So I'm going to project these up to this plane. Select. Let's just go for this entity here and press Okay. So we see we've now got that entity there. And let's go on the horizontal constraint center point of the circles. And let's find the midpoint of this line by holding down Shift. We've got the midpoint there. Let's go back on our top view. It's okay. Now we see we're constrained there. We just need to position this on the X axis. So let's dimension, and we'll select this point here to this line, and we'll just do half of the total width. So 64/2, enter. It's now fully constrained. Let's finish that sketch, then. We've got our profile there. E on the keyboard, select that profile. Make sure that we're going down. We don't want a cutting operation like so. Definitely want that to be Let's go for a joint operation. And in terms of the extent type, let's go to object. Let's select this one here. However, there's a slight problem in doing this. And if we come over to our bodies and I hide our existing body, we'll see that we're getting a lot of conflict of material, which is not exactly what we want to have. And so under extend, let's go to adjacent faces, and let's see how that changes there. So we see here the material of our extrusion will only go down until it contacts any of these bodies here. So, let's press Okay. That's looking good. And we've also got these slot features running through this cylindrical feature as well. So let's do a new sketch. Let's go on this face here. Let's project this circle here, and we can reference this point. So I'm going to project this circle here. Okay. We've got that point in there. It's going to create rectangle to center rectangle, select that point and bring out a rectangle there. The width of this slot is five mil plus tab on the keyboard and the distance or the height just has to be farther than the extent of the circle. So just about 35. Let's finish that sketch. Let's set E on the keyboard, then, extrude cut. Let's go this profile and this one. If we bring the arrowhead down, we've got our slot coming to play. So depth of that slot, we've got 8 millimeters. So in this case, yeah, minus eight. That's okay. Now we've got our slot feature looking nice. Now let's work on another feature. So let's focus on this one at the back here. So let's the drawing, we're going to follow the same process. We're going to create a plane, do a sketch on that extrude down until the extrusion meets these faces here. So let's go and construct, offset a plane. Let's offset it from the base of our base plate, and we'll bring this up. So this starts 29 mill, so -29. We're going to press let's R on the keyboard, rectangle, make sure we select this construction plane. I'm just going to roughly draw in a rectangle or something like that. Press D on the keyboard. Let's give this guy a dimension here. We've got 14 mill and I'm also going to put in a coincident constraint between the endpoint of this line and this line here. I want to make sure this is in the center as well. So I'm going to move this one up slightly. Then I'm going to use a coincident constraint, hold down shift, select the midpoint and hold down shift, select the midpoint of this line here. That should be in the right position. Now, we only want one profile, which is up until this arc here, right now, the whole thing is being selected as a profile. So what we're going to do, we're going to project and we're going to select an entity. So this one, okay. And then we've just got the one profile here. That's exactly what we want. Let's finish that sketch, then. And that's at E on the keyboard, and we'll select this profile here. We're going to bring this down. So again, not a cutting operation. Let's go for another join extent type. Let's go to object. Got to select this face here. I want to make sure that we select two adjacent faces. Okay? Let me just hide the existing body. Yeah, that's exactly what we're after. Let's press Okay. And then we just need to give this edge here, fill it. So F on the keyboard, select that edge. And we've got a fillet there of five mil. And we've also got this through hole on this face here. So let's go C for circle, select this face here. And that starts at the midpoint of this arc. Sorry, the center point of this arc. We'll bring that down, find the center point there. Let's bring that out. Got a diameter of three. E on the keyboard, select that profile. Bring that in this direction. Extent type. Let's go through all make sure the operation is cut. Press okay. Here we go. We're getting there, looking good. Okay. And the last two features that we need to add are the flange here and also this pipe. So to do this, we need to sketch on a plane here. So we're going to make another construction plane, and we'll go from there, create the flange and the pipe also. So a little bit tricky to do this. In terms of construction planes, the one I would suggest to use here would be a plane through two edges, so we can just sketch these in. Let's use the line tool then, and let's do a sketch on this plane here. Use the line to in. Let's draw down a line, something like that, let's dimension this point to this point. And that is 15.04. And this point to this one here, we've got 36.25. We know this line is at a 45 degree angle. So let's hit another line. Me that construction, draw this with a horizontal constraint D on the keyboard. Dimension these guys. Let's go 45. And we've still got some movement going on here. So let's apply one more dimension between this endpoint here and this endpoint, which we can't select right now, so we're going to need to project. Let's project an entity, this one here, press Okay. We see we've now got that point there, dimension between these guys. And the distance there is 14.75. Yeah, that's good. That lines now fully constrained. Let's finish that sketch. Let's create another line on this face here. So let's go L on the keyboard and select this line here, and we could just project this existing line. So let's hit P on the keyboard and select this line. Press Okay. Now we've got these two edges here. We can form that plane. So let's finish the