Autodesk Inventor 2025 - Complete Beginners Guide

1. Promotional Video: Hi, everyone. My name is Chris and welcome to the Autodesk Inventor, 2025, complete beginners guide. I am an automotive design engineer with extensive experience in off road vehicle design and military applications. With over 15 years of experience, utilizing various CAT softwares, I have found Autodesk inventor to be one of the most comprehensive and user friendly industry standard tools available. This beginner friendly course will guide you step by step through the powerful capabilities of autodesk inventor. Whether you are an aspiring engineer, an engineering student, or a professional working in the industry, this course is designed for you. Throughout this course, you will learn how to navigate the various file interfaces, create paths and sketches, build three D assembly models, and produce detailed two D engineering drawings to industry standards. Throughout the course are exams and tests that will enable you to apply the skills and techniques that you will learn. This course is structured in a logical order to build your skills and knowledge in this powerful CAD software. And by the end of this course, you will possess the necessary skills to use Autodesk Iventer for personal projects, academic work, or professional engineering tasks. So let's dive into the world of three D mechanical design. 2. Course Overview: This course consists of seven sections, which are structured in an order that provides a progressive learning experience, enabling you to enhance your understanding of inventor's tools. By the end of this course, you'll have the skills and knowledge necessary to create a wide range of designs at an intermediate level. So let's explore each one of these seven sections. In the first section of this course, we will explore the home screen interface and navigation. Specifically, we will cover how to create and edit projects. As part of this process, we will create a dedicated project for this course and its contents. Additionally, we will take a look at the default templates supplied within inventor and focus on templates for parts, drawings, and assemblies. This will include an understanding of the properties associated with each template type. Lastly, we will learn how to determine the units for different file types. This will ensure that we can confirm whether we are working with metric units, for example, millimeters and kilograms or imperial units, I inches and pounds, based on the requirements of the project. The second section, we'll focus on part files and sketching. We'll begin by exploring the user interface of Part files, understanding the available tools and their locations, and additionally, we will learn how to customize the environment, including adjusting settings such as background colors and other visual preferences. Next, we'll take a look at the fundamental sketch tools. We'll cover a variety of options, including the line tools, rectangular tools, hex tools, slot tools, circle tools, and of course, the arc tools. Following this, we will explore the fundamental sketch modification tools that allow for precise adjustment. We will then move on to patterning sketches, so how we can implement linear patterns, circular patterns, and sketch mirroring techniques. Within sketch mode, we will also cover dimension control, and I'll give you a detailed overview of constraints and how they can be used to accurately define geometry based on specific requirements. To reinforce learning, I will provide three practice assignments under sketching. These are designed to help you apply the tools and techniques covered in this section. These assignments will test your knowledge of sketching fundamentals. Should you have any questions during these, please don't hesitate to reach out to me. And finally, in this section, I will present three sketching examples where I will demonstrate how to create fairly complex sketches using all the tools covered in this section. I would encourage you to attempt these sketches on your own before watching the full demonstration. In Section three, this is where we will begin three D modeling. We'll start off with the extrude tool and we'll learn how to add and remove material to our parts. 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 and embossed texts such as logos, brands, part numbers, and similar features. Moving on, we'll study the shell and hole features and how to apply threaded features, including both male and female threads, IE for fasteners and threaded holes. We'll then study how to assign materials to parts and customize their appearance for a more realistic representation. You will then be provided with three practice assignments. Each assignment involves creating a three D model based on defined dimensions. And these exercises are designed to test your ability to apply the tools and techniques learned in this section. At the conclusion of this section, you'll have access to three complex modeling examples. Here I will demonstrate the complete process of sketching and remodeling these parts using the tools learned in this section. And again, you are encouraged to attempt these models on your own before watching the full demonstration, but otherwise, feel free just to watch the complete demo. In Section four, we focus on creating assemblies by combining individual three D model parts. We'll start with modeling a bearing block assembly. So we'll model each part required to create the bearing block assembly, and I will guide you step by step through the process of designing these parts. Once the individual parts are modeled, we'll then create an assembly file where we will place and learn how to position each part. After the parts are placed, we'll then study how we can assign various types of mates and constraints to build the complete assembly. Autodisk inventor provides a complete content library. 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. We'll then explore how we can pattern parts within assembly files, focusing on both linear and circular patterns. On top of that, we'll study how to create cross sectional views to visualize and analyze parts that may otherwise be difficult to see within an assembly. Then 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. Finally, we'll cover how to edit existing assemblies, including modifying constraints, repositioning parts, and making any necessary adjustments to achieve the desired result. Section five focuses on creating two D engineering drawings. We will begin by reviewing the default templates available and how we can open and customize them, such as adding new sheets and defining border controls. Using the bearing block assembly modeled in the previous section, we will insert a base view. We'll project additional views from that, and we'll also create sectional views as well. 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 styles, add labels, and include essential information. Following this, we'll learn how to insert dimensions and modifying their related styles. Once the dimensions are added, I will demonstrate how to apply linear and angular tolerances. For assembly sheets, we will cover how to add a parts list and use identification balloons to correlate parts with the parts list and any relevant details. This section will also include a complete example of a generated two D engineering drawing with a bearing block assembly modeled earlier. And finally, I will guide you through how to create a custom title block. While we will initially work with default title box and templates, you will learn how to design your own tailored to your company client or academic requirements. In Section six, we'll explore some additional content that's not necessarily required for additional assignments, but useful for understanding the software better. We'll start with an example of modeling a spring using the coil command, followed by loft modeling based on geometries and features. And next, we'll learn how to split bodies within apart, which is a handy tool for creating separate bodies. And finally, I'll provide a 30 minute overview of Audodsk inventor and a 15 minute summary of two D drawing creation, both designed to be easy to follow based on earlier sections. In Section seven, this includes several practice and modeling examples. This section demonstrates creating parts using the techniques learned in this course. I recommend attempting these models yourself when given the dimensions at the start of each lecture. If you prefer, you can watch the full video to see how we would typically model these parts with the tools that are taught in this course. Overall, this course provides a clear and logical overview and structure for learning autodisk inventor 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 throughout the course, please feel free to contact me. I wish you all the best of luck in your future endeavors in CAD design, and I look forward to seeing you in the course. Welcome to the team. 3. Section Introduction - Homescreen, Projects and Templates: In the very first section, we'll be taking a look at the home screen interface. So we'll be understanding more about what's presented to us and what options we can do as soon as we open up Autodesk inventor. We'll then be taking a look at projects, so how we can create and modify these, and we'll also be creating our first project that we'll be using throughout this course. Then we will move on to templates. So where we click New and we start a new part, an assembly or a drawing, we'll take a look at where these templates are and how we can choose an according one suited to what we're doing. So a nice introductory section to begin with, before we move on to the next section, which is about part files and two dimensional sketching. I'll see you shortly. 4. Homescreen Interface: In this lecture, we will take a look at the home screen interface. So when we open up Autodesk Inventor, you'll be presented with this home screen here. So in the very center, we have the recent files. So right now, if you haven't used Inventor before, you won't have any parts displaying. But when you do work more with inventor, you'll see your parts start to appear here. These always correlate to the project that you're working on. And we can control projects just up here, but we'll take a look at that in a bit. When we do have parts, assemblies, drawings, and so forth in this area here, we can change how they're viewed, so we can look at a list view, we can see the according details there. Or for me personally, I like to have them in grid view, and I can actually see firsthand what these parts, drawings and assemblies are. Can also choose to pin these if we want. So when we do have a lot of parts, okay, let's say it's on a particular project with tens or hundreds of parts, we can use the pin icon here. So if we left click this, you'll see it then gets pinned, okay? And then anything which we don't want to pin, we can click Remove unpinned and that will remove any of perhaps the excess parts that we don't necessarily want to see on the home screen. Okay? And we can left click to unpin that. We can also sort them by categories such as here, so name, date modified, and so forth. A lot to choose from. I generally just have them sorted by last opened. And on the right hand side, if we do have many parts here, we can just do a search in here, just to quickly find them. We can also filter these as well. So, for example, if we're working on them in the last seven days or the last month or we want to see everything under a particular project for the last three months, we can also sort as well by parts assemblies and drawings. On the left hand side, at the very top here, we have our selection of projects. So I'm currently under one of the projects I've entitled udomCurse. Okay? But if we open up this drop down, we can see there I've got quite an array of projects there relating to different projects that I've been working on and so forth. I would always recommend for any project you're working on to create a new project and have a project solely or whatever it is that you're working on. And in the next lecture, we will be looking at how to create a project, okay? So we'll be entitling this, you know, something like, udomi course studies or a private study of Autodesk inventor, something like that. We'll look at that in the next lecture. We've also got the option here to open existing parts. So if you click open, we can then run through our entire PC, looking for an according part to open, and we can also select new, as well. So this is where we would create a new art assembly or a drawing, and we would choose a suitable template for that, which we'll be covering also in another lecture. And at the very top, we do have a selection of tools. I rarely use these, might be using the application options, but do note that the application options are also available to us in parts, assemblies, and drawings and so forth. So at any point when we're using inventor, regardless of the file type we're working on, we can come back to these options here and make any according edits that we need. So we won't go through these just yet, but we will be going through quite a few of these tabs later on throughout this course. That is an overview of the homescreen. It's very user friendly and we'll be using this time and time again throughout this course. I'll see you in the next lecture. 5. Create your first Project: In this lecture, we will create a new project, and this will be the project that I recommend that you work in throughout the remainder of this course. Therefore, it will keep all of your file types under one project. So that's all your parts, all of our assemblies that we do, all of the drawings, and any of the practice drawings that you choose to do as well. So to do this, we're going to come over to where our projects are listed, and we're going to select the three dots here and then select settings. Now here, if you haven't used inventor before, you should just have the default project available, okay? You can work in that if you want, but I would recommend creating a new one, and I'll show you how to do so. So if we come to the very bottom, we're going to select new. We've got the option there for a new single user project and a new vault project. So this we're going to select a new single user project, okay? So this will just be you working on this individually. But next, then we can name the project. Let's go for Inventor 2025 studies. And then you can select the location for that. So if you click these three dots here, you then find a suitable location of where you want for this project to be stored, and then all of your parts, assemblies and such will be stored under that same location. Therefore, everything is stored under this project in one central location. Once you've chosen your location, click next. Okay, and then click Finish. And there we will see that we have a new project pop up, which is Inventor 2025 studies. Now, we can remove any one of these projects. For example, I choose the Ford Everest project, we can right click. We can rename it, browse new, and we can delete it as well. So if you need to do that in the future, that option is available there. The bottom here, it's quite a lot of information. I recommend leaving everything there as the default, okay? So the type, location, also the appearance libraries, definitely keep those the same. We'll be using these in later lectures. Same with the materials libraries. Keep those as they are. Okay, workspace, and the folder options, templates, keep everything as the default. That's all we'll be needing for this course. Once we're finished, if you click Done, and then now you can see that my home screen interface no longer has any parts here. And that's because we've created this new project, and so anything that I create within this project will then be shown here. But for the purposes of this course, I'm going to be staying with my project entitled Edomi Course. Okay, so that's an overview of how to create a project nice and simple, and I'll see you in the next lecture. 6. Templates, Units (Metric/Imperial): Throughout this course, we'll be opening up new parts, assemblies, and also drawing templates as well. I want to show you how to do that here. Now, there are two ways in which we can do this. So from the home screen interface, we can just click on New, and then we have a series of templates here, which I'll go through shortly. Another option to do this is to come up to the top left, and we have the New up here or the shortcut on the keyboard control n. So in future lectures, when I'm working on parts and assemblies, you'll see me just clicking on New in the top left here. It's easy to access. But if I'm working from the homescreen, I generally click New here, but both of those do exactly the same thing. When we open up new, we are then presented with a series of templates which we can choose from. Now, these are categorized. So, for example, we have part templates here, assembly templates, drawing templates, and so on. If we come over to the left, we can see here we have a series of folders. So if we go with English, for example, all of these templates here are in inches. So we can see there the standard part template is in inches. And if we come over to the left, we can see it part template units inches. But the same for assemblies and the same for drawings. And if we come over to metric, we can then see in the standard part file, we're in millimeters, and we can later confirm that. We can see it's part file and the units millimeters. So throughout this course, I'm going to be working in millimeters. I would recommend that you follow and do the same. So when we come under, let's say the part templates. So we always start with parts. We then build assemblies, and then last, we do drawings. Under the parts, you'll see here under the metric folder, we got four options. We have four different templates to choose from. Okay? So we've got two sheet metal options, and we've got two standard options. Throughout this course, I'll be working in the standard millimeter template. And whenever I create a new part, you'll see me select this one and then click Create. So I'll see you in the next few lectures where we will be opening up part templates. 7. Section Introduction - Part Files & Sketching : In this section, we will learn all about part files and two D sketching. Sketching is fundamental to three D modeling, and inventor provides many sketch tools that enable us to construct high quality sketches to the later three D model. We'll start with customizing the interface appearance to create a more user friendly environment, followed by working our way through the broad range of creation tools, modification tools, pattern tools, and also the constraint tools. On completion of this section, you will have the skill set to sketch fairly complex geometries before we move on to the next section, which is three D modeling. Each lecture 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 would recommend that you follow along with and take the opportunity to practice these tools and familiarize yourself with what they can do. In the following sections of this course, I'll be regularly using these tools covered in this section, and so will you. So to start with, let's open a new part file. So we've opened up AutoDesk Inventor. We're presented with a home screen. Let's come over to New. Let's come under our part templates, and let's select the standard millimeters template. That's located under the metric folder. Once we've clicked that, let's click Create. And I'll see you in the next lecture. 8. Part Files & User Interface: In this section, we will learn all about part files and two D sketching. Sketching is fundamental to three D modeling, and inventor provides many sketch tools that enable us to construct high quality sketches to the later three D model. We'll start with customizing the interface appearance to create a more user friendly environment, followed by working our way through the broad range of creation tools, modification tools, pattern tools, and also the constraint tools. On completion of this section, you will have the skill set to sketch fairly complex geometries before we move on to the next section, which is three D modeling. Each lecture 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 would recommend that you follow along with and take the opportunity to practice these tools and familiarize yourself with what they can do. In the following sections of this course, I'll be regularly using these tools covered in this section, and so will you. So to start with, let's open a new part file. So we've opened up AutoDesk Inventor. We're presented with a home screen. Let's come over to New. Let's come under our part templates, and let's select the standard millimeters template. That's located under the metric folder. Once we've clicked that, let's click Create. And I'll see you in the next lecture. 9. Colours & Background Customization: Before we begin sketching and modeling, let's take a look at how we can customize our workspace to suit our preferences. So in this example, the canvas that we're looking at is white in color, and the user interface theme is a light setting. We can change these by coming into the tab called tools here, and then select application options. This window gives an array of tabs to which we can select our preferences. In this section, we'll only focus on the colors tab, which is just here. Now, the options that we have down here is to change the user interface theme. So right now, I've got it under a light setting. We can change that to a dark, okay? So if I click Apply. For me, personally, I prefer the dark user interface theme. Moving on, we have the in Canvas color scheme. So if we scroll down. So right now, I've got presentation color scheme selected, and the background is just one color. So it's just a single color white, in this case. I can change that to a gradient. Then if I click Apply, we can see we're getting a gradient from more of a darker color to a lighter color. And we can do the same for any of these. So quite a popular one is high contrast. If we just go on one color, just black, and then if we change to gradient, we go from a dark gray over to a light gray. My preference here is presentation and gradient, which is this one here. Now you've also got the option to add your own background image. So if we select this, we can then select here an image that we want as the background. Okay, so for example, if I select sky sun two, click Okay. Apply. We then got that as a background. So feel free to choose any images that you have on your PC that you like. But for me, as I say, I'll go with presentation and gradient. So here we have this nice gradient canvas color, which is subtle and easy to work with, in my opinion, I'll be using this option throughout the course. 10. Start Sketching - Planes & Common Tools: Now that we've customized the interface and the Canvas scheme, let's start sketching. Sketching is an essential step in creating any part or model. There are a wide variety of tools available in sketching, and the more you sketch, the more you'll become familiar with these and able to create more complex geometries. In this lecture, we will take a look at the three default planes, and also we'll do some basic sketches using the line tool. So let's begin. If we come up to the top left where the tabs are, there are two tabs here, three D model and sketch. We can select either one of those, and both of those will present us with start two D sketch, or we can press S on the keyboard. So if we left click and select that, we can now see that there are three planes here, the XY plane, Y Z plane, and the X Z plane. Now, these are two dimensional planes to which we sketch on before we start three D modeling. We won't go into detail now in how to choose one of these, but the more you start sketching and modeling, the more that you will become accustomed to selecting the correct one. For the purposes of this lecture, let's select the XY plane. If we left click there, and now we are looking perpendicularly at that plane, and we can begin sketching in this environment. Inventor has automatically opened up the sketch tab, and at the very top here, we can see a wide array of tools available to us. Might seem a bit intimidating at first, but don't worry. We're going to break these down and go through each of them. Now note that they are broken up into sections. So we've got the create tools, okay? So line, circle, arc, rectangle, and so forth. They got the modify tools here, the pattern tools, constraints, and also dimension there. So I'll cover modify pattern and constrain in different lectures, and then in the next few lectures, we'll be focusing on the main tools here, which are the creation tools. Let's take a look at the line tool. So if we come under line, you'll notice there's a drop down, and if we select that, we've got some different options there. So we've got the generic line, midpoint. We've also got splines and curves. So splines and curves are used for more complex geometries, we won't be focusing on those in this lecture. But let's take a look at line and midpoint line. So if we select the line tool, remember we're looking at the XY plane. Bring the mouse over to the working environment, and you'll see this yellow.in the middle. So that's called the origin or sometimes called the center point. Okay? So on the axis system, that is 000. And then if we left click on the center there, so we should snap to it, we'll see that turns into a green circle. Then if we move the mouse around, we can start to draw a line. If we notice there are two dimensions here. One is a linear dimension, so currently 8.515 millimeter, and the other is an angle, and that's to the horizontal line. You can see there. First of all, let's apply a dimension. So let's apply a dimension of 15 millimeters to the linear, and then we're going to hit tab on the keyboard, and then we'll come over to the angle. So on the angle, let's select 30 degrees. Then if we press Enter, we can now see that we have this straight line with a 15 millimeters in length and a 30 degree angle to this horizontal line here. Now we can continue drawing lines. So if we keep left clicking, we can draw as many lines as we like. If we want to exit the tool, we can right click and select. Okay. I'm going to select these lines here that we don't need, and then I'm going to hit Delete on the keyboard. We can remove those. If we want to move these dimensions around, we can hold down the left mouse button, we can move those so we can see them maybe a bit more clearly. And if we want to edit these, it's very simple, double left click, and then we can input the dimension we like. Let's go 18 millimeters there. Let's change this angle to, let's say, 45 plus enter we can make the modifications like so. So that's the basics of the generic line tool. So if you want to move if you want to pan around the axis, there are two ways to do this. We can select the pan just on the left hand side there, then we can left click and move around, or we can hold down the middle mouse button, and we can do exactly the same. So I'm just going to pan over here slightly, and then I'm going to select the midpoint line. Select that. And then if I click anywhere in the canvas, let's just say here, you'll see, I've started at the midpoint, and now as I move the mouse, I can create the length of that. And again, I can input an option here for the length. In this case, let's just about 20 millimeters, press Okay. Then I'll right click and select Okay to leave that. So that's a quick introduction to the line and the midpoint line tool. These are used very commonly throughout sketching, so they're kind of fundamental, but they are very simple to use. I'll see you in the next lecture. 