sketch. Come under construction and go plane through two edges. We can select these two edges here, press okay. Then from here, we can start sketching. So let's model in our flange first, and then we can do the pipe, which will be extruded down to these bodies there. We no longer need to see these sketches, only the construction plane. So let's go into our sketches folder. We can hide. In this case, it's a sketch nine and also sketch ten. We're just left with the construction plane. So let's go on create sketch, and we'll make sure that we select this construction plane here. We're looking at that perpendicular. That's correct. G to first of all, draw in the let's go for the through hole. So this has a diameter of 16 mill. We can position that roughly over here. So as for the drawing, there's not a fixed position, and so it's up to us here to make an assumption. In which case, I'm going to assume that it snaps on to this arc here, and that it's vertically constrained with, let's say, this arc here. So to do that, I need to project some geometries. Let's hit pee on the keyboard. Going to project, not that one. I just want to project the single entity down there. And also, let's go for this one, press Okay. And then if we move our circle over, so it does drag over, use the vertical constraint between the center point of this arc and the center point of this circle. Okay, yeah, that's looking good. And then we can just go ahead and snap on to this line here. So we can use the cointinentra, center point of the circle onto the arc. Now that's fully constrained in the right position. That's looking good. Let's go ahead and draw in the remainder of our flange then. So to do this, let's go and create. Let's go rectangle, center rectangle, start at the center point of the circle. Drag this out. We've got dimensions 30, tab 30, 30 square. And then we also got the four holes. They're three mill diameter each on a PCD of 30, so pitch circle diameter for a C on the keyboard. Add this in as a construction line, D it to account as any profile. Let's at 30 diameter for our PCD. I set C on the keyboard again, then, and we're just going to snap on to this location here, the intersection between the PCD and this construction line. Going to turn off construction here. Add 03 mile circle. Then very simply, we can go create circular pattern, select that circle. And the center point would be the center point of these circles. Full distribution, 360 degrees and quantity, we're going to go for four. It's press okay. It's looking quite nice. Alright, I think we're almost there ready to extrude. Let's finish that sketch, then, E on the keyboard, select our profile or to make sure that we're extruding in this direction, not in this direction, okay? Because when we put in our construction plane, it was this face of the flange. And so the distance or thickness rather of the flange, we've got four mil. Let's also go ahead and add in our fillets then. Let's press F on the keyboard, like one edge, two, three, if I can get that one and four. And the to have a round of five mil. Press Enter. Looking nice so far. We just need to add in the last feature, which is the pipe section. So let's create a new sketch, and let's go on this face then. And what I'm going to do here is I'm just going to hide body one, just so that we can see the flange more clearly. Let's go back a look at that. And let's set on the keyboard circle, start at the center point here, and we're going to bring this out. So let's put the drawing. It's got a diameter of 20 mil.'s enter.'s finish that sketch there. Let's put body one back. And let's sit E on the keyboard extrude, select this profile here. Make sure we're going in the right direction. Yeah, okay. We don't want a cutting operation. Definitely want to join. And under the extent type, let's go to object. Let's select this object here. Then make sure we have two adjacent faces. Have a look at that. Yeah, that's looking really nice. A join function as well. Okay. There we go. So that is our complete model. I hope you enjoyed that. And if you were able to do that yourself, yeah, big well done. That's good use of multiple sketch tours techniques and also the use of construction plans as well. So you need to be quite methodical when we're modeling parts like this. Hope you enjoyed that, and I'll see you in the next exercise. 96. 3D Modelling Exam 2: In this exercise, we will model this part here. And this was sent to me by a student in America. This was one of their CAT exams when they were studying at university. If you want to have a go at drawing this part yourself, feel free to refer to this drawing here. And for the remainder of this lecture, I will have a go at modeling this part myself. So in terms of where to start, we could start, well, we could start at any of these three bodies, really. I'm going to start with the most complicated one, though, which is this one here. It requires some unique and slightly complex sketching techniques. So let's go ahead and start a new design then. Let's first of all start off with this through hole, then. Let's go see on the keyboard. Let's go for a circle tool, and let's do this on this plane here, the plane. Let's start at the origin, and the through hole is diameter of 40 mil. That's okay. And let's do the four mounting holes on this part. So to get these into the right position, I'm going to use the creation tool and I'm going to have a rectangle. And let's go for a center rectangle, but I'm going to make this a construction because we don't want to take into account its profile. We bring this out by the distance between these mounting holes, which is a square 80. And then we know that each of the corner points of this square are these holes. Sit see on the keyboard, turn construction off. And let's get one of these holes in. That's got a diameter of four holes by 16 mile diameter. Let's go ahead and pattern these around to each of these corners then. Let's go create circular pattern, select the circle, and we'll choose the center point as the origin here. Let's go over a quantity. Let's go four. Okay, and that'll be revolved around 360 degrees. Let's