11. Circle Tools: And let's move on to the circle tools. So if we select the drop down, we've got the centerpoint circle, which is the most commonly used. Then got the tangent circle and also the ellipse. So ellipse is more used for complex geometries. Start by taking a look at the centerpoint circle. So first, I'm going to hold down the middle mouse button and just pan over to some empty canvas. I'm going to left click anywhere in the canvas, and you'll see we're beginning to draw a circle, and we can adjust the diameter by moving the mouse. Center a dimension there of 20 millimeters I'll select okay, there we have our 20 mill diameter circle. Now, we're still in the circle tool. You can see it's selected. So if we left click here, we can draw more circles as many as we need. We want to leave the tool. Again, we right click Select Okay. Remove these three circles. We can just press Control Z on the keyboard, remove these three like so. If we want to adjust this dimension, just like the line tool, we can double click. Let's go for 18 millimeters, reduce that slightly. Now we have an 18 mill diameter circle. I'm going to pan across again. I'm going to show you this time, the tangent circle. So to do this, I want to have three lines. So I'm going to select the line tool, draw in one line, right click. Okay. Raw in another line, and one more. Let's go for this one. Now let's go on the tangent circle. So we have these three lines. We're going to select one, two, and three. And you'll see that inventor will recognize the positioning of these three lines and draw a circle according to what makes it tangential to those three lines. There's more used for more complex drawings. The right click Okay, to leave that. And we're going to pan across to some empty canvas here. And now we're going to use the ellipse tool. Okay? So if we come across anywhere on the canvas, first of all, we start with the center. I'm going to select the center being here, and then we're drawing out an axis point. So in this case, I'm going to left click here. Okay? And then I can draw my ellipse like so. It's more commonly used when there are lines and other positioning tools in place to ensure that we get an accurate positioning and dimension of an ellipse that's needed. Okay, so those are the three circle tools that I've just showed you there, centerpoint circle, tangent, and ellipse. But again, the most common one we'll ever need is the centerpoint circle. 12. Arc Tools: So far, we've taken a look at the basic line tools and also the basic circle tools. Now let's move on to the arcs. So we've got three options here, the three point arc, which is the most common that I use, tangent arc and center point arc. Now, all three of these have their own uses. Let's take a look at the three point arc to begin with. I'm going to be using my sketches, I've already drawn here to support me in demonstrating these. So the first point we must define is the start of the arc. So I'm going to snap to the end of this line here, and then I need to define the end of the arc, in which case, it is here. And then you can see I've got an option to control the radius of the arc. I can control that by entering a number, or I can just left click and place in the arc like so. That's the basic principles behind the three point arc. A tangent arc is basically an arc that becomes tangent to point to which you define. So a start point, let's say this one here. Now, wherever I draw this arc, we can see it is tangential to this point here. I I drop that here, right click. Okay, we can see that joining point there is tangential. So those are the principles behind the tangential arc. And then moving across, let's take a look at the center point arc. Very straightforward to use. First of all, we need to define the center. So if we select the center at this junction here, and then we come out and we can select the starting point of the arc, let's say here. And then wherever we move the mouse to, we can see the arc forming. If you want to end the arc here or here, so let's go over here. And so those are the principles of the three arc tools. Again, most common is a three point arc very straightforward to use. Okay, let's jump into the next lecture where we'll take a look at the rectangle tools, the slots, and polygons. 13. Rectangles, Slots & Polygons: In this lecture, we'll cover the key rectangle tools, the slot tools, and also the polygon tool. So first of all, let's take a look at the rectangle tools. We've got four to select from. The most common two that I use are the two point rectangle and the two point center rectangle. We'll run through all four just so that you understand the principles behind each one. Let's start with the two point rectangle. A straightforward. One click starts at one corner, and another click will start at another corner. So it's typically at this point that I actually enter dimensions. So let's say 15 by ten and press Enter, and there we have our two point rectangle very straightforward. Next, we have the three point rectangle. So a little bit more advanced here, so we select our first point, and then we have the option to input an angle. Let me put in a dimension there. So we'll do a linear dimension of 20, press tab on the keyboard. We'll do an angle of, let's say, 15 degrees, press Enter, and then we need to do one more click, which is the third corner. So we need to define where that is. This, I'll put in a dimension of let's say 8 millimeters, and there we have all of the dimensions there, and we can control this angle. So if we double click, we can change that to let's say 25, change that width, 15, and change the height, a six, like so. So a bit more capability and offerings in this tool compared to the two point rectangle. Moving on, let's take a look at the two point center rectangle. Again, I use this quite commonly, the very first click is the very center of the rectangle. And then when we drag out the mouse, we can then see that the rectangle shape forms, and we can input dimensions there. So typically, here, I'd add my dimensions. Let's say, 25 and ten press Enter. So yeah, very straightforward tool. Next up, we have the three point center rectangle, which is a bit more advanced on top of the two point center rectangle. So we click, and that is our center point of the rectangle. And then we need to provide some dimensions here. So I'm going to input 20 to an angle 15 degrees press Enter. And then, as you can expect here, we can then define the height. In this case, I'll enter six, and we can adjust all these dimensions accordingly, like so. So those are the four rectangle tools there. Two point rectangle, three point rectangle, two point center, and the three point center. Next, let's move on to the slot tools. The very first slot tool we have is center to center. Very straightforward. It's like the bread and butter of slot tools. The first point defines one center, and then the second point defines another center. So I'll just put in a dimension there of 20, and then we need to define the diameter of the arc. So in this case, I'm just going to put 8 millimeters. There we have our slot, all the according dimensions to which we can then adjust as necessary. For example, I make that six, the 20. Let's bring that down to 16. So descender slot very straightforward. Now we've got the overall slot. So this is slightly different. I'm going to do here to demonstrate this is to snap to this line here, then drag that across and snap to this line here. And then I'm going to input my diameter. Let's go to six mil again. And so what we can see here is I've come from I've done an overall slot. So I've come from the outer quadrant of this arc to the outer quadrant of this arc as opposed to a center of this arc to a center of this arc. A very similar principle. Output is slightly different based on where you're starting. Next tool we've got is the slot, which is a center point. All right. So here, instead of starting, we're not starting at the center of an arc. We're not starting at the outer quadrant, but instead we're starting at the very center. So to demonstrate this, we'll do our first click where the center should be, and then we'll come out to where the center point of the arc is. And then let's add in a diameter there of six milo, so we've achieved the same result there by using a different tool. The next slot is a three point arc. I'm going to come over here for this. So first of all, we need to define the center of the arc. Okay, so one click there, and then the end of the arc. To some dimensions here, so I go for 12. I'll press tab on the keyboard and put it in an angle of ten degrees. Okay. Now I need to define my arc. So I'm going to give that a radius, say 10 millimeters. Okay? So we've got our arc, and now when we move the mouse, we can see the slot forming about that. I need to put in a diameter there. So, in which case, I'll put in 5 millimeters, and we've got all those dimensions there. Tidy that up a little bit. There we go. And then next, we've got the center point arc slot. So very similar principle, but instead here we start at the center of the arc, okay? So I'm going to draw that out like so, right? Then put in my arc. I can put in an angle there, let's say 45 degrees, and then I can draw my slot based around that arc there, a four mill. And again, just like the other tools we've been playing with, you can adjust these dimensions as you need. For example, I'll change that too, let's say 60. Okay, I could change that to say three. And last but certainly not least, we have the polygon tool. So let's go into our drop down and select polygon, and then we have this toolbox pop up here. I just pan across a little bit. So we have an option for inscribed and circumscribed. So I always go for inscribed and then make my dimensions from there. Here we select the number of sides. So we go for six side. So in this case, a hex. And to begin with, we just select the center of the polygon, and then as you move your mouse, you'll see the hex to pop out from that, okay? So we can just put that in there, a right click. Okay. Let's select that tool one more time. In this case, let's put in a 12 sided polygon. Alright. And then we can see our polygon so and click Done. And then from here, as I said, I normally put in dimensions. So I haven't covered this yet, but I will cover this in a later lecture. Here we have the dimension tool, which comes under the constrained tab. Okay? So if we select dimension, we can do a dimension from the flats of this hex. Okay? So let's say that's eight mil. Let's say from this flat this flat here of the 12 sided polygon. Let's put that as 12 mil. Right click. Okay, that's our polygon tool. Okay, so that covers it for the polygons. We've done the slots here. We've also taken a look at the four variants of the rectangle tool. I hope that all makes sense, and we'll be using these tools in the exercises to come up at the end of this chapter. So I will see you in the next lecture. 14. Fillets & Chamfers: In this lecture, we will study the fillet and the hamper tool in sketch mode. So I'm going to come up and I'm going to select a rectangle. This time, I'm going to select a two point rectangle, start at the origin, bring that out. I'll enter some dimensions in. So we'll do a width of 15 millimeters, press tab on the keyboard. We'll do a total height, let's say, 10 millimeters, press Enter. Right click. Okay. Center that. We can use the middle mouse button to zoom in and out. Now if we come up to the fillet tool, we'll select that, and then we need to input the fillet dimension. So in this case, let's go with 4 millimeters. We need to select two entities to which a fillet will be formed. So the first entity is this line here, and the second entity is this line here. Now, as soon as we hover over that, we can see a preview of the arc form, the same with this entity here. So that arc is forming there. Going to select this line here. Okay, that's good. Then going to exit out of the fillet tool. I like so. And there we have our four mill fillet. So, likewise, let's do that for the other corner. Let's put a fillet on there 1 millimeter, select the first entity and the second, exit the fillet tool, and there we have our one mil fillet. A very similar tool to use, very effective. There is also an option to fill it in three D mode as well, which we will cover in the next section on three D modeling. But it's really down to preference whether you do this in sketch. I typically do it in three D modeling mode. But again, this is something that we can always do in sketch mode as well. And the next to I want to show you is the hamper. So if we click on the drop down, we've got the ShampaTol here. Let's select that. Then we've got our options here. So here we've got different options. We can do an equal hamper. So let's say we do a two mill hamper. I'll select this entity and this one here, we can see move those dimensions. You can see we've got our two mill dimension here and a two mill dimension here. Now, if we look at this dimension, there is a function at the beginning, so FX colon two, it's relating to something, and it's relating to dimension seven, which is this one here. If we double click on that, it's called D seven. And so if we change this, let's say, let's change it to 3 millimeters, we'll see that this dimension will change already because that relationship is there between these two dimensions. And that's because it's an equal ShamFa. Now if we select the two D ShampaTol and then we click this option here, we've then got options to put in different distances. So let's say the first distance, it's 1 millimeter and the second, let's go with three, make that visually quite different. So select our first entity and the second. It's okay. And then those dimensions will pop in here, right? So we've got our three mill on the vertical, and then we've got our one mill on the horizontal. And for the last champa option, I'm just going to pan over here, draw in another rectangle do the same dimensions. Select the ShamfTol again, and then we're going to select the third option here. So let's say a distance of, let's say, 4 millimeters, and let's put an angle of 20 mil. So here we're not actually defining what the distance will be, but instead, we're defining angle. So let's select first entity and the second entity. It's okay. Then we've got our distance here, so four mil on the vertical, and then inventor has input the angle for us, so 20 millimeters. And again, we can change this, let's say, 45, okay? So that would be an equal champ so four to four. Let's go with, let's go with 15. Okay, so these are different options there for hampers that we can use as we begin to progress with our sketching capabilities. That's it for the Fillet and the hamper tool quite straightforward. And I will see you in the next lecture. 15. Text Tools: In this lecture, we'll be learning how to use the text tool. So I've got two examples here of where I have used text. Down here, I've used text to emboss some lettering onto a surface. Now, it can be used to emboss lettering or numbers, let's say, a part number or a model or a brand. So here I've got inventor. Okay. And then at the top, I've used letters to engrave into a surface. So here we can see I actually engraved into that surface. And then if we move down, we can see I've embossed onto that surface there. So in this lecture, we'll just be learning how to use the text tool, how to modify the text, and how to make it conform to geometries prior to three D modeling, which we will be covering in the three D modeling section. So I'm going to start a new part. We'll come up to the top left, select new. I choose a standard millimeters template again, create come on to start a two D sketch. In this case, I'll select the XY plane. And then very simply, I'm just going to hit the text option here. That's a shortcut T on the keyboard. Left click the mouse, then we can enter our text here. Enter inventor for now. And then we have a myriad of options that we can play with to customize our text. These are very standard options that you would get, for example, in office software. But this here, I'm going to stay with this font and choose 6 millimeters. And then if you want to re edit that text, we can just double click on it. You can also add bullet points, numbers, justification to left center or right positioning up, middle or bottom. Yeah, make it bold, change the color, and so forth. Feel free to have a play around with these. If at any point you do want to enter any symbols in here, that's an option that we do have as well. So I typically do this in drawings. But if we do ever want to do it when sketching or modeling, we can just select the drop down here, and then we have, let's say, the tolerance symbol plus or minus degrees diameter and so forth there. Okay, so let's say with inventor, okay? And there is one more text tool which I like to show you. So this is if we go on the drop down, it's called geometry text. Now this is where we conform text to a geometry. I'm going to give an example here. Let's choose the line tool, and I'm just going to draw a line anywhere. Let's give that a length of Let's go for 50, and let's just say 25 move that dimension out the way. And then we'll come into the dropdown, and we'll select geometry text. Now, from here, all we need to do is to select a entity. So in that case, is this line here, or left click Enter my text. Press ok. And now we can see that the text is now sitting on this line. If we want to move this text, though, we cannot just hold down the left mouse button and drag it. But what we can do is double click, select it, and then we can center justify it. Press Okay. And now it's sitting in the center of the line. And likewise, if you want to write justify it, we can do so. We can also change the direction of the text, as well. Se press Okay. We can now see that change direction. It's like it's inverted. And this is very useful if we're doing plastic injection molded parts. Double click on that again, put that direction back to how it was. We can also change the offset distance. So if we want to offset this from this entity here, let's say we do that let's say 2 millimeters plus enter, we can now see that it sits off of this line, so it's offset by a total of 2 millimeters. We can also make various changes to the text itself by clicking the launch text editor, and there we have the same options that we had when we've just done normal text. So we can make any changes or formats there, select Okay. And there we go. That's how we conform text to a particular geometry. So that's a summary of the text tool, nice and easy to use, and we'll be using this later when we come on to the three D modeling section. I'll see you in the next lecture. 16. Modify Tools: In this lecture, we will take a look at the modify sketch tools. So I'm going to start a new part. I'm going to select the standard millimeters template, but create now let's start two D sketch. An of our three default planes, let's go with the XY plane. So the modified tools are just up here. There are nine key tools. Let's take a look at these today. So first of all, I'm going to draw some geometry. I'll start with a centerpoint circle. And I'm just going to start anywhere in the environment, let's say here, and I'll draw that out, and I'll enter. Let's go with 10 millimeters. That's diameter. Let's enter. Now we have this ten mil circle. Let's first of all, take a look at the move tool. There are different ways in which we can move this circle. We can use the move tool, and there's a shortcut that I show you afterwards. So if we want to move this, first of all, we need to select the geometry to move. I'm just going to left click drag around the circle, let go of that, and then we need to select the base point. So the base point is from where we move the circle to where it's going to go. So, for example, if I select the center point of the circle, and you can now see that where I left click will be the final destination of that circle according to that base point. So in this case, I'm just going to move this to the origin, which is the yellow.in the center there. So that's 000 on the X Y and Z axis. I'll left click once, and there we've moved the circle. We have a few more options here to copy. Okay? So I select this, select my circle, use the same basepoint again. Then if I left click here, you'll see that it's just copied the circle. I've moved it, and I've copied it also. We can also use precision input, right? So if I select this circle here, I go base point, I select the center point. I like precise input. I can then input a precision point. So for example, if I want to go across, let's say we go across on the X axis by ten mil, tap on the keyboard, on the Y axis, let's say we go minus ten. We can then see that precise point there. Another way in which we can move a sketch, which is easier, in my opinion, is just to hold down the left mouse button. Let's say on the center point of this circle here and let go, and I can just move it like so. But if we do want precision or anything like that, we'll need to use the move tool. Next, let's take a look at the copy tool. So quite simply, we're just going to copy. In this case, let's go with this circle here or select the base point. Let's again go with the center point of the circle, and I can left click as many times as I want. We can have as many of those circles as we need. We could also have the option here to clipboard, so Control C. If I select this and click Done, if I put my mouse in this position here and press Control V, you'll then see that I can input a circle, and likewise it's here, likewise it's here, and we can go on indefinitely. We've also got the option here as well for precision input, so we can use the coordinate system to accurately input circles where we need them to be. If we want to remove any of these circles, we can left click on them and press delete or alternatively, we can just press Control Z on the keyboard, which is just undo. We can undo all of these copying of the circles or moving them around. Next, we've got the rotate tool. So for this, I'm not going to use a circle. We use a different geometry there. Let's go with a two point rectangle. I draw in a rectangle. I put in some dimensions. Let's go with 20 and ten. And if we select the Rotate tool, we need to select the sketch to rotate or the sketch pieces. Now we can select these lines individually, so we can left click on each one of the lines we just highlighted. Or just like before, I'm going to hold down the left mouse button drag across the entire rectangle and let go of that. And now highlighted in blue. We can see we've got the entire rectangle selected. We need to define a center point, so this is a rotation point to which this rectangle will turn around. Let's go for this corner point here. And you might have a dialogue box pop up, okay? In this case, we want to click, though, this is just saying that these horizontal lines are constrained horizontally, okay, so they're not able to rotate. And also the vertical lines will be constrained vertically. But in this case, we can just remove the constraints. There's no issues here. So yeah, around that base point we've selected, we can then rotate this. And what we can do in this box here highlighted in blue is to input an angle. I I rotate this by, let's go for 335 degrees, you press Enter, and then we've changed that 335 degree angle. We've also got the option there for copy as well, and also precision input. In terms of the trim tool, let me draw some lines to showcase this. I'm going to draw a straight line across the line tool again and do a vertical line. Now, where these two lines intersect, if we no longer want to have this material here or this material, what we can do is to click trim, and then we can hover the mouse over the line, and inventor will recognize the point of intersection and then enable us to trim away this line here. So if we left click, that gets removed. Other way to do this, as well, especially if we are trimming away quite multiple lines or quite a few lines, we can hold down the left mouse button, and then we'll start to see this blue line form like so, and anything that intersects with that blue line will be trimmed. So if I come down here, see immediately that extra line that we didn't need has now been trimmed away. We've then got the extental again, very straightforward. To showcase this, let me draw in another vertical line. Go for this one. Now, if we wanted for this line to extend to this line, we just select the extental and then if we hover the mouse over it, we'll see that extension preview pop in place. And if we left click, that line is now there. To another example. Let's put a line in here. Want to extend this to this line, so we just extend Left click once. There we go. We've extended those two lines. Now the next tool is split, so it's quite an interesting tool. So if we draw a circle, I'm just going to give that a diameter, let's say 15 mil, say we draw a straight line across that circle. Now, if we wanted to remove this material here, we could trim it. But if we wanted to split this circle so that it's split into two arcs that are distinguished by where this line intersects the circle, we can choose the split command. And then if we select the circle here, inventor will recognize the intersection points and we'll split it accordingly. So now if I go ahead and let's say, I copy I want to copy this whole circle, if I select this arc here, I can only copy the arc. Here, let's move that from the center point. And then as we can see here, I've actually split the geometry. So the whole circle has now been split into two arcs. And likewise, I could do the same for the other arc, as well. Okay, like is the split command. Next, we have the scale command, so very straightforward to use. We're just scaling. For this, let's go back to one of our ten mill circles. So we need to select the geometry, I'll select the circle, the base point from which we're scaling from. So in this case, the center point of the circle. Okay? Just click yes here. And then we can scale this. So we can scale it if we want it three times the size, so this should be 30 mill enter three, press Enter, and now we've scaled that by three times. So the diameter is now 30 mill. Likewise, we can shrink Okay, let's shrink that by, let's do not 0.5. Okay? And then we're down. We've scaled it by half, and now we're down to 15. For the stretch command, I rarely use this one, but it can be useful in some cases. We demonstrate I put in just put in a rectangle like so. And then if we select the stretch command, we can choose here entities to sketch. So, for example, if I choose these two and then select the base point, let's say, the corner here, just press yes to remove any constraints. I can then stretch these two entities. Okay? So if I left click once again, we now stretch those according to the new position. In the last modified tool, and I use this one a lot, in fact, in the upcoming lectures throughout this course, the most tools that I use within Modify are offset, trim, and extend. These are the three tools that I commonly use and would recommend for anyone learning inventor to master these first. The offset tool, absolutely fantastic and very simple to use. We just need to select an entity, in this case, I'll set the circle, and then we're just going to offset it by a certain distance. So, for example, if I put in, let's say this were to be a pipe, I want to put in some wall thickness. Okay, let's say, let's go with 1 millimeter offset. Okay, we can now see we've got this dimension pop up there of one mil. And we can always change that by double clicking on it. Change that to two. Now we've got a two mill wall thickness there. So we just use that by offsetting. We can also offset on the outside as well, just by dragging the circle out. So offset that by two. Okay, we then got that dimension pop up there. And again, double left click. We can change that to one, something like that. So that's a quick overview of the modified tools. Again, I will be using these in future lectures, so we'll have more of an opportunity to experiment with these. I hope that helps, and I'll see you in the next lecture. 17. Sketch Pattern Tools: In this lecture, we will learn how to use these sketch pattern tools. So rectangular pattern, circular pattern, and mirror. So let's go on New, start a part file, go to go with standard millimeters. Click Create. Go to start a two D sketch. And for this, let's go with the XY plane. But the pan tools are located just up here. A, rectangular, circular and mirror. Let's go for a rectangular pattern. So to demonstrate this, I'm going to start by drawing in a two point rectangle. I start at the origin, to bring that across, and I'm going to enter a dimension here of 150. Then going to hit tab on the keyboard. I can enter my height. In this case, I'm going to put 20. Double click middle mouse button. Hey, bring that to the center. Then from here, I'm going to add a circle, and I'll begin to pattern this. I'll click the circle tool, I'm going to click anywhere inside my rectangle, add my circle. Going to give that a diameter of 5 millimeters. And I'm going to dimension that. So let's position the circle from this horizontal line. Let's go for five mil. And again, the circle from the vertical line. Let's also go for five mil. Okay? So that's fully constrained, as we can see in the bottom right corner. That's great. Now let's go ahead and rectangular pattern this circle over our rectangle. So when we have the toolbox pop up here, we need to define the geometry which we wish to pattern. But in this case, I'm just going to drag across my circle, let go of that. That's highlighted in blue. And then I need to define my direction, which I want the pattern to be in. Now, in this case, we need to select an entity. So I'm going to select this line here so that we mirror in this direction. Okay, so if I select that line there, we'll then see a green arrowhead pointing in the other direction, and we see there's been a pattern circle in the wrong direction. No issues there at all, because under direction, we can just flip that, and now we're going in the correct direction. Okay. In terms of the number of circles I'm going to pattern, I'm going to go for 15, and I'm going to spread these by distance. We could do any distance you like here. I'm going to go for ten mil. Okay? And as per the dimensions of this rectangle, that should bring us nicely to the end. We've got the same distance over here of five mill and over here of five mil as well. Now, notice here that we can also add a second direction. So we've only patterned in one direction, okay? So down the X axis. That's also pattern down the Y axis as well. I'm going to select direction two. Now, in this case, I'm going to select this entity here, and we'll see the green arrowhead. Is luckily in the right direction this time, but if not, we could just flip that. A number of instances, in this case, I'm just going to select two. Okay If we select more than that, we'll see we're going beyond the rectangle, so I only need to have a pattern of two here. Okay. I'm also going to choose the same distance there. So 10 millimeters between the two center points of the circle. I click Okay there, we see the pattern complete, and that's looking nice. Now, if you want to edit your pattern, you can do that at any point. You can come across to any one of these circles. Let's choose this one. And right click, and then we have some immediate options here. One of those is Edit pattern. So if we choose that, we can make any according changes here. So we could go for, let's say, if we want to increase that to five or likewise, we could change the distance here to, let's say 20. And then we've got this very large gap of 20 between all of them. Okay, we keep the on ten. That's okay. That's how we edit a rectangular pattern. Another useful tool as well as to suppress. It's not commonly used, but on an occasion where you do need to use it, we can suppress any circles like this. For example, if I suppress these three and then I finish the sketch, you'll see that those three circles have now been suppressed and they're no longer a part of our sketch. That come back into the sketch, I'll come to the design tree and right click edit the sketch. Just going to right click on this one again suppress, do that for all three. If you want to delete the pattern, we can also again, right click on any one, including the original one, and we can just click Delete pattern there, and then we're back to the original. So that's a quick overview of the rectangular tool. It's very useful and very simple to use. Just select the geometry that we want to pattern, and then we select an entity giving it the direction, and then we input our distances and how many entities to pattern. But the circular paternt tool, very similar and again, another very easy tool to use. Let's go with another circle. Let's go for a circle of ten mil diameter. Bring that up there. Now, to use a circular pattern tool, we need to have an axis to pattern this around. So for this, I'm just going to enter a point. I'm going to enter a point down here, so in line with the center point here. I'm going to dimension that, give that a bit of accuracy. Let's got a 20 mil looking good. Select our circular pattern tool, and just the same thing here. We need to select our geometry by drag across the circle. And then in terms of the axis, and they're going to select the point that we put in here. And then we've got some parameters we need to control here. So how many of these circles we want there to be, we can increase that to ten. We can just go for four. In this case, let's go for six. Then we can also choose how much of an angle to pattern these around. So what degrees around the point or our axis? Will we pattern these? If we go for 180 degrees, for example, we're only patterning around 180 degrees and six instances. We can also flip the direction. We've got the flip option there as well. That looks pretty good to me. I'm going to leave that there for now. Again, if we want to edit this, we can right click Edit pattern, make any according changes, and also just like the rectangular pattern tool, we can right click and we can suppress any one of these circles. I I suppress these two for now. And now, the last pattern tool is mirror. Now, I use this a lot when I'm sketching, really, really useful. Now, for the mirror tool, we need to have a mirror line. And I'm going to mirror these circles here. So I'm going to add in a line, go to draw that anywhere for the time being, right click on that line. I make it a construction line. It's not absolutely necessary that you make it a construction line, but I like to do so just so that I know it's not part of any profile, and it's just used for constructing a sketch. I'm going to make that a bit more accurate by dimensioning from the centerpoint of this circle to our mirror line here. Let's go for 15 mil. Okay, right click Okay. Leave the dimension tool. Now let's jump into the mirror tool. So under the mirror tool, we need to select our entities to mirror, I'm going to drag across all of these, select them. I'm going to click the mirror line, then select our construction line here. And I'm going to click Apply and done, and that's looking good. So we can see there we pattern across our circles and also the two that we suppressed. And when we click Finish Sketch, we'll look at that, we can then see that the circles we suppressed have not been mirrored, as well. Okay, and that's the mirror tool. So I will be using the mirror tool quite a lot in the upcoming lectures. It's a brilliant tool, really useful. So that is an overview of the three pan tools that we have in sketch. Okay? So that's the rectangular pattern like we did down here, circular pattern like we did here, and then the mirror, which is like we did just here. Okay, I hope that all makes sense. Any questions? Please send them to me, but aside from that, I will see you in the next lecture. 18. Dimensions & Constraints: In this lecture, we will learn about dimensions and constraints. So let's start a new part, come under the part templates, select standard millimeters, create. Then we're going to start a two D sketch. For this, let's go for the XY plane. And now that we are under this sketch tab, we've got all our sketch tools, modification tools, got our pattern tools there. And here we have constraints. Constraints are regularly used when we're sketching. I think I use them in every sketch that I do. So let's take a look at these. First of all, we have dimension, very straightforward to use, and you would have seen me use that in quite a few previous lectures. We've then got three options here, so automatic dimensions and constraints, show constraints. Constraints settings, and then we have the key constraints themselves. So we've got the coincident, parallel, tangent, collinear, perpendicular, smooth, concentric, horizontal, symmetric, fix, vertical, and ecor. Now, that does sound like a lot, but every one of these is very straightforward to use. I'm going to demonstrate them now. So let me start with a line tool. I'm going to start, in this case, from the origin, and I'm just going to draw a straight line at an angle like so. First dimension tool, sure you've seen me use this before. Just select the line itself, and then we can come up and give that a horizontal dimension. Or if we come over to the left or to the right, we can give it a height dimension. But what if we want to give that line a fixed length? Because we're only given an option here for vertical. That's vertical and horizontal. What we do is we bring the mouse close to the line and left click once, and then we can see we can give it a fixed length. If I left click again, let's give that a dimension of 20 mil. Okay, we can do so like that. If I draw another line in, let's go for a horizontal line. I want to give an angle between these two. Again, I'm going to use the dimension tool. I'm going to select this line and this line, and then I'm going to input my angle here. So let's go let's go 45 degrees. We can move this dimension around just by holding down the left mouse button, so we can bring that in or out and we can move the dimension where we so that's the dimension tool, very straightforward to use, and I'm sure you'll be using that a lot throughout the remainder of this course. Let's move on now to the constraints themselves, so I'll demonstrate these one by one. First of all, let's take a look at the coincident constraint. Demonstrate this, I'm going to draw two lines If we want to have the endpoint of this vertical line and the endpoint of this horizontal line to be in contact with one another, this is when we would use the coincident constraint. If I select this, I then select the endpoint of this line and the endpoint of this line, we can see now they are constrained together, and wherever I move these entities, you'll see that that constraint will remain. And we can see that constraint by left clicking just on the corner there, and then we see we've got the coincident constraint applying to the vertical line and then this coincident constraint applying to the horizontal line. We can remove these. So if we left click once and then right click, we can delete that constraint, and then we can separate those lines and you'll see, they're no longer constrained. I'm going to put that back in for now. Another example I'll show you if I add a circle, let's give that five mil radius. I'm going to use the coincident constraint here from the center point of the circle to this line here. Now, if we move this circle, if we try to move it, you'll see that it's constantly keeping that relationship, that relationship is maintained between the center point of the circle and this line here. If you want to fix this in place, can put the coincident constraint between the center point of the circle and let's say the endpoint of this line here and you'll see that relationship there is maintained. That's a very commonly used constraint. You'll see in the following lectures, and you'll have plenty of examples where you'll be experimenting with these constraints, and the coincident constraint is one that I'll be using quite regularly. Next, we have the parallel constraint. To demonstrate this, I just draw in two lines, any particular angle, so we can see here that these lines are not parallel. And to change that, select the parallel constraint, and quite simply, we just select the two lines. They are now parallel, and we can see visually the constraint that has appeared. If we left click this line, we can see that constraint there. And again, if we right click Select Delete, I can then change the angle, and they are no longer parallel. If I put that constraint back in, and then I try to rotate one of these lines, go for this and I'll select the rotation point, let's say, the endpoint of this line. I'll then have a warning pop up from inventor, so telling me that there is a constraint already applied that restricts me from rotating this line. So if you want to remove that constraint, reflect, or otherwise, we can just leave it as it is. Next, we have the tangent constraint. This is another very commonly used constraint. Let's take a look at this. It's going to use this circle as an example. I draw in a line, say like so. If I want this line to be tangential, so roughly in this position here with the circle, very simply, select the constraint, circle line, there we see we've got that constraint. And if we left click on the circle, we can see that constraint right there. And likewise, if we select the line as well. Okay? So that's a really useful tool. That relationship will always be in place. Next, we have the colinear constraint. I'm going to move these guys out the way. I'm going to draw in another line. In this case, let's draw it here. Give that a dimension, ten mil. Now if we select the colinear constraint, we can make this line here colinear, in this case, with this line here. I'm going to select this line and select this line, and you'll see that relationship has been formed. And where I move this line, you'll see it will maintain that colinear relationship between these two lines. Okay? So that's this one here. So again, we can right click and delete that, then this line is free to move and no longer colinear constraint. Next, we have the perpendicular constraint to demonstrate this drawing a line at an angle like so. If we want this line here to be perpendicular to this horizontal line, this is when we'll use the perpendicular constraint. We'll constrain this line to this line, and you'll see that relationship has now been formed. So we've got this constant 90 degree angle here. We can then add to that by using the coincident constraint, can select the endpoint of this line and this line here. Now I see they are in contact. They're constrained coincidentally. And also on this slide here, we see a perpendicular constraint with this horizontal line. Next, we have the smooth constraint. This is only really used for advanced sketching when we're using spins. Since we won't be covering that material in this course, we won't be covering this constraint. We will be covering the concentric constraint. Again, you'll see me using this throughout following lectures. So if I select a circle, let's go for five mil. I'll select another circle, go for ten mil. Right click. Okay. I'm going to use the concentric constraint between these two circles. I'll select one, select another. And now we can see that relationship is formed where both of them have a concentric midpoint. If I try and move this now, regardless of where I move it, those two circles will always remain intact with that relationship. Next, we have the horizontal constraint. Let's choose this slide here actually. If we select the horizontal constraint, it's very straightforward. Makes an entity horizontal. But this line here is currently at an angle. If you want it horizontal along the X axis, just left click on it once, and you'll see it's now horizontal, and we'll see the constraint pop up there. We've got the tangent constraint to the circle. It's looking nice and this line is horizontally constrained as well. We are unable to change the angle of this. We can only move it up and down. We have the symmetric constraint. Draw some more geometry for this. Let's go for a symmetry line. So I'll give that a dimension, let's say ten, then come off of that with an angle, let's say another ten, and I draw one more line in. Let's go for an angle like this of ten. So we've got these two lines here, which have different angles coming from our symmetric line. What we can do here, symmetric constraint. Now, first of all, we're going to select the two lines, one line, and then the other line, and then we select the symmetry line, which in this case, is this one. Now what we see is the angle between this line and our sentry line is the equivalent, as is this angle from this line to this one. Let me just put in some dimensions to show that, let's say, 30 degrees. And then we can see that is 30 degrees as well. So if I then change this dimension, let's say I go for 45, we'll see both lines will now be at an angle of 45 from our symmetric line. You'll see here the dimension is in brackets. You might be questioning that. That's because it's a reference dimension only, so we cannot control the angle that's controlled by this dimension here and the symmetry constraint. This is just here for reference. So let's change that to 30. Okay? Now both of them are showing 30 degrees. Next, we have the fixed constraint or the lock constrain, as I call it. If we select the join of these entities here, we are free to move this around. So it's not fixed, not fully constrained. What we can do is use the fixed constraint and then select that point there. We'll see that padlock appear. Okay? And now we'll see that we cannot move any one of these. But this entire sketch is now fully constrained. All lines have a linear dimension. They have an angle, and they have a fixed point here. So nothing here is able to move. Next, we have the vertical constraint, very simple. Now, the vertical constraint and the horizontal constraint, I'll be using these a lot throughout the upcoming lectures. You have plenty of experience to work with them. So you'll have plenty of opportunity to get hands on with them. For this, I draw a line, and I draw that line. That's like so exactly the same process as the horizontal constraint. We just select our vertical constraint, then select our entity, and then immediately, we can see that constraint there and that that line is now constrained vertically. We can change its length. We can move it around, but we cannot change the angle. And next, we have the equal constraint. Let me draw in another line here. I want to dimension the first line. Let's go to eight mil. If I apply an equal constraint to these two lines, it will mean that this line here will become eight mill in length. Let's select this line, then this line. Now this line here is eight mill in length, but in the dimension, and we can see 8 millimeters there. And if I change this, let's say for 15, we'll see that this line changes to 15 mil as well. So that traol is then constraining them so that they are equal let's use a few more constraints and tidy these two up. Let's go for a horizontal constraint between the endpoint of this line and the endpoint of this line. So they are now horizontally constrained, and we can see that they are coming to the same position on the endpoints. Then use the dimension tool, tidy that up. Let's put in ten more. Example, I'm going to draw in a circle going to be ten mil circle, and I'm going to use the tangent constraint here between this circle and this line, and then we'll see there's this tangent constraint with this line here. So that perfectly fits inside our two lines here. We can also use the horizontal constraint, for example, from the midpoint of the circle to the midpoint at this line here. And now that circle is now constrained. And for the most part, it's fully constrained. There's just that bit of movement still available there, which we can change by adding in a fixed constrain, say, this point here, okay? And now these entities here are fully constrained. There are three more tools I'd like to show you, so automatic dimensions and constraints. Simple to demonstrate. If I draw, I'm just going to freehand drawing a triangle. And then if I use the automatic dimensions and constraints, I can choose to apply dimensions and constraints. In this case, just for an example, I choose dimensions. Then if I select my geometry, hold down the left mouse button, drag across, then I click Apply. Then see that this angle has been put in place and also a distance has been put in place, as well. That's then fully constraining this triangle here. That's quite rough by a free end. We could tidy that up. Let's go for 60. Another tool is the show constraints. But if we select this, we can then select any entity, and it will show us if there are any constraints available. So for example, if I choose this horizontal line, we'll see a constrain arise here, which is the horizontal constraint. So we know this line is fixed horizontally. Likewise, for the vertical, we see a vertical constraint there. Let's see what's happening with the circle. We've got that tangential constraint, okay? And with this line here, we've got a vertical constraint, and we've got the equal constraint as well. Again, we can edit these anytime just by left clicking, then right clicking, then press Delete. And now that equal constraint is no longer there and change the dimension of this. Let's go for 12 mill. If we want to hide our constraints, we come down just to the left down here. The shortcut there is F nine on the keyboard, hide all constraints. Like so. And then the last tool here is constrained settings. I'd recommend, at least for this course, to keep these all as the default. Typically, when I'm doing sketching and modeling, I'll leave them as the default, so I'll leave those as they are for now. So I hope that all makes sense. And again, it might be a bit much to cover in one lecture, but in following lectures and all the examples we'll be doing together, we'll be regularly using an array of those tools to get more of that experience and a better understanding of when and how to use them. And I'll see you in the next lecture. 