press okay. It's looking good. Then from here, we can get the walls which surround these holes here, which have the same center point. So let's see on the keyboard. It's going to start here again. Let's start a midpoint, the center point there. And we'll bring this out by that's got a rod of 20, so diameter of 40. And let's again, use the circular pattern tool. Let's get this guy and around the center point here. Let's go for 4/360. Press okay. That's nice. And now we just need these arcs sitting in here. So to do this, I'm going to use the circle tool. I'm going to draw out a circle. And we know that the radius of this arc is 55, so I'm going to enter 55 times two, so 110, move this circle up here. I make that tangential. So tangent constraint between this circle and this one and this circle in this one. Then quite simply, we're going to circular pattern, this circle, center point, origin, 4/360, press ok. And there we have our profile including these profiles here to which we want to extrude. Let's finish that sketch, then. And that's a E on the keyboard and select the according profiles. So we definitely want this one. These guys and also these guys down here. Let's just get a preview of that, make sure that's coming out correctly. Yeah, that's what we're looking for. And the distance as per the drawing is 20 miles Enter, there we go. We've turned that fairly complex sketch into a nice three D extrusion. Got the chamfer to do on this edge here, but we've also got the chamfer on the edge on the opposing flange, as well, so we can do those in the same operation later. But let's continue then. So we've got this. We've got a pipe joining them together. Let's hit C on the keyboard. Let's do a sketch on this face, start the origin. And we're going to bring this out we've got a diameter of 60. Let's set E on the keyboard, and that's extrude that profile. Just draw that out. Yeah, that's looking good. We've got a distance there of 100 -20, that's 80, but plus we want the 20 of the opposing flange, as well. So if we do this 100, it's okay. That's looking good, let's get this other flange in there, then. So let's go for I want to do a rectangle on this face here. Let's go and create sketch, select this face here. In terms of the rectangle tools, in this case, we're gonna use a three point rectangle. I'm just going to draw this in just roughly, something like that. And we can use constraints to position this. So let's go for the horizontal constraint. Sorry, vertical constraint between this point and the origin, also this point and the origin. And I want to bring this guy up, and I want that to be made horizontal. Let's go horizontal, this point to the origin, and this point to the origin, as well. It's looking good. We can go ahead and dimension that. So we got 120, so total length of this line to 120. It's 120 square. It's looking nice. And now we can get the four holes in there as well. So as per the drawing, we're not given a dimension on the distance or the offset between the center point of the circle and the origin here. So we're going to have to get a little bit creative. Let's set C on the keyboard and put in one of these circles. And we've got A. There's four of these by 20 milli diameter. And we're going to do the same over here as well, 20 milli diameter. Goa put a vertical constraint between the center point of this circle and the origin and a horizontal between this one and the origin, as well. And we've got a distance between the center point of this circle and the center point of this circle at 80 mil Okay, that's looking good, but there's still quite a bit of movement going on here. We want the distance from the center points to the origin to be equal. And this is where I'm going to use some construction lines. That's it L on the keyboard then. Let's turn these as construction. We'll do the center point of the circle to the origin, and origin to the center point of this circle. And then there should still be that movement there. We want these two lines to be in the same distance. So we use the equal constraint, select this center line. Sorry, select this construction line and this one. And now that should be fully constrained. Let's just have a look in sketch. Yeah, we've got the red padlock fully constrained. It's looking good. Let's go ahead and draw a mirror line then. Let's start at the midpoint of this line, and we could just come up to the origin, actually. Now, let's select the mirror command, select these two circles and our mirror line. We use this construction line here. That's okay. Put our four holes there. That's good. Let's finish that sketch. Let's E on the keyboard, select this profile. And we actually want to extrude in this direction. So we want that to be a join operation. Definitely not a cut. And we're gonna go for a distance of we got 120 -100, so that's 20. We're gonna go -20. Make sure that's in the right direction. That's nice. Get these fillets on these sharp edges, then. Sit F on the keyboard. Gona drag select this guy, this guy. This one. Let's do this one as well. Okay, got four edges selected. And the fillet, in this case, it's got a rad of 20. Let's enter. Looks nice. Let's get the hampers in there as well. Let's go modify hamper this edge, this edge as well. So it's a 45 degree Shampa equal hamper. And we know the whole is 40 mill and the outer diameter, this pipe is 60. So that would that'd be ten mil. Ten champa equal, that should make as per the drawing. If we hit inspect, it should make this circle 60 correct. And this circle here, just clear that. This circle here is 40. That's correct. As per the drawing. That's nice. Let's go on the home view, then, and of course, let's apply an appearance to this. I'm going to go for a copper in this case. So under metal, kind of copper. I'm going to go copper polished. Just drop that in here, close. Then we have the completed model. That's looking really nice. If you were able to model it yourself, working from this drawing here with all these dimensions, I know it's quite hectic. Yeah, big, well done. That's really good. You enjoyed that exercise, and thank you very much for watching.