19. Project 1 - Sketching: In the next couple of lectures, we'll be doing a series of exercises to use the skills that we have learned in the previous lectures. So this is the very first exercise. And what I would recommend here is that you have a go at sketching this by yourself. And try to use the following tools, which are the rectangle, circle and slot tool, the Fillet tool, dimension tool, offset tool, constrained tools, and also the mirror tool. So I will now demonstrate this using the listed tools and you see how I would typically draw something like this. I'm going to start a new part going one of standard millimeters, click Create. Then I'm going to go to Start two D sketch, choose a plane. In this case, I can choose any, but I'll choose the XY plane. And I'm going to start, first of all with the outer body of this part. So for this, I'm going to use a rectangle tool, I use the two point rectangle. I'll start at the origin, and I'll left click just to form the body itself. Going to use the dimension tool. Okay, I will dimension the horizontal line first. So that's 80 millimeters in length. That will click the middle mouse button, zoom out a little bit. And then let's dimension the vertical length, which is 40 millimeters. Okay. Go to right click and press Okay to exit. Uh, the dimension tool, and now we're going to add the fillets on the corners. So for this, we'll use the Fillet tool, and we can see as per the drawing that the fillets are five mil. So we'll select our first entity, and the second, repeat the process for all four corners, and there we will have our body with five mill fillets on each of the corners. Up, let's take a look at these mounting holes, the three millimeter diameter ones. All right, so we can see the position of them is five in from the vertical and five in from the horizontal. Now, we know that the fillet is five mil, which must mean that the three millimeter circle is concentric with the center point of this arc. Therefore, what we can do is select the circle tool. Let's just click on one of the arcs center points and then we'll press three on the keyboard. Okay. And then we have our three mill diameter mounting hole. We're going to do the same for the other three, as well. So I'll do the same for this one. And for the other two, I'm going to use the mirror tool. So for this, I need to choose a sketch and then a line, but this will be my mirror line. I'm going to hover above this horizontal line here until we snap onto the center point, which we'll see is a green dot. We'll bring that down to the bottom horizontal line and then come across until we see exactly the same. Sort of center point there is the green dot. Click once, then we'll right click. Okay. And we've got our mirror line. This is for construction purposes only. We don't want this to be a part of any profile. So we're going to right click on this. And we're going to left click on construction, and then we'll see it's a dash line indicating that this is now a construction line, and we can use it for the mirror tool. So let's select the mirror tool. Okay, bring our box down. But first of all, what are we selecting? We're going to select this circle here and also this circle, then we're going to select the mirror line. So then we select our construction line, and then we click Apply. And then we see over here, those two circles have been mirrored, and we've got all four of our three millimeter mounting holes. Moving on, let's do the large two circles. So the 20 mil diameter and the 15 mil diameter. Again, I'll select the circle tool. And I'm going to draw the outer first, which is 20 mil. I place that anywhere inside our body. Right click, rs okay. Now, I want to position this somewhere in the middle here, we're already snapping on. So to do this accurately, I'm going to use the constraint tool. So here I use the horizontal constraint. Like the center point of the circle. Then I'll come across to our vertical line here. If I go down, you'll then see we hit the midpoint of the vertical line. We left click there. Circle is now constrained horizontally with the midpoint of this line here. So it's in the position in this axis. Also, we want to add a dimension there from this circle to this vertical wall. In this case, that's 20 millimeters. Okay? Tidy up these dimensions a little. That's looking good. And then we've got this inner circle, which is 15 mil diameter. So for this, I'm just going to use the offset tool. Very simple. Select my circle there, and I want to offset inside. And so the wall distance there is so it's a five mil difference. So div about that two. Let's do 2.5. Okay? And that should give us a 15 mill diameter circle. Let's just double check that. Yeah, it's coming out at 15. Perfect. Okay, if we look down to the bottom right, you'll see that we're fully constrained. So everything is precisely where it needs to be, and there are no kind of missing dimensions there, nothing's going to move. Though looking good so far, we just need to put in the last feature, which is a slot. And as we can see here, it's dimensioned center to center is 15 millimeters, and it has a radius of three mill on the arc. So let's select the center to center slot. Again, I'm just going to put this in anywhere. We'll come across. We'll put in the center to center distance, which is 15 millimeters plus enter. Draw the mouse out. And then we need to add this three mil radius on the arc, but here we're putting in a diameter. So let's say six milt. Okay, so that's looking good. And again, we've got complete freedom of this. It can move anywhere, which we don't want to do. So let's put another horizontal constrain constrain from the center of the slot, and let's go to the midpoint of this vertical line. It's looking good. And then we just need to add in one more dimension. So click the dimension tool. It's from the center point of this arc to this vertical wall, and that has a dimension of 15 millimeters plus okay. And then that's all the features. We're just going to double check. Everything is fully constrained by looking down here, and again, fully constrained, that's looking good, and that is the exercise complete. I hope you're able to follow along, okay. Any questions, please do post them as a comment, and I will reply as soon as I can. And I will see you in the next exercise. 20. Project 2 - Sketching: In this exercise, we will be sketching this model here. The tools that we'll be using in this case, are the line circle and arc tools, also the polygon tool, the text tool, hamper tool, and of course, we'll be using constraints and dimensions. So just like the other exercises, I would recommend that you pause this lecture here and have a go at doing this yourself, and then following that, feel free to watch the remainder of this lecture and see how I would typically draw something of this. Now, one thing I will say with all these exercises that I'm hosting here, no necessarily right or wrong way to sketch, okay? Just because perhaps the way you sketch this would be different from me, it's not to say that necessarily that's incorrect. At the end of the day, we're trying to get to an end result, which is a fully dimensioned sketch, as we can see here, and there are many different ways in which we can do that. Okay, so if I am to draw this part, I would start with a two D sketch and I would select a plane. Again, we're only drawing a sketch, so two D, so we can select any plane. Let's go with the X Y. I'm going to start with the line tool at the bottom right corner. I'm going to come straight across by 84 mill. And they're going to go vertical by 60 millimeters come out of the line tool. And you'll see in our exercise that we have a Shamp in this corner here. Going to be using the ShamfTol to input that. This Samfor is not a 45 degree Shamfa. It's ten on the vertical and five on the horizontal. So for this, I want to be able to select my two distances. The distance one is my ten, distance two is my five. We need to be careful here about which line we click first. If we click the horizontal line first, it will associate the number ten with that, which is incorrect. So we want to select the vertical line first, then follow that and we can see the preview there. That's correct. Our left click there. It's okay. Now we've got our ten mil on the vertical of the chamfer and the five mil of the horizontal. Okay, let's come up to the top, and we've got this half circle here or an arc. To put this in place, I'm going to be using the arc tool, so three point arc, and I'm going to start at the endpoint of the vertical line. And I'm going to bring that across by the diameter in this case. Twice the radius, in this case is 24. Going to hit tab on the keyboard, and I want to put it in a zero there to lock that angle at zero degrees. Now you'll see we can input an arc like so. I'm just going to click anywhere for the time being. We'll click there. And what I'm going to do is I'm going to tidy up this dimension first. What we're going to do is I'm going to use the tangent constraint tool just to mix it up a little bit. Going to select this arc and then this straight line here. You can see that's now tangential, and that's looking good. So then we'll select the line tool and continue. It's come across by 24. Okay, now I want that to be horizontal, so I have done a slight miss click there, no issues. I'm going to come up to the horizontal constraint. I'm going to select this line here and we'll see that it's now horizontal. We've also got a hex in here as well, so that's starting at the center point of the arc. To do this, we'll come under our rectangle tools. We've got the slots and polygons. It is a six sided polygon, and from point to point is 16 mill. I've got my six sided selected start there, and I'm just going to drag that out left left click. Okay? Press done. Now I want to put a horizontal constraint on this flat here. Okay? So it's in the correct position, and now we just need to assign a dimension to that, to give this 16 mill from point to point, I'll select those two. 16. Then we have out hex in place. I go to bring this 24 up. Okay, that's looking good. So continuing on here, we then have this angled line, so it's 45 degrees, but a length is not specified. I'll leave that till the end, and you'll see why. So let's come back to our starting point at the origin. We'll select the line tool, and we'll continue the geometries from here. So we come up by 18 mill, we come to the left horizontal 18, and then up vertical 24. Then quite simply, we can just come across and we can snap on to the endpoint of that line. Now I want to ensure that this is a 45 degree angle. So for this, I'm going to enter a construction line here, the endpoint here, draw that up. That's vertical. Right click Construction line. And I'm going to select dimension, and I'm just going to double check that this dimension here is 45 degrees, which we can see it is. Okay, that's perfect. We can then delete that construction line. Okay, now coming back to other shampors we see we have a circle or could be a hole. Okay, so we'll select the circle tool. And again, we'll just place this anywhere for the time being. It's got a diameter of 12 mil. Roy, that's put its in position. So it's 12 from this wall here, then 12 from this one here. Our circle fully dimensioned in position. Okay, that's looking good. Just one more thing to add, which is the text up here. Are you a bit of conflict with these dimensions if I move those out of the way. So for the textal come the text options, they're going to select geometry text. So we're going to start with selecting our geometry, which in this case, is this arc here. Now, the text is inventor 2025. Okay, not exactly what we're looking for. First of all, this is offset slightly. You can apply your own offset here. It's up to you. I'm going to apply 2 millimeters in this case. Okay, might reduce the size of that text as well, bring that down to, let's say, 2.5. Then we only need to worry about its positioning. So we want this to shift around the arc. Right now, I've got it left justified, but I want the start angle to be slightly offset. So let's go with 45 degrees. Okay, and that's then put the text in the according position. So 45 degrees from here, we then start the text. Okay? So 45 degrees around. We then got inventor 2025. So it's in the correct position there. Alright, so that's looking good. And then if we look in the bottom right, we can see it's fully constrained. Everything is fixed. Nothing is going to be moving there. That's exactly what we're looking for. And there we go. So that's typically how I would draw such a sketch. If you have any questions on this, please have them in the comment section. I'll reply as soon as I can. And I'll be seeing you in the next example. 21. Project 3 - Sketching: In this exercise, we will sketch this model here. Now, at first, this might look a bit intimidating with all the arcs, circles, slots, and dimensions. But if we break this down, it's actually quite straightforward. But this model, we'll be using the circle line and the slot tools. We'll be using the offset tool, the trim tool, and, of course, constraints and dimensions. So at this point, I would recommend that you pause the lecture and have a go at this yourself using the listed tools. Once again, there is no right or wrong way to sketch this model. We just need to achieve the same final result. So from here on in, I will begin to sketch this myself. So I'm going to start this model with the 30 mill diameter circle in the bottom right. So I'll start a two D sketch. Let's go with the XY plane again, select the circle tool, start at the origin, expand that out to 30 millimeters diameter. Okay? Zoom out a bit. And I can see there's this arc around it with a radius of 30 millimeters, okay? There are no sort of start and end points on this that are distinguished in the model. So I'm just going to start a circle from the center point of 30 mill circle. That has a radius of 30 mill, so a diameter of 60 mill. Right click, okay? Now, later on in this model, I will trim away this part of the circle that we don't need, and that leaves us with the according arc. Moving on, they're going to reference the 18 mill diameter circle. So circle tool again. I'm going to just going to throw that over here 18 millimeters, okay. I can see that that has a dimension from the center of the circle to the center of these circles of 100 millimeters. Okay. Right click. Okay. And I can also see that the center point of this circle is horizontally constrained to the center point of these two circles. So let's once again, select the horizontal constraint, center of this circle, center of these two. And now that's in the correct position, and we are fully constrained. Next up, I'm going to put in this slot. So for this, I'm going to use the center point arc slot. Okay? So the very first point we need to define is the center point, which is here. I'm going to draw that out. I need to know my radius, which as per the model here is 60. Then I'm going to press tab on the keyboard, and I need to put in an angle to define the start point. We can see that from the horizontal, which is 180 degrees within ten degrees in this direction. So 180 minus ten is 170. We defined our start point there. Now the endpoint is somewhere up here. So as per the model, the endpoint is ten degrees plus 100, 110 is okay. Now we've got our start and end center points of this slot. Now we need to give that a width. So in this case, the arc is a radius of ten, so that has a width of 20. There we have our slot in position. I'm going to press right click Okay, to leave the slot tool. And now I can see that the surrounding arc of this slot has an offset of five mil. I'm going to select the offset tool, select my slot. I'm going to bring that out into five on the keyboard, okay? Now I've got my outer slot there. Now you'll also notice that we've got a whole slot here, which we don't need. We will be trimming away this excess material once we have the other geometries here. Let's go ahead and add these in. So we need an arc from this arc to this circle. So to do this, I'm going to choose the circle tool anywhere over here, go to draw in a circle which has a radius of 60 millimeters. I'll enter 120 on the keyboard. That's okay. Right click. Okay. And then this circle here is tangential to this circle. I'm going to use one of our favorite tools, the tangent constraint, select this circle, select this circle. And now we've got that tangential constraint between the two we need the exact same constraint between these two, so I'll select the circle the arc, and there we have the arc that we need. Now, we don't need all of this remainder material of the circle. So I'm going to select the trim tool. I'm going to highlight over this circle, left click to remove that. Right click. Okay. I take off this dimension, and I'm just going to replace that with a radius, select dimension tool, select the arc. But in a radius just makes it a bit more easier to see. Alright, and now here we've got an arc coming up, which goes into a straight line following down, which is tangential to this arc. So I'm going to use the same process here, go to put a circle in place, put that anywhere for now. And this arc has a radius of 15, so a diameter of 30 mill. Gonna make that tangential to this circle here. So this circle and this circle tangential. And then there's a dimension in there. Se the dimension tool. I know that the center point of this circle to the center point of this circle is 22 millimeters. It's looking nice. We're fully constrained. Everything's in position, looking good. And now we just need to add this connecting line, which is tangential to this circle and then tangential to this arc. I'll select the line tool, click anywhere on this arc, anywhere on this circle. Select the tangential tool, select the line, selec the circle. We've got that tangential joint there looking good. Exactly the same process here. Select the line, select the arc, tangential here. That is looking good. Now we can use the trim tool and tidy this up. Select trim. Firstly, I'm going to move this portion of the circle here, which we no longer need. So we're just left with our arc. Again, I'm going to remove that diameter, but in a radius there, tidy that up, ok? Again, select the trim tool and take away this arc which we no longer need. Again, coming up here, we can remove this arc, this one, this one, this one, right click. Okay. And there we have the completed model. So, as I say, when we break this down step by step, it's actually relatively straightforward. All the dimensions are there. We just need to understand the relative tools and constraints that we need in order to achieve the final result. I hope that was okay for you guys. If you managed to do that by yourself, big congratulations. That is quite a tough sketch to do. Again, any questions, please send me your comment. I'll see you in the next lecture. Thank you. 22. Section Intro - 3D Modelling: In this section, various modeling tools will be introduced to convert sketches into three D models. I will begin with the fundamental EtrueTol and we will learn how to add and remove three dimensional material. Following that, I'll go through other common three D modeling tools and commands such as revolve modeling, sweep profile and paths, engraving and embossing, shelling, adding precision holes, fillets and chamfers, and plenty more. Each lecture is presented step by step where I demonstrate how these tools can be used for common practices. Range of examples will be provided throughout the lectures, concluding with three examples for you to practice. Now I will be demonstrating how to complete these examples, but it is recommended to attempt them independently using the tools and skills learned in previous lectures. I hope that you enjoy this session. And again, if you have any questions, please don't hesitate to contact me. Thank you. 23. Extrude and Cut: In this lecture, we will learn how to use the extrusion tool and understand its various options. We'll be using this tool to add material and also to remove material in order for us to model this part here. Let's take a quick look at this part. It's a basic block, 100 mill width, 60 mill height, and a depth of 20 mil. We've then got this rectangular slot which runs through it, which is 40 by ten mil. And then we've got this cylindrical boss, which is 20 mill, out of diameter of 25 mil inner diameter of 20 mil. So let's start with the three D block very easy to draw. Come up to sketch mode, start a two D sketch, and we'll select the XY plane. We'll use the rectangle tool, start at the origin, expand that out, and straightaway, we'll input the dimensions. So we've got 100 mil and the width and the height, in this case, is 60 mil. Zoom out a bit. Okay, that's looking good. Now let's go ahead and three D model this. Let's extrude it. So we come to three D model. We have a whole array of tools available here. We'll be covering many of these in the following lectures. In this lecture, we're going to focus on the most common tool, which is extrude. Now, as soon as we click that, a dialog box shows. Just to start with this, you can move this around the environment. It's not fixed there. You can also hold down on the tab itself, and you can actually install it just on the toolbar on the left hand side, if you prefer. My preference is to have it in the environment and I can move it as necessary. You can also change its shape, like so. So let's have a look at the inputs here. So first of all, we've got the input geometry. So here we're defining the profile in which to select. So one profile has been automatically selected. We click the cross there. We can then hover our mouse over our shape that we can see there in red is highlighted. That is one profile that we can extrude. And that's the correct one. So we'll click that. Is extruding from, so the sketch plane, yet we want to extrude from that plane, correct? Then we've got behavior. So here we're under the default direction, right? So as we can see by this arrow is extruding in this direction from the sketch plane. You want to flip that, flip. Now we're extruding in the opposite direction. We've also got the symmetric symmetric extrusion. So in this case, we're extruding a total of ten mil, okay? So that's five mil in the default direction and five mil in the flip direction. We've also got the option here for asymmetric. So this is where we need to input two distances. So we've got distance A. Let's put that as 30 mil, and distance B, let's just put that as ten, and we can see that from the sketch plane, we're extruding 30 in this direction and then ten in this direction. But for this model, we only need the default direction, so we'll just click that. And we need a distance of 20 mil. Then we've got the body name. So this is what will appear in the design tree here. So let's say extrusion one. We've also got some advanced properties which are rarely used. In this case, we can put a taper on this. So if I put a five degree taper, I look through to that, we can then see this five degree taper just here. And if we flip that, then we can see the taper in the other direction. There's no taper on the block that we're drawing, so we're going to leave that as zero. Okay, I'll press Okay. And there we have our very first extrusion, the block. So moving on to the next feature is a rectangular slot through this face here. So to do this, we need to sketch on this plane. Now, the easiest way to do this is to left click on that plane. We've got a series of options here. So we can edit the extrusion, we can edit the sketch, and so forth. But on the right hand side, we can create sketch. Okay. So once again, left click. Then we left click Create sketch, and now we're sketching on this plane here. We want to sketch in that slot. Let's go ahead. Rectangle tool. It's 40 milwidth ten mil height. We want to position that, go to use constraints. So we're going to use a vertical constraint. So that will be from the midpoint of this line to the midpoint of this line and a horizontal constraint, midpoint of this line to the midpoint of this line, right click. Okay. And now we can see we're fully constrained on the bottom right corner. Everything's fixed in exact location. That's perfect. Now we need to go ahead and cut all of this material out according to this geometry here. We're going to use the extrusion tool once again. Let's go three D model, like extrude. And now as we can see, the preview shows actually adding material, which is not what we want. And if we come under the output option here, we then got the output of cut. But this is where we remove material, and if we select that, we'll see the preview is now cutting material, which is exactly what we want. Unfortunately, it's just not exactly the depth that we want. It's extruding by a distance here of 20 millimeters. Now there are different options for us to control how far this extrudes. Uh, one option is to extrude, yet the full length. So in this case, 60 mill, okay, that previews showing correct. That's what we want. I want to show you a few other options as well. So an option here is to go through all. So if I put that back to 20, if we select through all, it will recognize all of the material to remove and do that automatically for us. That's great. That back to 20. And then if we select two, here we need to select a face. So we can say extrude to a particular face. In this case, the face will be this one, and if I left click here, we'll see the preview shows correct, extruding all that way through. Another one, let me put that back. Another one is two next. So if we click To next, inventor will automatically recognize where the next face is and it would extrude there. But in this case, I would just commonly click on through. No taper involved. We can hide the advanced properties, and if we click Okay, we've then got that extruded slot there. Perfect. And the last feature to add on this block, we need to extrude this boss feature, and that's coming from this face to a left click the face and create a sketch. Let's get these cylinders in there. So let's start with a circle tool, draw that anywhere for now. Got an inner diameter of 20 mil. And I'm just going to use the offset tool to offset this circle here. Now, the outer diameter is 25 mil, so there's a wall distance there of 2.5 mil. So offset by 2.5. Now, this sketch is still free to move, so let's use our constraints once again. Let's use the vertical constraint, centerpoint, to the center point, horizontal constraint, centerpoint to center point. Now we're fully constrained. Everything's fixed. That's looking good. Now let's go ahead and extrude this. So three D model. Let's select the Extrude tool or shortcut E on the keyboard. Now here, inventor has not selected for us a profile to extrude, and that's because it's not sure which profile to select. We've got one profile here and one profile here. So this is the one we want to go for. Let's click that. The direction is correct. So the default direction, we don't want to go the other direction, and the total extrusion is 20 millimeters. Okay, we'll press Okay there, and then we've got our boss. And there's just one more feature we need to add here because there should be no material here. So we want to cut away this material up to this face. Note that in the model, it does not go all the way through the block. Though quite straightforward. We want to sketch geometry on this plane. Left click Create sketch. For this, I will use the projected geometry tool. So I'm going to project this geometry here. If we zoom in, we can see I'm going to left click here, and then we've got this yellow circle that's appeared there, that's a direct projection of this geometry here. So I've just projected that onto this plane. So from here, we'll go to three D model, go extrude. Now we want to extrude cut, but again, inventor is going to add material, not what we want. So we'll select the CUT output. And if we look down, it's going through the entire body, not what we want. We only want to come up to this face here. Though different ways to do this, we could just select to the next and then select this face here. Okay. We could also enter a distance there. So if I enter say ten mil, okay? That's correct. Okay. Through all, we cannot choose because we don't want to go through all the material. Okay, so quite typically here, I would click two, then I would select the according face, in this case, is this one. Cross Okay. And there we could see there's no material loss in here, or the material loss is now in here exactly as per the drawing. So that is an overview of the EtruTol. It's the most commonly used three D modeling tool, very simple to use, very straightforward. We will be using this tool in many future lectures, and I will see you there. 24. Fillet and Chamfer: In this lecture, we will learn how to use the fillet and the hamper tools and the various options within them. We're going to continue working on the part that we've done in previous lectures. But first of all, let's start by applying some fillets. Come up to the modification tab, select the fillet tool, and our dialog box pops up. So for a basic fillet, essentially, we can input our fillet here. So that's the radius. Let's go with 2 millimeters, and then we can just select an edge. For example, I'll select this one here, I press Okay. We then got our two mil radius on that edge there. We want to edit that, and right click on the fillet, select Edit feature. Then we can make the according edits. If we want to unselect this edge, hold down Control on the keyboard, and this will turn red, left click once and it will remove it. I also want to show you the variable radius as well. I've selected my variable radius, to select my edge. Need to put an input here. 0.0 is the start. Let's put that as one mil radius, and then at 1.0, which is the ending point. Let's go over three and exaggerate that. As we can see, we've got this variable radius here, starting at one mil and ending at three. Go to edit that feature one more time and remove that fillet. Another example I want to show you is how we can select edges. So, for example, right now we are selecting individual edges, but what we can do is select the loop option. So if I now hover my mouse over this edge and I click there, we can see that inventor has recognized that loop of edges, and then we can assign a radius to that. So if I put, let's say, two mill, press Okay, then we can see a two mill radius has been applied to all of those edges. Again, I'll come back to edit that feature, the cross to remove that. One more feature I'd like to show you is about selection as well, and that's to select actually an entire feature. So right here, we cut away material of this entire slot. Now, if I select that slot, it will pick up that feature and it's associated edges. Then by the preview, that looks good. Click Okay. You can see that a two mil radius has been applied to all four of those corners. So let's go ahead and apply a few fillets to this part. I want to modify this. Let's go for 3 millimeters. I want to add another radius. So I'm going to cook plus here. I'm going to assign that one mil radius. Let's go for the loop selection, saves us a bit of time, a bit more easy. We'll select that loop there. Also select the loop on the underside, like so. Also add in one more radius as well. And this time, I'm going to hit the feature. That's going to be a two mil rad. I'm going to select this block here, all of these associated edges. Okay, so it's picked up all of them, that's looking nice. I'm going to add one more end of this one, which is a one mil here. Then if we click Okay, you can see we've applied a whole series of constant radiuses there, that's looking nice. It's a very simple tool to use, and we just say how much that we want for the radius to be if we want it to be a constant or a variable. We choose our selection tool, and then we can choose to add more radiuses if we like. And again, in terms of edits, we just right click Edit feature, can change anything accordingly there. Let's move on to the ShampTol now. So very straightforward. Again, under the modified tools in the top left, got the hamper option here. Different dialogue box compared to the Fillet one. First of all, we need to select our edges. For this example, I'm going to choose this edge here. Now, the type of shampo that we're applying is a 45 degree hamper, okay? So let's go ahead with that. Let's just say 1.5 mil. That's okay. If we view this from the left side, we can see we've got this 1.5 mil on the horizontal, 1.5 mill on the vertical, so 45 degree shampa. Right click on that, press Edit. I'd like to show you the distance and angle. So here we select the distance. Let's go again with 1.5, and let's choose the 45 just to begin with. But first of all, we need to select the base. Here's the face, and then we need to select the according edge, which in this case, will be the outer one, going on the left view. And what we'll see here is exactly the same hampls been applied. So it's 45 degrees by 1.5. But if we change this, let me change that too. Let's say 15 mil. Then see that the 1.5 mil is coming from this face up vertical, and then we've got the 15 degree angle, a very sort of acute angle coming off. Another option we have is two distances. So here we just select an edge, say this edge, then we define distance one and two. So let me exaggerate that 0.5, and let's stick with two. Let's go on the left view. And if we look at that preview there, we can see that the 2 millimeters is the horizontal and the vertical is 0.5. Likewise, if I change those around, I'll do two mill. This one's now on the vertical, and the 0.5 is on the horizontal. Okay, let me go to edit that one more time. Edit feature. We're gonna stick with a 45 degree champ. It's most common. I'm gonna go for a one mil. Select this shirt. That's okay. There, we've got our 45 degree one mil champa. 25. Viewcube: In this lecture, we'll take a look at the view cube. Now, you may have seen me use this tool quite a lot throughout the previous lectures, and I'll definitely be using it for future lectures as well. The view cube is up here on the top right hand side, and it lets us view our part from different angles. So, for example, we can look at the front view, then we can use the arrows to move around, like so. Okay, top view, Okay, right view. We've also got these rotational angles here, so we can rotate our part, like so. Very important button that I use a lot is the home button. If we click this, we're automatically brought back to the home view, which is between the top, front and the right. Now, there are various changes that we can make to this. The right click, we've got an option there to go to home or just click the button, so I'm going to use this one. We can quickly change how we view this, so orthographic or perspective. So if I change a perspective, gives it that element of realism. Is that we would typically see that, with our own eyes. And for me, I typically work in orthographic. Another view as well, which some people use is perspective with ortho faces. So we're looking at this in perspective view, but if we look at the top, you'll see we then change to author view, okay? So it just enables us to sort of see those faces from Athoview but see the rest from perspective. Set current view as home. So this is currently the home view. If we want to change that, let's say, we'll choose this corner here. We right click and set that as home. Now, a fixed distance so I could fix the distance like so. We can bring it really close, or fit to view, so inventor will automatically adjust that. So if I now go to the home view, Okay, there we go. We've got to our new home view. I'm going to turn that back. Another option we have is to set current view as. So what we can do is, if this is our left view so, we can go to set current view as the front, and we'll see it's now changed to the front, okay? If we want to reset that, we can go reset the front. And likewise, we can do the same with the top as well. A few options here. I'll only run through a few key ones to display where the view cube actually is, so that it's top right, we can put it in, let's say, the bottom right, click Okay, and now we see it appear down here. Go back to options. I'm going to put that back on the top right. Cube size, I always have this as normal. Some people like it large. So people like it smaller, so they got more realistic to play with, but that as large and the inactive opacity. So when we're not using the view cube, it's how obvious it is on the screen, basically. So we put that to 25%. Okay. We now see the view cube is a large size, and we see that it's quite transparent. You know, it's quite well hidden, as soon as we move our mouse over it, it comes fully into view. I just put those back, so I typically do normal, typically have on 100%, but feel free to play with any of these options here as per your preferences. Okay, I will see you in the next lecture. 26. Revolve Tool & Modelling: In this tutorial, we will learn how to use the revolve tool. So so far we've done Extrude tool. Another very important tool and commonly used is revolve. So revolve is creating a feature or a body by revolving one or more sketch profiles around an axis. So this is the part that we'll be modeling here. And in order to model this part, we need to create a sketch and an axis and then revolve that sketch about the axis. So if we move on, this is then the sketch that we need to draw. It's a very straightforward sketch. If you'd like to do this by yourself, by all means, please pause the video and go ahead. But if you'd like to follow along with me, I will create this sketch for us now. So let's go on Start Tod sketch. For this, I'm going to choose the YZ plane. I'm going to select the line tool, start at the origin. Immediately, you go left 100, okay? Do them out a bit. Then we're going vertical, so 90 degree up by 40, going to the right by 60, Vertical 80, the left by 60, Vertical 40. You go to the right 16, bound 12 to the right, 24, up 12, cross 16, bound 12 or more 24. Up another 12, and then we'll go to the right by 20. Then we're going to finish off that sketch by coming down vertically at 90 degrees back to the origin. There we have a full sketch profile. So the very first thing we've done there, we have our sketch. Now we need to create our axis. So for this axis, it'll be a straight line. We can draw that line in anywhere for now. It can be any length. Let's just go for 100. Right click. Okay. Now, this sketch, we need to be a fixed distance from this line here. So for this, they're going to choos the dimension tool, select this line, select our axis. And the dimension here is 15 millimeters. A good practice. I'm just going to right click on this and set it as a construction line. So we've got our sketch. We've got our axis, and now all we need to do is revolve them. I'm going to hit Finish Sketch. Okay? Go back to the home view. Come up to three D model, and we'll select the revolve tool. Our toolbox pops up here. Remember, we can dock that here if you prefer. Okay, or change the size of it like so. And a few options here. So the profile inventors selected the only profile available, which is correct. We do want to revolve that profile. We just need to tell it which axis to revolve it around. So in this case, we'll select our construction line. We see a preview of the part there. And then just like the extrude tool, we have the behavior options here. So in which direction that we're rotating this. So if we flip it, symmetric and also asymmetric and also by the angle. So if I set that at 270, then we flip the direction. Yeah, we can see we flip the extrusion like so, or we can go symmetric. So yeah, 270, but I'll be split in both directions. So 135 each way. Or we can go asymmetric. So here we're going to put in two angles, so we can go 270 in one direction, and then perhaps we can go. If we put in 20 degrees, we'll see we only go 20 in that direction. But for this model here, we're only revolving by 270 degrees, so I'll select the default. Okay? And again, body name, we can call that rev one, but go okay. And there we have our revolved part. A very straightforward tool. All it requires is a sketch and an axis to then revolve that sketch around. This can be used for many different geometries that have revolution features such as this one here. Okay, hope that all makes sense, and I'll see you in the next lecture. 27. Sweep Tool: In this lecture, we will learn to use the basics behind the sweep tool. And the example model, in this case, is an RClp as we can see here. The sweep tool is very straightforward to use. It consists of two sketches. One sketch is your profile and the other sketch is a path. So let's go ahead and I'll demonstrate on how to use a sweep tool in order to draw components such as this. This diagram here will show you the dimensions that I'm using, but that down in the bottom right corner, then we'll go ahead and we'll complete these sketches, and then we will sweep the profile along the path. So as I say, there are two sketches. The very first sketch is the profile and the second sketch is the path and the profile will extrude through the path. We will follow that. Let's go ahead and do the profile, which is very straightforward. For this, we're going to choose Y Z plane. We're going to choose the circle tool, start at the origin. We're going to bring that out to a diameter of 4 millimeters p enter. Okay. And then we can finish our sketch there. That's one sketch complete. That's our profile. Now we only need to do the path. So we'll start a new two D sketch. This one here will be on the XY plane. Okay? Let me just draw a line in there to demonstrate, make sure we start our line from the center point of the circle. We don't want it offset. Check in our line there. So what's going to happen is when we use a sweep tool, this sketch here, our profile will extrude following our path. So let's go ahead and finish off the remainder of our path. So following the dimensions on the sketch in the bottom right corner, we've got 68 mill length there. Then we're coming into an arc, a straight line down, another arc, another arc, another arc, and then the ending point. I'm going to put in all of the points for all of these arcs, and then we can just add in the lines and the arcs afterwards. So quite straightforward. Let's put in our first point. It'll be the large arc there with a rat of 12.5. I know the dimension between the center point of that arc and this baseline here will be 12.5 millimeter. I just want to make sure that is vertically constrained. So a vertical constraint between the point and the endpoint here. No fixed in position looking good. Now let's go ahead and add in that circle there. So start from the point in there, bring that down. And there we've got our arc and the arc is going to finish off somewhere here depending upon where the other arcs are. Go ahead and add in another arc then. We'll do our center point first. We'll dimension that. Center to center there, we've got 24.5 millimeter. And we've got a height here of about 10.5. Okay, let's go ahead and add in our circle, which will turn into an arc later, the rot of five diameter of ten. Do the same thing. We've got another point. I was just roughly down here. Dimension that from the original center point there, which is 36.3. It's got a height there to the base of 5.6. Go ahead and add in a circle there. Okay, Route five, diameter ten. Good, add in the other arc as well, roughly up here. We know that it's horizontally constrained to this circle here. Is a horizontal constraint. I like that point. I like this point. Then we'll just put in one more dimension to the center point of this circle. That is 53.2. Then we've got one last point. I'll throw it over here. Again, that's horizontal to this point here. Constrain those two. And then I'll dimension that point there. Original center point over here at 68. Hey, everything's fully constrained. Let's go ahead and add in the remaining arcua diameter ten. Then we just need to use the line tool quite simply start forming lines between our circles like so. There'll be the path. The profile follows. I use the tangent tool here. So I believe this is already tangent. Okay, so now that's tangent line to circle. Okay, that's already tangent line to circle. Again, just repeating that good. We can tidy this up. We use the trim tool. Don't need this material, this material, this material, this material. If we finish the sketch there, let's take a look at where we are. But our profile will follow a straight line around this arc, down, up, down, and then to the end point there. Looking good. Go to three D model then and try this out on the sweep tool. Now under the profile, inventors already selected our profile. Okay, fantastic. Then at the path, all we need to do then is to select the path, which in this case, is what we've drawn here that sketch. Not going to include a taper or a twist. And if we look at that, that's looking good. If you do want to experiment with taper, you can. If I put a one degree taper on that, you'll see it becomes larger, one degree. If I minus that, let's do -0.3, Okay, 0.5. You can see by the profile there what the taper does. But for this, an RClip doesn't have a taper, plus okay. Going to tidy that up a little bit. I'm gonna apply material to this. Let's go with carbon steel. Gonna come under the view tab. Gonna put the visual style shaded. You're on the home view. There we have our completed arclip using the Sweep tool. It's a very simple tool, two sketches, a profile and a path. The profile will follow the path throughout its extrusion. Okay, I hope you're able to follow along, okay. Any questions? Please send them to me. Apart from that, I will see you in the next lecture. 28. Engraving Embossing Text: In this tutorial, we will learn how to engrave or emboss text. So in the two D sketching section, we learn how to add text or text geometry, and now we'll apply those principles to our part that we have here, we'll either engrave or emboss that text. So let's add some text to the front face here. So we left click on that face, create TD sketch, bring that to the center roughly, and then we're going to add in some geometry text. So we need some geometry to kind of project this text from. So in this case, I want to use this edge here. So I'm going to project then select that edge there. Now we see that's now in yellow. It's a direct projection, and we can use that to base our geometry text. So we come up to the text tool, and we'll select geometry text, and then we need to select the geometry for that text to be on. In which case, it's our yellow line. We have our dialog box pop up here. Feel free to write your name or anything else you like. I'm going to write Inventor 2025. I'm going to select that. I want to offset it from this line. So I want it slightly up. Let's go with 3 millimeters. In terms of justification, let's put it on the right justification. Make that bold. I think there was about all the edits from here. Let's also add a few spaces after the last piece of text. Let's add four spaces. It's okay. Then we can see we've got that text on the bottom there. So that's two dimensional currently. Let's look at how we can emboss that from the surface or engrave it into the surface. So for this, let's finish the sketch. Let's come up to three D model, and we'll select our Extrude tool. Now we need to select the profile in which to extrude. So in this case, it is a text itself. We'll select that. It's extruding from the sketch plane, which is correct. And in terms of direction, yet, that's looking correct to emboss the text. Okay, let's go by 0.5 mil. Okay. There we've embossed that text onto our part. Let's have a look at how we can engrave this. So if you want to change this to engraving, we can come up to our design tree. We can right click on the extrusion. We go down to Edit feature. Then from here, we're just going to make some small edits. So first of all, we want this to cut into the material, and just make sure that we're cutting in the right direction. So we need to flip the direction. Yep, so we're cutting into the material. Now. If we look from the right side, we can see that we're now engraving into the surface. We press Okay. There we can see we've engraved our text there. Okay, so a very simple tool to use and can be very effective, especially if you're designing molds for plastic injection. Okay, let's leave that on this part, and I'll see you in the next tutorial. 29. Fillet and Chamfer: In this lecture, we will learn how to use the fillet and the hamper tools and the various options within them. We're going to continue working on the part that we've done in previous lectures. But first of all, let's start by applying some fillets. Come up to the modification tab, select the fillet tool, and our dialog box pops up. So for a basic fillet, essentially, we can input our fillet here. So that's the radius. Let's go with 2 millimeters, and then we can just select an edge. For example, I'll select this one here, I press Okay. We then got our two mil radius on that edge there. We want to edit that, and right click on the fillet, select Edit feature. Then we can make the according edits. If we want to unselect this edge, hold down Control on the keyboard, and this will turn red, left click once and it will remove it. I also want to show you the variable radius as well. I've selected my variable radius, to select my edge. Need to put an input here. 0.0 is the start. Let's put that as one mil radius, and then at 1.0, which is the ending point. Let's go over three and exaggerate that. As we can see, we've got this variable radius here, starting at one mil and ending at three. Go to edit that feature one more time and remove that fillet. Another example I want to show you is how we can select edges. So, for example, right now we are selecting individual edges, but what we can do is select the loop option. So if I now hover my mouse over this edge and I click there, we can see that inventor has recognized that loop of edges, and then we can assign a radius to that. So if I put, let's say, two mill, press Okay, then we can see a two mill radius has been applied to all of those edges. Again, I'll come back to edit that feature, the cross to remove that. One more feature I'd like to show you is about selection as well, and that's to select actually an entire feature. So right here, we cut away material of this entire slot. Now, if I select that slot, it will pick up that feature and it's associated edges. Then by the preview, that looks good. Click Okay. You can see that a two mil radius has been applied to all four of those corners. So let's go ahead and apply a few fillets to this part. I want to modify this. Let's go for 3 millimeters. I want to add another radius. So I'm going to cook plus here. I'm going to assign that one mil radius. Let's go for the loop selection, saves us a bit of time, a bit more easy. We'll select that loop there. Also select the loop on the underside, like so. Also add in one more radius as well. And this time, I'm going to hit the feature. That's going to be a two mil rad. I'm going to select this block here, all of these associated edges. Okay, so it's picked up all of them, that's looking nice. I'm going to add one more end of this one, which is a one mil here. Then if we click Okay, you can see we've applied a whole series of constant radiuses there, that's looking nice. It's a very simple tool to use, and we just say how much that we want for the radius to be if we want it to be a constant or a variable. We choose our selection tool, and then we can choose to add more radiuses if we like. And again, in terms of edits, we just right click Edit feature, can change anything accordingly there. Let's move on to the ShampTol now. So very straightforward. Again, under the modified tools in the top left, got the hamper option here. Different dialogue box compared to the Fillet one. First of all, we need to select our edges. For this example, I'm going to choose this edge here. Now, the type of shampo that we're applying is a 45 degree hamper, okay? So let's go ahead with that. Let's just say 1.5 mil. That's okay. If we view this from the left side, we can see we've got this 1.5 mil on the horizontal, 1.5 mill on the vertical, so 45 degree shampa. Right click on that, press Edit. I'd like to show you the distance and angle. So here we select the distance. Let's go again with 1.5, and let's choose the 45 just to begin with. But first of all, we need to select the base. Here's the face, and then we need to select the according edge, which in this case, will be the outer one, going on the left view. And what we'll see here is exactly the same hampls been applied. So it's 45 degrees by 1.5. But if we change this, let me change that too. Let's say 15 mil. Then see that the 1.5 mil is coming from this face up vertical, and then we've got the 15 degree angle, a very sort of acute angle coming off. Another option we have is two distances. So here we just select an edge, say this edge, then we define distance one and two. So let me exaggerate that 0.5, and let's stick with two. Let's go on the left view. And if we look at that preview there, we can see that the 2 millimeters is the horizontal and the vertical is 0.5. Likewise, if I change those around, I'll do two mill. This one's now on the vertical, and the 0.5 is on the horizontal. Okay, let me go to edit that one more time. Edit feature. We're gonna stick with a 45 degree champ. It's most common. I'm gonna go for a one mil. Select this shirt. That's okay. There, we've got our 45 degree one mil champa. 30. Shell & Holes: In this lecture, we will take a look at the shell tool and also how to add holes. So for the shell tool, let's start with that. I'm going to start a two D sketch. In this case, we'll select the X Z plane. Going to use the rectangle tool, two point center rectangle. To start at the origin. Going to zoom out. We're going to do 100 mill, es tab on the keyboard, Enter 100 again, Enter. We've got a square 100. Got a three D model. Let's extrude that. Extrude that as well by 100 so that we have a cube 100 by 100 by 100. That's okay. Now we're going to use the shell command. Let's click this. Our dialogue box pops up. Now, we have the option here to remove a face. I'm going to do that for the purposes of this lecture as we can see more clearly what's happening. By the preview, you can already see that we have a wall thickness there, which currently is one mil. Then we bump that up to ten mil. Well press Okay. If we zoom out, we can then see that I've shelled away the inner material. Right click on Shell, Edit Feature, click Remove faces, so I can remove another face. I'm to select this one here.Rsoka. Now we can see that both of those faces have been removed and we have our ten mil wall thickness. I'm going to select that sketch, right click on it and turn on the visibility, and we can see the dimensions there. I want to show you edit that feature again. The difference that's made if I select an outside shell or an inside shell. The shell we've done is inside. What's happened here is that the ten mil wall thickness has been added to the inside, and then any further material inside has then been removed or shelled out. But if we click outside, we'll see that the ten mil wall thickness has been added outside of our sketch. And that anything inside of the sketch has then been removed. There's one more option here as well, which is the kind of both inside and outside. So we'll see here that five mil has been added to the inside, five mil to the outside, and anything further inside of that has been shelled out. That's okay. Okay, and we just turn the visibility for that sketch off again, and then we'll move on to the whole command. For the whole command, let's go back again and work on this part here. I go to use this as a demonstration for the whole command. Let's select this face here. This is where we want our holes to go through. Click Create sketch. Okay? Now we're facing this plane here. Now, we need to add some reference points for where these holes are to start. So for this, we use the point. I'm going to sketch in one point there and roughly one over there. Do the dimension tool. But these in an accurate position. Let's go six from this edge here, and then six from this edge here. Likewise, we'll do the same over here, six. Same here. Six. Those are now fully constrained. And there are reference points. Let's finish up the sketch there. Let's go to three D model, and we'll select the le command or shortcut H on the keyboard, then we'll see this dialog box pop up. The very first input is the geometry. So in this case, inventor has selected for us both of the points that we've added, which is correct. You can choose these manually. So if we clear the selections, we can select if we just want the one, or in this case, we'll go for the both, so we'll keep them both selected. In terms of the type, we need to define the hole. So in this case, simple hole, clearance tapped, and then a taper tapped hole. So for this example, we're going to go ahead with a simple hole. We also need to define the seat. So right now we've got the counter sink option selected. There's a spotface option, okay, like so. There's a counter bore option, like so, or there's no seat at all, and it's just a straightforward through hole, so no seat. Let's go with a countersunk hole. Both of these. Let's come further down. So termination. Right now, I've got the through all selected. So these holes will go through all of the material available. We want to change that and only want that to be a certain depth, we can select a distance there. And also select the type of drill point, okay? So going from there before this demonstration, we're going to go with through all. We can also select two, as well, which we can then define like a face to go to. Alright, let's stick with through, and then direction. We don't want to well, there's nothing we can drill in the other direction. So keep the default direction, that's looking good. And then we've got a series of numbers here, which we can define ourselves. So the diameter of the countersunk. Yeah, let's go with eight mill. The angle, stick with 90, and then the diameter of the hole itself. So yeah, let's stick with five mil. In this case. We press Okay. And now we even put two countersunk holes which go through the diameter there of 5 millimeters. Et's just go back quickly to that tool. So you see there are many options, many different types of holes, many variables and inputs that we can give. We can customize this as much as we need, feel free to have a play around with this tool. And aside from that, I will see you in the next lecture. 31. Applying Threads: In this tutorial, we will learn how to apply a visual thread. So to demonstrate this, we'll go ahead and draw this basic hex head bolt, and then we'll apply that thread. So let's start with a two D sketch. Let's select the XY plane, and we'll start with a polygon. So we'll come under the rectangle tools, select our polygon tool. Make sure we got the number six there so six sides, start at the origin, bring this out. Right click. Okay. And then immediately we'll add a dimension, which will be the dimension of the flats. So flat to flat dimension, in this case is 10 millimeters. Looking good. Tidy that up. I'll put in a vertical constraint on this line here. Make sure it's like so it's fully constrained, looking nice. Let's go ahead and extrude that then three D model. Let's go extrude. We'll go for as per the drawing, 4 millimeters, okay. Looking good. Now we need to draw the shank and the threaded part. But in that case, we'll be drawing on this face. Left click once, create two D sketch. Wants to use the circle tool, start at the origin, open this up. This is an M six bolt that will go for 6 millimeters in diameter. Right click, okay. Back to three D model. Let's extrude that. So total length is 20 millimeters. Let's enter. Okay, let's also put a shampa on this edge here. They use the hamper tool here. Add the hamper, in this case, it's an equal chamfer of 0.5 mil, so not 0.5. I'll select that edge there. That's okay. But our hamper there. We've got the hex head. Now let's go ahead and add this thread. So for this, we come up to the modified tools, and we select the thread. Okay, our dialog box pops up once again. So the input geometry, we only need to enter a face here. So very straightforward and a click on this face here. And then we have some details pop up. So this is where we can detail the type of thread. So you'll select the according standard, I typically draw using isometric profiles. The size, it's recognized, the diameter there. So at six, then designation, so the thread pitch. So yeah, the standard. I'm going to go for six by one. Class and then direction clockwise, counterclockwise, and then behavior. So if we want to do a full thread, we can select this button here, which is full depth, okay, full thread, so 19.5 mill. But in this case, we can only enter. Let's go for 16 millimeters. Okay? Press okay. There we have our visual thread. Now if we zoom in on this, we can actually see that there's no material missing from this shank. And that's why I say it's a visual thread. It's not a physical thread. Now, one of the great advantages about this in Autodesk inventor is that a visual thread will not consume a lot of hardware power. As soon as we start taking off material here and having a physical thread, the part file becomes increasingly large, and it can really put a strain on your hardware and your computer. Where we're able to do visual threads, I would always recommend using them over physical threads. Okay, I hope that makes sense. Any comments, please put them in a comment section, and I will see you in the next lecture. 32. Materials & Appearances: In this lecture, we will learn how to assign a material to a part and also an appearance. So right now, these are controlled at the very top. These are controlled at the very top. So we've got two boxes here with drop down options. The very first one is a material. So let's the drop down there. At the very bottom, we've got options there so the favorites, the autodesk material library, which is huge, then the inventor material library, which generally has everything that we need. So for this example here, let's go ahead with a stainless steel, and immediately, we see the appearance of this change. We've got this nice stainless steel visual appearance, and all the properties of generic stainless steel have then been applied. For example, if we go into file and then select I properties, then come under physical, click Update. We've now got information such as the mass of this part according to those dimensions and the material assigned, this weighs 0.776 kilograms. We've got the area there, millimeters squared, and the volume millimeters cubed and so forth. But the mass itself is actually calculated, taking into account the density, in this case, of stainless steel. So that's how we assign a material, a bit more advanced on top of that if we select this option here. So yeah, material brings up this box here. If we open up the home, then we open up the inventor material library, we've got a series of options here that have been categorized under ceramics, concretes, we've got liquids. We've got a whole series of metals here, but plastics, as well. So we can choose to add any one of these materials and assign it to our part. For the most part, I do it from this drop down here. In this case, I've selected stainless steel. On top of that, we can also apply an appearance. So stainless steel has been associated with a semi polished finish. Okay? And that's a reference directly to stainless steel. But if we want, we can also change that. So, for example, let's go on, I know, sky blue dark. Okay? So this is now the appearance. Now, this part will retain the properties of stainless steel. The appearance will be, in this case, sky blue dark. Okay, I'm going to press Control Z to go back. And what we can do is assign appearances to individual faces. For example, if I select this face, I can then assign, let's go for red, and then we have that appearance there. Control Z. What I want to do here is assign an appearance to the inventor 2025 embossed text. So I need to select all of the faces there. There are different ways to do this. Number one, I can just hold down left mouse button, drag over all of those, and let go, and I've selected them all. Another way is to actually select the feature itself in the tree. But in my case, extrusion ten. Hey, I'll select that. All those faces have then been highlighted. Going to come under the appearance. And I'm going to give this let's go for an anodized black appearance. West the front view. There we go. So it's looking like it's nice. It's got quite a bit of contrast there on the stainless steel appearance of the remainder of the part. If you want to remove any appearances that you've assigned, you can click on clear. And if we bring this across, we can say select all. Okay? So we'll recognize the appearance that we've assigned. So that's an anomaly in this case. Click Okay. And then that has returned to the semi polished appearance, as is linked with the stainless steel material. Cross Control Z on the keyboard, bring that appearance back. I quite like that. Looking good. Okay, so feel free to assign any material you want to this part and also any appearance. Feel free to have a play around. Okay, yeah, thanks for listening. Any questions? Please put them in the comment section, and I'll see you in the next lecture. 33. Decals Images: In this tutorial, we will learn how to add an image to our part. So I'm going to be working on the same part that we've been doing in previous lectures. And to do this, it's quite a straightforward process. We come up to start a two D sketch, and then we need to select a plane or a face. In this case, I'm going to be adding my image to this face here while left click on this face. And then I'll come up to the insert, which is under the sketch tab, and then I'll move up to image, so insert image. Then if you head to your location of where your images, our location is here. It's called picture one. It's open. Now I see this box appears, and we need to left click on where we want this to go. I'm just going to put this to the side by now, and we'll see how big this is. Okay? As we can see there, it's quite a large image, the engineer loading. So if I move that over our part, it's far too big. I need to scale that down. Come back to the front view, so I'll click on the front face on the ViewCube. I'm going to move this over here. Now, in terms of scaling, we have various options. Number one, we can just select the image. Come over to the corner here, hold on the left mouse button, and we can scale that manually like so. Another option is to use the scale tool. So under sketch, come up to the modified tools. Got the option here to scale. You need to select what we're scaling. In this case, the image. We need to select a base point. In this case, we can choose what we can choose anywhere on the image. I'll just choose this corner, and then we can input a scale factor. I want to scale this right down, so roughly like this. So if we go 0.25 per center, we can see that that's scale 0.25. A press Control Z on the keyboard, and I'll show you my favorite way of scaling, which is just to use the dimension tool. Coming up to the image, we can select the horizontal line in this case, and I'm going to give that a dimension of, let's go with 20 millimeters. Okay, so if we come across, I think that size is acceptable. I come out of the dimension tool, I'm going to left click and then track this around. Okay? So it's not constrained in position to do that. Let's come under the dimension tool, select this corner here, select this edge. Let's give that a dimension of let's go for 2 millimeters. I think that looks okay. And then to this vertical edge, let's dimension from the corner point. Let's do that again 2 millimeters. Right click Okay, come out of the dimension tool. And so now the image is constrained, and we've scaled it to the size that we want. Let's click Finish. Now, that's looking good, but unfortunately, we've got a series of dimensions that are showing. We can also see the border around the image as well in this orange color. That's because it's still in a sketch. Okay? So if we look under here, the name of minus sketch 17. Let's go under three D model now. Let's come under the decal tool. Going to select the image. So inventors, there's only one image here, and inventors just pick that up for me. Fantastic. If it doesn't for any reason, then we can then select the image, left click once, and then it selected that image for us in the blue border. Now we'll select the face that we want to decal that too. In this case, it's this face here. So we'll left click once Pres okay. Now we can see those dimensions are gone, and also so is the border. If we look at our design tree, we see the decal command here, what's got a drop down next to it. So if we want to make any changes, we can right click on the sketch, edit sketch, change any of the dimensions, we can rescale this, et cetera. And that's how we can add an image in Autodesk inventor. So feel free to add any image that you like to your part, and I will see you in the next lecture. 34. Basic Rendering: In this lecture, we will learn how to do a basic render. Rendering, I think is absolutely fantastic. I can output a really nice image. It can be used in presentations for clients, co workers, reports that we're feeding back, perhaps to our boss or lecturer, et cetera. Let's go ahead and do a basic render of this model here. So to do this, let's go under the environments tab. Now there are two key environments in inventor. Number one is stress analysis, and then we've got Inventor Studio. So let's select Inventor Studio. In the studio, we've got various options here, okay? So in terms of doing a basic render, we're going to select render image, and we're going to use the options that we have available to us here. So under the general tab, we can define the resolution that we want. So I typically go for 16 by nine high resolution, give me a nice quality output, and I can then use that in a presentation or such. So I'll select this one camera will stick with the standard. Now you can input your own camera bit more advancer rendering. That will be under the camera option here. Terms of lighting studio, I'm just going to go ahead with the default IBL, but feel free to have a play around and choose whichever one that you think is most appropriate or the part that you're trying to show. I'll choose default IBL. And output. That's just saving the image, which we can do. Anyway, we don't need to necessarily select that here. Then the renderer, we need to choose one of these three options here. So we can specify a time to render, so that really comes down to your sort of computer power on the quality output there. We can just state render for 1 minute however many iterations that may be. We can also state a number of iterations. So the higher the number of iterations, the better quality and the more representative and realistic that the rendered image comes out as dependent on the assigned material. So in this case, stainless steel. This is going to set to 64 iterations. Okay, or you can select until satisfactory, so it'll render indefinitely until you tell it to stop rendering until you're satisfied with the quality output. But for this example, I just go by 64 iterations, and the lighting and material accuracy, I'm going to go with high and leave the image filtering as it is. Go ahead and render and see how that comes out. We can see the number of iterations just down here. So iteration is completed, round 11, 12, and so forth. And that's got to go to 64, and that's dependent on the power of the PC that I'm using. And there the 64 iterations is complete and quite happy with the outcome of that render. Now, if I did want to increase the quality, I could increase the number of iterations or just render it indefinitely until I'm satisfied with it. We can still see quite a bit of grain detail here, particularly in these reflections. But for me, that's satisfactory, and I'd be happy to use that in a presentation. In terms of saving the file, you can just click Save then save that to suitable location. Do want to change the angle, it's completely dependent on where the view cube is. So yeah, if you want to render from this angle here or from the home view, you go from the left view. And one thing you can also do is to change if you're an orthographic or perspective. If we view an orthographic, you know, we render like this or if we view in perspective, like I just did there. But overall, I'm quite happy with the render that came out. So yeah, that's how to do a basic render. It can be really effective if you're presenting to clients or your boss to your lecturer, and so forth. I'll see you in the next lecture. 35. Project 4 - 3D Modelling: In this example, we will three D model this part here. So the very first thing we need to decide is where we will start. What will be the very first extrusion. In this case, the most easy part to start in is the base. It's 100 by 60, and I get the 60 from taking the radius of the arc, take that radius of 30, multiply that by two, 60, then we'll add in the arc itself. Then we'll three D extrude that, also accounting for the slot, and then we'll add the other two extrusions at the back of this part. So to begin with, let's start a two D sketch. Let's do this on the X z plane. Let's start with a rectangle tool. Go for the two point rectangle. Start at the origin, bring that over. Zoom out a bit, and let's enter some dimensions. So for the width, let's say twice the radius, so 60. And for the length of this part, we're going for 100 mil. Now we're going to go for the arc, which is around here, move this dimension out the way. So for this, I'm going to use the arc center point. And this is very simple because we're going to start at the center point of this line here. We'll bring that out and well to snap on to the endpoint of this line, and then bring that arc all the way around and then snap on to the other endpoint of that line. Right click, okay. Right click that. But as a construction line, we don't need that to be taken into account when we three D model. Now let's input the slot geometry. So for this, we'll come back into the rectangle and slot tools, and we'll take the center to center slot as we've already got that dimension there of 24 mil between the centers. We'll start at the center point of this arc. We'll bring that across to 24 enter. Okay, now in terms of the width of that slot, it is 16 mil there we have our slot in place. Let's finish the sketch there, back to the home view. Let's extrude. Select the profile. We're going to extrude that as per the drawing at 20 millimeters. Enter. Just go to change the home view quickly. Would prefer to be looking at it like so. So I've selected my corner there on the ViewCube, right click Set current view as home, and I'll put bit to view. The only part left to do are the two arms at the back here. Now, to do this, I would recommend drawing the sketch on this plane and then extruding backwards. Let's left click that face, create sketch. Ahead and model this in. So I'm going to go let's go with the rectangle tool again. Start at the corner point here, bring that up. Now, the diameter of that arc is the length is 48 mil, press tab on the keyboard, and the height of this rectangular part is 50 -20. That's 30. So we've got this rectangular portion in place. Now we need to put the arc in so the same process here, centerpoint arc. Start at the center point of this line. We're going to start the arc at the endpoint of this line, bring that around at the endpoint of this line. Nice. Now we need to put in that through hole. So for this, simply, use a circle tool. Again, start the center point of this line, bring that out, the diameter is 20 millimeters. Let's go ahead and delete that line. We no longer need that in place. Finish the sketch there. Go to three D model extrude. Need to select the profile. In this case, this one here. Okay, so that's going in the wrong direction to what we want. I'll click flipped. And in terms of the depth of this extrusion, it is 10 millimeters as per the drawing. Okay, previews looking good. Press okay. And now we need to add the other arm, okay? So to do this, we could repeat the exact same process, but the time consuming. The way I would go about this is to add a plane, and then I would add a plane running down the center here and then mirror this feature in that plane, so it will mirror into position. So in terms of the options here, I'm going to go mid plane between two planes. My first reference face is this one. My second reference face is this one. And as we can see this preview here, so we've just generated a plane essentially in the middle of the part there. Okay, now let's go ahead and use the mirror tool. So we'll come to our pattern tools, select mirror in terms of features. I'm going to select this feature here so you can either click on it as in the model, or we can come over to the design tree. We can select that extrusion. So in this case, extrusion to. The mirror plane, that's the plane that we created here. So again, we can either click this plane or select in the design tree. And we see a preview in green there. That looks good. Okay, let's go ahead and accept that there we go. There we have both of the features back to the home view. I don't want to be seeing this plane, so we can either right click and turn off the visibility or in the design tree, we can come under the plane, right click and turn off the visibility. There we're left with a complete part. We'll go ahead and add an appearance to this. Let's go for Skyblue Dark. That's quite a nice one. Okay, I hope you were able to follow along okay. And if you did this yourselves, big, well done. Any questions, any comments? Please send them to me. Aside from that, I will see you in the next lecture. 36. Project 5 - 3D Modelling: In this example, we'll be modeling some basic piping structure such as this. I've included the dimensions on the screen here. So if you'd like to have a go at this by yourself, feel free to do so. Just keep in mind what is the optimal feature, the optimal command and tool to use for a part such as this. And moving on, I'm going to have a go at drawing this myself. I'll come up to a new part, select the standard millimeter part, click Create Okay, so we need two sketches. We need our profile, and we need our path. So for the profile, I do that on the Y Z plane. It's like the circle tool. As per the dimensions, we have an outer diameter of 30 mill and a wall thickness of 2.5 mil. So in this case, I'm going to use the offset tool, select my circle, draw that in, type in 2.5, press Enter. Then we can see we've got our 2.5 mil wall thickness. That's our profile complete. We only need our path now now we could do this in a series of two dimensional sketches, but it will get a bit hectic. And what we can do is just to use the three dimensional sketch very straightforward. So we'll start a three dimensional sketch. Select the line too. Make sure we start at the origin of the circle. We don't want to be offset. So make sure that snaps to the origin. Okay? And then we're just going to follow the dimensions from here. So going in this direction, we have a length of 200. Okay, we're then turning right 200, vertical 200. This direction, 200 going down. Then we're going to finish that off 200 there. Right click Okay, to leave the line tool. Now, we need to add in these radii around the corners so they're 50 millimeters. But to do this, we're going to come under our three D sketch tools select bend. And here we'll enter 50 millimeters, then we'll just select the according lines. The one line here, this one. These guys these guys. And the last one. There we go. Okay, let's finish that sketch there. Let's have a look. Got profile is looking good, and the path is looking good as well. That's all as per other dimensions in the drawing and the bottom right. Let's go ahead and see if we can sweep this. Who's our sweep command. Need to select the profile. Now we've got two profiles available to us. This one, this one. Obviously it's piping. We'll be going with this one. Another path. Get on to select our path here. Review is looking good. I like that. Okay, no taper, no twist. Press Okay. Right, and there we go. There we have our model. We go to tidy that up a little bit. Let's add an appearance there. So let's go for a copper. Let's go on view, turn off. So we turn on just shaded. And let's also go on a perspective view. Hey, looking a bit more realistic in what we'd maybe see in real life. Okay, I hope you were able to follow along, okay. And if you did that yourself, yeah, well done. Any questions, please send me a message. Aside from that, I'll see you in the next lecture. 37. Project 6 - 3D Modelling: In this example, we'll be drawing this part here. Now, this might look a bit intimidating at first. There's quite a lot of various geometries going on here. I got a number of different size fillets. We've got some chamfers. We've got some whole features, additional material there coming on the outside, which is then mirrored around. There's a lot of detail to include here. So we need to, first of all, think about which three D modeling tool would be the most optimized for generating as much of this geometry as possible. And in that case, it is the revolve tool. Following that, we'll need to use the extrusion tool, and we can add any hampers later. So at this point, I would recommend that you have a go at drawing this yourself using this sketch schematic here, which is a basis of the revolve feature. But from here on in, I'm going to have a go at drawing this myself. But let's start a new parts like the standard millimeters part create. Start to D sketch. I'm going to do this on the XY plane. I'm going to start at the origin with a line. Now, this will be my axes of revolution. I'm just going to draw this in here. I can put any dimension there. It doesn't need to be anything fixed, but let's put ten for now. I make that a construction line just so it's definitely not a part of any profile that I draw. Okay, and then I'll also do the distance line as well because there's a through hole in this part. So we don't want any material to be in here, so we want a distance between this and any of the profiles that we create. So let's start with the line tool and just follow the sketch from here, so 45 across. We're going vertical by five, coming across by 15, and then we've got an arc. So a shortcut to use the arc tool. Currently in the line tool. If we go back to where the line started, hold down the left mouse button, we can then bring out an arc. And we can follow that up with some dimensions. The dimension that arcs eight radius. We want to make sure that it's tangent to this line here. So if we select the line, we'll see it's already tangent with this line there. Fantastic. Then we're going to go ahead and draw that vertical line in, which is 50 mil in length. We want to make sure there's a tangency here, which there isn't. So we'll select the tangency constraint. Select the arc, select the vertical line. Then if we select that arc, we'll see the tangent constraint at the top and also at the beginning of the line. Perfect. Let's go back into the line tool and continue our sketch from the endpoint of this line. But here, we've got another arc. Let's go back to where the line started, hold down the left mouse button, add in an arc like so. Dimension that up. Give that a radius of 40. Okay? We've got that tangency constraint there with this straight line, perfect. Let's continue with the line tool. We're coming across by 40. Wanna make sure these are tangent, as well, which they're not. But let's tangency arc to line perfect. Back to the line tool. Now we're going vertical by ten, cross 15, down three, right, three. And we're going up eight. We're going across five. Then we're going down five. Then we're going across 65, going to go up four, going to go across 14. And then if we go down, we should have a vertical line going all the way back to our starting point there. Here we have the profile in which we're going to revolve. That's great. We've got our axis of revolution just here. We can see we're fully constrained, so everything's dimensioned, everything's fixed. Let's finish that sketch right there with a home view. Go on three D model, we'll select our revolve feature. Inventor selected the only profile available, which is the one that we want to revolve. We just need to tell it the axis. In this case, I'll select the axis that we drew in here, and we can see a preview of the model that's looking good. Press okay. Let's go ahead and add some hampers now. Let's go two mill chamfers. There's one chamfer on this edge here, another chamfer on this edge, both two mill, press okay. Now we need to take a look at the whole features which are surrounding the top plate here. To do this, let's begin a sketch on this plane here. Just going to go roughly to the top around this area. We're going to draw in a circle. In this case, it's 40 mil, 20 mil on the radius, but in a vertical constraint between the center point and the center point here. Okay? So now we can move our circle anywhere alongside that constraint we've just added. We know that the center point of this circle is coincident with this circle here. But we choose the coincident constraint, center point to the circle, now that's fully constrained. It cannot move anywhere. That's great. Now we need to add in this mounting hole. Is a circle tool again. Let's add in a circle anywhere. It's ten millimetres diameter. Then we use the vertical constraint between the center point of that circle and the center point of this circle. Right click, okay. Add in a dimension there then. So from here to the top of this circle is 12 millimeters. We can't quite select that quadrant, add in a line here, and also use that line to mirror, as well, some arcs. Right click on that line construction. Move that dimension. So that's dimension between the top of this line and the center point of our circle. Do that at 12 millimeters. We no longer need the remainder of this circle, so I use the trim tool to remove that we only need here two arcs, one coming off here and one coming off here. Both of these are tangential, so they'll be tangent to this arc and tangent to this circle. So use the arc tool then. Again, I'm just going to place in an arc. I'll give that the radius here, which is ten mil. Okay, not quite what we had in mind, but we can use the tangent tool to tidy that up, select this arc and this one, but that nice join there. Again, we'll select this arc and this circle, but that nice join there, and that's fully constrained. Now we can go ahead and trim away this excess material here, the trim tool. Trim away that, right click Okay. Now we need to do the same on the other side. In this case, I've got the center line, and so I'm just going to mirror this arc across. P let the mirror tool, the geometry I wish to mirror this arc, the mirror line I'll be this construction line here, okay. Trim away this material here also. There we go. Just tidy up these dimensions. At a radius on that. Now we're fully constrained. We have our mounting holes. Let's go ahead and extrude that. Really model extrude. Got two profiles to select from. We want to choose this profile here, and we want to come up to this face here. So profile selected. It's coming from the sketch plane, perfect. Going in the wrong direction. Lip that direction. Okay? We could come up by ten mil, be a bit more accurate, and I'll click two and select the face, this one. Then we'll see it will only extrude that sketch profile to this face here. Okay. Looking good. Now we just need to pattern this around. So we've got five instances. In this case, I'm going to select the circular pattern tool. I need to highlight a feature to pattern. Come to my design tree, not the Shampa or the rev going to pattern this extrusion as selected. And under the rotation axis, we can just select at this face here, and we'll take the axis of that, so we can see the axis has popped up there. Okay, so we've got six iterations there. We want to change that to five. I want to keep the angle of 360. Change up to 180. Yep, it won't cover the full of the face. Cover 360. Okay. So there we go. That's how we use the revolution command to get the vast majority of the feature there. Then following that, we've just added a few of the basic hampers, then added one of the extrusions. So this is the mounting hole, and then we've circular pattern that feature so that we've got all five of them. Change the material here, make that look slightly different, go with the carbon steel. Okay, and that's looking fairly representative, following the dimensions that were given in the sketch. So yeah, I hope that's quite straightforward. Again, any questions, any comments, please send them to me. And if you did have a go at that yourself and were able to complete that, then a big, well done. A really good use of tools there. And I will see you in the next lecture. 38. Section Introduction - Assemblies: In this section, we will learn how to create assemblies. We will start by modeling individual parts, including a cast iron bearing block base, a bearing block cap, and a structural beam, and then we will learn how to insert fasteners from Autodesk inventors Content Center. Following that, we will then create our first assembly file and learn how to add and orientate parts and then constrain them in place, forming a complete engineered assembly. Each lecturer is presented step by step where I demonstrate how we can end up with engineered assembly files. I hope that you enjoy this section. Again, if you have any questions, please don't hesitate to contact me. 39. Part 1 - Cast Body: In this section of the course, we will be working with assemblies, and we will be learning how to bring parts together to form an assembly, such as we see here. So this is the example that we're going to be working with. In the next few lectures then, we need to draw in these parts. So in this lecture, we will be drawing in the cast body. Which is this part here. In the next lecture, we'll draw in the cap sits on top. And then when we come to the assembly file, we'll add in these fastness. And we don't actually need to draw these parts. We can add them in from Autodesk Inventor's content Library. And I'll show you how to do that when we do the assembly. But for now, let's focus on modeling this cast body here. I'll start a new part when a standard millimeters create. And I'll put the dimensions of the part here. If you'd like to have a go at this yourself, by all means, please feel free to do so. But moving on, I'll be drawing this part myself, and you can follow along if you like. So there's quite a lot of geometries going on here. We'll need to do several extrusions and use quite a few other sketch tools. No problem there. Let's start with the base. Start a new sketch. Go on the Z plane, and I'm just going to rotate the view cube. See, the default is the top but rotated by 90. I'm actually going to turn back 90, this just helps us a little bit later when we come to using the vertical and horizontal constraints. We're going to be looking directly at the top face. Let's go on the rectangle tool, and we'll do this with a two point center rectangle, so we'll keep the origin in the center. We'll draw that out. We've got a wick there of 200. Let's tap on the keyboard, we've got a depth there of 46. Okay, so we could extrude that now, but I'm also going to include the two slots that we could see. I'm going to choose one of these slot tools. Now, we've got the dimension from the center point to the center point of the slot. So in that case, it's just easier to use the center to center slot tool. I draw that in roughly over here. Though the center to center distance is ten mil, then the width of the slot is 12 mil. Now we know that's in the center position. So I'm going to use the horizontal constraint, go from that center point, the origin, and then we're going to add in the dimension there. So from this center point here to this line, we have a dimension of 18 millimeters. That's one of our slots. We need to do the exact same on the other side. So we could repeat that process, but in this case, I'm just going to mirror this sketch across. Let's draw in a mirror line then. I'm on the line tool now. We're in my mirror line on a right click, make that a construction line. Come up to the pattern tools, select mirror. Going to brag across the sketch that I want to mirror, so my slot. So like the mirror line will be our center line here. Lo apply done. Now we are fully constrained, as we can see in the bottom right, and that is looking good. But we can now go ahead and finish that sketch back to the home view. Really model that's extrude. Now we need to choose which profile to select. And obviously, we're going to be choosing this profile here. As for the thickness of this base, it's 14 millimeters as per the dimension on the drawing. And at this point, I'm going to start to add a material, so it looks quite nice when we're working with it. But I choose here cast iron. Next, we need to do the extrusion in the center. So for this, we're going to sketch on this plane here and then extrude across this plane here. Let's left click this face, create sketch. Then we know the length of this is 100. So I'm going to use a midpoint line here. I'm going to start at the midpoint of this line, which I can see. I've got my green dot there. I drag that across 100. Okay. We've got our line there, and now we need to come up vertical by 54, use the normal line tool. Endpoint of this line come up by 54. Okay, then we're coming across by 100 -40, then divide that by two. So that's 20. But then coming down by 16 and coming across by six. Then we've got this arc here, which has a rad of 24 mil. So I'm in the line tool, I'm going to come back to the origin, hold down the left mouse button, and then just drag across, and I'm just going to draw an arc anywhere. Okay, let go of that. I come out of the line tool. And now I need to dimension this arc. The radius in there is 24 mil it's looking nice. We're fully constrained. So yeah, everything is constrained here. Everything's looking good. And now we need these lines over the other side. So going to suggest that we mirror those. Choose the line tool, draw our line in here and right click construction line. So like the mirror tool. Then the entities that I want to mirror are this one, this one, these guys. Choose my mirror line in the center line here. So apply done. Now we've mirrored across those parts, and we are fully constrained. Everything's fixed. That's looking really good. So at this point, we're ready to extrude this profile here, finish that two D sketch. Come into the Extrude tool. Okay? So inventor has selected the right profile. Unfortunately, it's the wrong direction. We'll flip that direction. And then we want to extrude to this face here. Okay? We could put in a dimension here. I'm just going to click two, then select this face here. Reviews looking good. Like, Okay. Here we go. That's looking nice. So there's two more things to add. Number one is the arced material, which comes around here, also on the other side here. We've also got to add in these threaded holes, M 12, thread pitch 1.75. Let's go ahead and add these arcs in first, so we'll do the sketch on this plane, create sketch. I'm just going to use the three point arc tool because we know the starting point. We know the ending point, and then we know the radius for the drawing that's 50 millimeters, enter. And we need the same on the other side. Could mirror that if you like. I'm just going to draw that in myself. 50 millimeters. Okay, yeah, that's looking good. Now we've got a profile here. I want to make sure that profile is complete. So I'm just going to project this line here. We can now see it in yellow. We can see a complete profile there and also there. Inventors also projected. These lines, which we don't need, we can leave them there, but I just delete them, keep it tidy. Hey, we've got our two profiles. Finish the sketch. And it's extrude. We need to select our profile, so we'll select profile one, profile two. Now we need the distance to come all the way to this face. So again, I'm going to extrude two. I'm going to select this face here. Looking good. Okay, there. Let's go on the home view. Now there's just one more feature to add, which are the two holes. We're going to be drawing these on this, it's the same plane, but either one of these faces we can choose, create two D sketch. Now to use the whole tool, like we've done before, we're going to add in some points, one point here, one over there. To use a horizontal constraint between that point and the origin, then with this one and the origin. And then I'm going to dimension this line here from this one as 80 mill in the drawing. I just want to make sure that they are equa spaced. So I'm going to dimension from here to here. I want that to be half of 80. So we can actually click this dimension here, so recognize that dimension. And then if we put the divide sign, then two should be 40, which it is, yeah, perfect. We can also see that we're fully constrained in the corner. We're going to finish the sketch there. Then we're going to use the whole tool. The inventors picked up our two points already. That's great. See what options we've got available to us. We want this to be a threaded hole. So yeah, tapped, in this case. We don't need a seat countersunk or counterbll. Going to go for an isometric profile. Inventors assigned 12 already, which coincidentally that's correct. Designation. So we'll go with 1.75 as per the drawing, so it's a thread pitch. Okay, direction. That's all good. Termination. We want this to be fully threaded. So we're input the entire depth of this part here, which is 54 plus 14. So that's a e. We'll click Okay. Two holes have been made. They're going through, and they are fully threaded with that M 12 by 1.75 thread. And that is our cast part. Okay, if you did that by yourselves, yet a big well done. And we're going to move on now to the next lecture, which is where we're going to be modeling the cap that sits on top of this cast part here. I'll see you very shortly. 40. Part 2 - Cap: In the previous lecture, we drew the cast body just down here. Now let's go ahead and draw in the cap. We'll start a news part, a standard millimeters create. I'll put in the dimensions here. Again, feel free to have a go at this yourself. Moving forward, I will continue to have a go at drawing this. We'll start a two D sketch. In this case, I'm going to choose the XY plane. We're going to start by drawing the geometry here and then extruding, and we'll get most of this part out of one extrusion. But first of all, I'm going to start at the origin. I'm going to start at the center point of the arc, which has a radius, in this case, of 24 mils. So I'm going to choose the arc tool, center point arc, start from the origin and bring that out to the left by the radius, which is 24. I'm going to bring that all the way around and enter 180 degrees. Hey, there we have our arc. I'm just going to use the horizontal constraint between the endpoint of this arc and the origin. Now we can see now we're fully constrained. Let's continue from the endpoint of the arc here, use the line tool, and come to the left by six mill, come up vertical 16, left 20. Then up we're going 12. Them we're coming across by a distance we can't quite tell, but we don't necessarily need to know. I'm just going to finish the line at this point, come out of the line tool, and I'm going to input another arc, a center point arc. We know that this starts at the origin, and it has a radius of 44. Rest tab on the keyboard, and then when we come to choose the angle, we're just going to snap onto this line here, rim away the remainder of that line. We'll bring that across until we see the snapping point over here. That's looking good. I want to trim away that line tool, trim away the remainder of the line there. And I just want to make sure that this point here is horizontally constrained to this point. There we go. Everything's fully constrained. Nothing's moving. Now we just need to mirror across these various lines here. While drawing, well, first of all, move some of these dimensions. There we go. I'm going to draw in a mirror line. So the top quadrant of this arc because it snaps on in green, and then exactly the same here. Right click construction line. So like the mirror tool on to mirror this entity. These guys. These guys then the mirror line, this one here, supply done. Can see we're fully constrained, and that's looking like a good profile. Let's finish the sketch there on the home view. Let's extrude this profile. I'm going to extrude. I can extrude it in any direction, prefer to extrude away. Though the length here the extrusion is 46 mill. Okay. One thing we need to do here is to add in the arc here and on the other side, and then we'll extrude that material. So easy to do. Let's go into a two D sketch. We'll select this face here. Going to use the arc tool. In this case, we'll use yet the three point arc. We know the start point, the endpoint. We also know the radius, which is 50 mil. You could mirror that across or in this case, do it manually, start to end, 50 mil. So we've got the yellow line here. That's good. We've got a full profile. Let's project this line as well. There we can see we've got that full profile or so. Let's finish that sketch. Looks extrude. Going to select this profile, and this one. Don't want to quite extrude by that much. So we'll click two. Then we'll select this face here. And the preview on both sides. We're just extruding to this face. That's looking good. So. Next up, we have some material that's been removed from this area here. We a large arc there with a rad of 20. Okay, let's go ahead and start a sketch on this face. I'm going to draw in two circles, one being 40 and the other being 40 also. Now I want to distance between these two at that's 80 millimeters between the centers and make sure that they are in the correct position. So I'm going to click from this center of the circle to the origin. Give that dimension of 80, so I'll click that dimension, divide by two, enter. I'm going to use the horizontal constraint, center point of this circle, to the center point of this line here. And now this is the material that we want to be removing. I've got a three D model. Let's go extrude. Select this profile and this profile, where we can select both of them. Fine. We don't want to add material, we want to remove, and we want to remove material in the other direction, go in the default direction. And here we'll just click through all Lo. There we've removed that material there. Last feature to add, the two holes. And before I forget, go ahead and assign a material to this. Let's go for copper. Left click on this face now. I'll start a two D sketch. We'll start a circle. Now we want the center of this circle to be concentric with the center point of this circle. So when we move the mouse over this arc, we'll see the center point pop up, we just snap onto that. And a a diameter of 12, the same on the other side. Center points popped up, 12, finish the sketch. Extrude, select those two profiles, and cut, go through all. Make a look at the preview. That's looking good. Okay. And there we go. There we have the cap. If you did that by yourself, that's great. And aside from that, we can now move on to putting parts into an assembly file and understanding how we can orientate them and form relationships between them. So I'll see you in the next lecture. 41. Part 3 - Structural Beam: In the previous two lectures, we drew the cast body and we drew the cap. In this lecture, we want to draw in an I beam, which is this part here. Then following this, we will create an assembly file where we will input for these pillow blocks on top of our structural beam. So let's go ahead and model this H beam. Let's click on a new part. We're going to a standard mill template. And here we can see the dimensions for this part, and we'll also add some fillets to that as well. So let's start a two D sketch. Choose the XY plane, use the line tool, start at the origin, come all the way across there by 200 mil. It's got a wall thickness here of five mil. Come back across 97.5 come up by 190. Then come across by 97.5 again. Then up by the wall thickness, five mil, come across the full 200, come down five, like 97.5, come down 190, cross 97.5. Then finish that with five mil, and there we have the profile that we need. Let's finish that two D sketch, go on the home view. Go to three D model. La select the Extrude tool. Inventor selected the correct profile there, that's looking good. And for this demonstration, we're just going to extrude that by 1 meter. Let's go on the home view, previews looking good. Okay. Add in those fillets. In this case, we're going to use four mill fillets. We're going to fillet the inner edges. So this one here, turning around on the other side, this one on the bottom, which is this one. And this one as well. Okay. Back to the home view again. Yeah, those fillets are looking good. Let's also add material to this, give it an appearance. In this case, let's go for carbon steel. Make sure we save that part, and we'll be using that when we come to the assembly file in the next lecture. 42. Placing & Positioning of Parts: In this lecture, we will create an assembly file and we'll begin to position our parts, and then later on we'll then constrain them and form the complete assembly. So let's head up to new. We don't need any parts, but we do need an assembly file. So we've got a range of templates available here. We're going to go with standard millimeters assembly template and click Okay. Then from here, we have a range of tabs and a range of tools available to us. Now throughout the following lectures, we won't be covering absolutely everything here, but we will be covering the fundamentals behind assemblies, and for this, we're going to start with the place. If we come up to our dropdown, we have place from the content center, which we'll be using today, place imported CAD files and logic components. This lecture will focus just on place. The according location of the parts that you've created. So I'm going to start with the cast body. I will click that file, and then you'll see that inventor has thrown in the cast body, and it's actually locked that at the origin. So the very first part that you add to an assembly file will always be locked to the origin, and then we've got the option to add more of these. So I could add, as many of these as we need. Then right click Okay, and then we're left with four of them. If you do happen to add more than you need, no worries. Te simply left click on one, delete, delete, delete. Let's go back into place. Let's place another one of these cast bodies. We'll press Okay. One thing we can do here to position this part is that we can rotate it. So where the mouse is, we see the Y axis. We see the Z axis and the X axis. If you want to rotate this in a different position, we can right click and then we can rotate it around any one of these axis. For example, if I rotate around the Y, could then place it in this position. I rotate around. Let's go for the Z. Okay? So that was vertically mounted and we could do like so and so forth. So feel free to have a play around with these and orientate these, how you like. Okay. Just going to delete these for the time being. We've got our cast body here. And if we look in the tree on the left hand side, we can see the cast body is here, and next to it is this white filled circle. Now, if that circle is filled with white, it indicates that this part is fixed and it cannot move. And we know that because if we hold down the left mouse button, we cannot move that part. We can't rotate it. We can't move it around the environment at all, so it is fixed in its place. I'm going to go up to view under visual style, and I'm going to turn on shaded with edges. I like to see edges during assemblies. I think it's better for visual purposes. Okay, so we've got one cast body now go back into place. Okay, let's find the cap. That's okay. And again, now we can rotate this any way we like. So for example, I could rotate it around the Y axis, around the z axis, and so forth. So I'm just going to left click once and add that part. And again, I've got the option to add more, but I'm just going to press escape on the keyboard. I'm quite happy with just one cast body and one cap. Now, this is completely free to move, and that's absolutely fine. We will constrain that later. But for the time being, I like to roughly move it into position. Do this, I'm going to come onto the front view on the ViewCube. Just going to move that across roughly like so. Let's take a look at that. That's looking good. Let's go on the right view, roughly move that into the correct position, come back, right, and then we're going to drop that down later on when we use constraints. Now notice that on the left side in our tree, like I said, we have a full white circle on the cast body indicating it is fixed, cannot move, but the cap is not filled with a white, and therefore we can still move that around that is not entirely fixed. We'll work on that in the next lecture. But that is how we add the parts that we've drawn, and that's how we can rotate them and roughly move them into position using the ViewCube and holding down the left mouse button. 43. Constraining Parts togethor: Now that we've added in the cast body and the cap, let's go ahead and add the final part, just the structural beam, and then we'll start using constraints to fix everything into position. So let's go up to place and find the location of the H beam. Okay, I'll open up that structural beam there. And again, we can just position this anywhere for the time being. We only need one of them, so we'll right click Okay, to leave that. That's in the correct rotation, at least anyway. I'm going to use the ViewCube to position that a bit more accurately to where it's supposed to be. There's something like this on the right view. Move that roughly in position there. That's looking good. Now, we know that the cast body here, this cast body is fixed at the origin. Only the cap and the structural beam are able to move. We need to put these into position and make sure they are fixed. And to do that, we use what's called constrains. But if we come up to the top, we've been using place so far, what's got joint and constrain. This is what we're going to be focusing on in this lecture. So let's select constrain. We have a toolbox pop up here. First of all, let's work with a structural beam and constrain this to the cast body. So one of the constraints we want to have is we want for this face here to be flush with this face here. But if we come up into our toolbox under the assembly tab, we need to define the type of constrain that we're doing. So we've got the mate options there, angles, got tangent, insert and geometry. So for this, we're going to be using the mate option. Okay? We've got here an option to offset as well, but we don't want any offset between these two faces being flush. Okay? We then need to make our selections. So selection number one in blue. I'm going to choose this face here, and then selection number two in green. I'm going to choose this face here. Now, if you notice, that's not what we're looking for. That is a mate constraint, but we want to be going for the flush constraints. So under the solution, we've got mate, so where the faces in contact with one another, and then we've got the flush option here, which is when the faces are flush with one another. So we'll click Apply there. Okay? We know that this structural beam is still able to move. And if we bring it down here, we can see these two faces are now flush, and that is a locked constraint. That's good, but we're still able to give this a lot of movement. Let's make a few changes there. We can do is make these two faces flush as well. The same process, select constrain. I'm going to select my solution here to be flush. Select my first face, and then the second one. Click Okay. Now, if we look from the side, we look from the side, we'll see that is flush, also these two faces here are flush as well. Looking nice. But we've still got this movement just in the one axis there. That's the y axis. So we want to prevent that from happening. So what we want here is a mate constraint between this face and this face here that will put them in contact. Let's come under constraint. Make sure we have mate selected. Select our first face and our second face. Okay. Now we can see that's looking good. We're flush here, these two faces. We're flush on these two faces, and we have a mate constraint between this face and the underside of the cast body. Now, if we look on the left hand side at the tree, we can see that our H beam part now has a white filled circle. And again, just like the cast body, that means it's completely fixed. We cannot move that at all. Okay, so that's good. Those two parts are now fixed in position. Need to constrain the cap. So again, we'll use the constraint tool. There are various ways in which we can do this, but I'll show you quite a simple one. I'm going to use the mate constraint once again. Okay. And under my first selection, I'm actually going to choose the axis of this hole here. So when we come into contact with the cylinder, we see the axis appear. So we'll select that once, and we're going to constrain that with the axis of this hole. So that will make these two holes concentric. Let's zoom in, and then we can see the axis of this hole, left click. Press okay, and let's see where we are. If I hold down the left mouse button, I can still move this part. Okay, but I can see that these two holes here are constrained. As we've achieved what we wanted there, that's great. Let's do the same then for the other two holes, this side. Go and constrain. Then we'll se like that circles axis, and this circles axis, press okay. There we go. That's looking nice. We can see both of those holes there, they're both concentric with the according holes in the cast body. Now we've only got this one piece of movement which we need to prevent here, so we want the cap to be sitting in position here. To do this, let's constrain. Let's choose a mate constraint. Go from this face. Let's select this face here. Okay. Go on to the home view. There we go. That's looking quite nice. And then if we look on the left hand side, we see that the cap now has a white filled circle indicating that it is fixed. And as I'm holding down the left mouse button now, I cannot move any one of these parts. They are all constrained in position. That's looking good. So in the next lecture, we will place some more parts, but we're going to place these from the content center. So these will be the fasteners that go into these two holes, and then following that, we'll take a look at patterning this assembly here across the rest of our eye beam. I'll see you in the next lecture. 44. Adding Parts from Content Library: In the last lecture, we added the H beam, and we also then constrained all these three parts together, and all of them are fixed and are in the according position. And we know that because in the design tree on the left hand side, we see that each part here, the cast body, the cap, and the H beam, all have the filled white circles next to them, so everything is fully constrained. Now, in this lecture, we're going to be adding some parts, so some fasteners, in this case, from the content library. So we're going to come up to the place, click on the dropdown, and then we're going to select place from content Center or content library. So this is a content center or library from Autodesk Inventor, and it has an absolute myriad of tools available here. Now, some of the parts we want to add in this example are fastness. We click on fastness. We then got the option here for bolts, nuts, pins, rivets, washers. We're going to go in this case, for a bolt, and then we need to define the type of bolt that we're after. So we're going to ask inventor in this case, for a hex head bolt. And under here, we've got a myriad of bolts, all according to particular standards and so forth. In this case, we're just going to stick the very first one, AS 210 to metric. Select, Okay. And then if we move the mouse, we'll have to zoom in. We can see this very small looking fastener. So that's obviously not what we need here. We need a 12 mill bolt, and it needs to be 1.75 pitch thread. So what we're going to do is we're going to right click change the size. So here we're going to select 12, and then under the nominal length, we'll go in this case for 60. Okay, we'll press Apply. Then if we see we've got this 12 bolt. Now, I'm going to rotate this roughly so it's in the correct position. I'm going to right click therefore. Now I'm going to rotate this around the Z axis. Okay, that's the wrong orientation. So let's rotate that around the z two more times. Then we see it's in the correct location. I'm just going to add one here. Then I'll add one over here. Right click. Okay. Now these fasteners. Now these fasteners are roughly in position. Let's go on the front view then. Let's roughly position these, bring these guys up here. Then rotate the view cube on the right view and put them in about these positions here, come back to the home view, we can see they're almost in the correct location. And from here, we're just going to use constraints like we did in the previous lecture. To use the constrain option. We're going to first of all, select the axis of this bolt, left click. Then we're going to make that with the axis of this hole here. Looking nice, let's click Apply. See where we are. Okay, yeah, nicely constrained there. Add one more constraint, which will be this face here. It's left click. It's gonna be a mate constraint to this face here. Like okay. Looking nice, okay? Still got some movement in the movement there is rotational. We're going to fix that a bit later. Let's repeat the process then for this fastener, Constrained, axis to axis. Then I'm going to stay in the constrained tool, face to face mate. Look, go on the home view. We've got our two fasteners there, but both of them are still not fully constrained. We know that because if we look on the design tree, we can see that that circle is not filled with a white color. So to do this, let's use the constraint or once again, but in this case, we're going to use the angle constraint. Though slightly different here, we need to select our solution. We have a directed angle, undirected, explicit reference vector, which I very rarely use. Typically, you just use the directed angle. Very straightforward. You need to make two selections. But here I need to make an angle between a face and another face. I'm going to select this face here and this face angle, I'm going to leave that at zero degrees. Click apply and then if we look at this fastener here in our design tree, we have the white circle, and it cannot rotate. Holding down my left mouse button, I cannot move this. I cannot rotate it. That's fully constrained in position. Unlike the other one, which we can still rotate, no problem. We're going again do the exact same process. So we'll go an angle directed, choose any face. Let's go for this one, and let's choose this face here. The angle zero. Okay. We zoom out. You can see we have white circles of every single one of our parts. They are all fully constrained and fixed in position. Well, that's looking good. So in the next lecture, the only thing we need to do is to pattern our assembly here across this eye beam. I'll see you in the next lecture. 45. Pattern Assemblies: So far, we've added in our recording parts to the assembly. We've constrained them, and we've also added in fasteners from the Autodesk content center. Now, the last thing we need to do by change to this assembly here is just to pattern across three more of our pillow blocks. Well, let's go back to our assembly. To do this, we're going to come up to the pattern tools. Got the options to pattern, which is what we'll select today, can also mirror and also copy components as well. In this case, we're going to choose the pattern component. So we've got three tabs here. We've got the associative, rectangular and circular. Now for this, we're going to go for a rectangular pattern. So that's just essentially patterning linearly instead of circular. So first of all, we need to select our component, make sure that's highlighted in blue. Then we're going to come across, and we can either select the parts from the environment itself or we can come over to our design tree. We can select the cast body. We also want the cap. We don't need to pattern the H beam. We only need one of those. We do want to pattern the two fasteners as well. We have all four of those parts selected. Then we need to choose a column. So this is the linear direction in which we're going to rectangular pattern. So let's select the column direction. And from here, we need to choose an edge. So if I select this edge here, we see this red arrow pointing in this direction. You can see this red arrow pointing in this direction off this edge, and this is the correct orientation that we want to pattern these parts. However, just for an example, I'm going to choose this edge here. I'm just going to increase my pattern distance. Let me just do that by 100. And we can see that's patterning in the wrong orientation, which is in accordance with the direction of that arrow. No issues at all. We can just flip the direction, and now we're patterning in the correct direction. So my length of this eye beam is 1,000 millimeters, so 1 meter. I know the width of our pillow block is 46 millimeters. So if we do 1,000 -46, then we're going to divide by the number of additional components we're going to add, which is three, we come up with 318. And in terms of how many instances that we want, we want to have an additional three. That would be four in total, starting with the one and adding on three, and going by 318 mill, we can accurately position the last one in the correct position so that these two faces here are flush. If I change that, let's go over 300. We'll see that it falls short so just a bit of simple mass, and we can end up with the correct number of pillow blocks that we want, and we're patterning them at the correct distance. Will we click Okay there? Now if we look in the design tree, we can see that we have a component pattern. And if we open this up, we've got element one, which is the original. If we open that up, we've got all four of our parts there so we can go back and edit any one of these. Element two. So that's this block here, element three, and then element four. If we want to remove the pattern, we can just right click and select Delete, and then we're left just back at what we had to start with, okay? And if we control Z, and then bring back that pattern, like so. Yeah, I hope that makes sense. Yeah, any questions, please post them in the comment section. And aside from that, I'll see you in the next lecture. 46. Cross Section Views: So in this lecture, we will learn how to use cross sectional views. So right here we have our complete assembly that's looking good. And if we want to apply a cross sectional view, perhaps we want to see a bit more detail. Then we can come up to the tabs at the top. We'll come under the view tab, then come down to visibility. We'll see we've got a drop down here with some options for section views. So we've got the quarter section view, the three quarter section view, and the half section view. The quarter and the three quarter, I very rarely use those. Very rarely even see those being used. The half section view is very common, especially when an assembly is quite complex. Perhaps we want to see some more detail in certain areas. So let's come under the half section view. Left click that once. What we need to do now is to define the plane or the face that we're going to section from. So I have a demonstration, I'm just going to select this face here. Then you'll see an arrow pops up. We've got a toolbox, as well. So we'll put the toolbox to the side, but for now, let's focus on this arrow. If we hold down the left mouse button and then move the mouse cursor into the part, you'll see we're creating our sectional view there. So we're able to see all that detail that we wouldn't otherwise see if we didn't have the cross sectional view. We've also got the option to more accurately position the section view, so we can use this box here. We know that the width of this Hbam is 200 mil. So if I enter -100, we'll go to the exact center of this Hbam. Then if we click Okay, we can then pan around and see any details that are now more visible than what were before. If we want to exit the section view, come back up to the drop down, and we're just going to select delete section view, and then we're back to the full assembly. Another thing I like to show you as well under the half section view. So if we select that again, I'm going to select this face here. I'm going to use the toolbox and enter in -100 again. And then if we select Rotate, we can then actually use these points to rotate the section view. So just using these points. And we click, Okay, there, we've got quite a unique section view there. But yeah, I hope that demonstrates the concept of section views. And again, if we come up to the drop down, select delete section view back to the full assembly again. I hope that's all clear, and I'll see you in the next lecture. 47. Visibility & Transparency: In this lecture, we'll take a look at visibility and transparency. These are two really useful tools when we're working with assemblies. So to demonstrate this, I'm going to work on this cap here. So if we come into our design tree, we've got our H beam, and we've got our component pattern. If we open that up, we've got the four elements there. Element one is this small assembly here that we patterned, element two, three here, and then four. So if we open up element two, we see each of the individual parts here. So we've got the two fasteners, the cap, and we've got the cast body. I want to demonstrate visibility options on the cap. So if we right click on the part in the design tree, we've got a whole range of options available to us. So we can actually edit that part directly in the assembly, which is a useful tool. We could open the part file up. We can isolate that part, for example, O. Breast control z. And if we scroll further down, we'll see two options here. One is visibility and one's transparency. So visibility has the shortcut V on the keyboard, and then transparency has the shortcut T. Right now, the visibility, as we can see is turned on. If we turn that off, you can then see it's no longer visible. We right click V on the keyboard, we'll come back. A if we right click and then hit T on the keyboard, so change its transparency. You can then see that that cap has become transparent, and we've got a better view there, in this case, of the fastness. I come back to the home view. I want to turn the transparency off, right click on that part, down, it the transparency there, or hit T on the keyboard, so that's how we change our parts visibility or transparency, and I'll see you in the next lecture. 48. Editing Existing Assemblies: In this lecture, we will look at how to edit assemblies. So far we've made plenty of constraints. Let's look at how we can change them if we need to. So to make this a bit easier, I'm going to delete our pattern that we did. Instead, we've just got a list here in the design tree of our individual parts that we began with. Let's take a look at the let's go with the structural beam then, so the H beam. We want to edit any of the constraints about this, we can select the plus next to it, and then we can see it's model states, which we won't be covering in this course. We can see the origin, okay? So relating to the Hbam we can see where the Y Z plane is, the X Z, and the X Y. We can also see the three axes as well, X Y and Z, can also see where the origin is from this original part file. Then we have these three items below, which are the constraints that we applied. If we select, let's say, flash one, we can see a blue face and a green face. These were the two faces that were constrained together as a flash constraint. See what flash two is? That was the blue and the green face here. These two faces being flush, and then we made a mate between the top, the top face. So in this case, it's green and the blue face, which we can't quite see here, but it's the bottom of the cast part. Now if we want to edit those or remove them, we can just simply right click and select Delete. That'd be deleting that constraint, therefore, we can then move that part once again. Press Controls Ed. We can also edit that constraint as well. So we've got delete, and we can then edit that. We go back into our options menu here and make any changes. We can make that offset, let's say 15 millimeters plus okay. Now we've got that 15 mil offset. And we can do that for any one of the other parts as well. So if we come into the fasteners, in this goes this fastener here, we've got the three according mates there. So the concentric mate, the face to face mate, and then the angular mate with this face here at zero degrees. We can also choose to suppress a mate. If I right click flush one of the H beam and suppress that, then temporarily, that constraint will be suppressed. But as soon as we click that once again, okay, there would then be an action. And so, yeah, please do use those tools in the design tree. You can see our constraints. We can edit or delete them, and so forth from there. I'll see you in the next lecture. 49. Section Introduction - 2D Engineering Drawings: In this section, we will learn how to create two D engineering drawings using a broad range of tools to convey detailed information such as geometries, dimensions, and tolerances. These drawing blueprints can be used to communicate design details to production teams and clients. We'll start by taking a look at templates and customizing two D drawings, followed by view types, angle projections, view styles, and labels, dimensions and style modifications. We'll also take a look at adding parts lists and customizing title blocks as well. These are all the essential elements to building two D drawings. Finally, I will demonstrate a complete two D engineering drawing for the bearing Mount assembly that we created in the previous section. Each lecture is presented step by step, so I'll walk you through how we can utilize the drawing tools for professional communication. To D engineering drawings are critical for prototyping and production, and after the following lectures, you will be able to create customized professional TD engineering drawings. I hope that you enjoy this session. Again, if you have any questions, please don't hesitate to contact me. I'll see you in the next lecture. 50. Adding Sheet & Customising Them: In this lecture, we'll move on to two D engineering drawings. So we'll take a look at templates, first of all, then we'll look at how to add sheets to a drawing and how to customize them. So right now, I'm on the home screen. If we come over to new Okay, so we don't need a new part or a new assembly, but we do need a new drawing. So there are many default templates available here. I do have a lecture in this section on how to create your own custom two D drawing template. So do check that out, I'll give you a lot more detail there. But for the purposes of this lecture, we're going to go ahead and select the ISO dot DWG. Now, there's also at IDW, ISO file as well. Key difference between these, at DWG is more cross compatible with other Autodesk softwares, such as Fusion 360 or AutoCad, and I generally always go with the dot DWG templates. So let's choose ISO, click Create. And now we're coming over to the two D engineering drawing. So this we have here is one sheet. Now, if we come over to the model tree, we'll see we've only got one sheet here. We can choose to add more sheets by right clicking, selecting new sheet. Okay? So if I add another two, we've then got a total of three sheets. Another one in white here is highlighted. This is the one they're currently looking at. If we want to change, we'll double click on another sheet. Now on sheet one, sheet two, and sheet three. So how can we customize these? What we can do is to right click on them and then click Edit Sheet. So here we can give it a name, for example, this would typically be an assembly drawing. We can customize the size, I typically draw in A three, but by all means, feel free to change the size as you need. In terms of the orientation, we can change between a portrait sheet. If I click? Okay, there, we've got that A three portrait sheet. Just go back to landscape. And we've also got the option there to change where the title block is. The title block is this element down here. Now, that's currently in the bottom right corner. We can move that top left, top right, top left, and the bottom left. I normally have it in the bottom right, so I'll keep it like that. That's okay. You see we've got this border here, so we've got six zones by four zones. Now we can edit that by coming into drawing resources. If we come under the borders folder, open that up, we've then got the default border, which is what we're looking at here. If we right click on that, we can insert a new drawing border, and press yes to this, so it's essentially replacing this current border we're looking at. And then we can define the number of zones. So if I change the number of horizontal zones, let's just double that. Let's go 12 in vertical zones. Again, let's just double that. Let's go eight. And then we have the option to define if they're so A, B, CD, et cetera, or numeric or none, for both the horizontal and the vertical. So I've changed to 12 and eight. Let's see what happens when I click Okay, there we have the 12 zones at the top and the eight zones on the vertical there. So that's the basics for adding sheets and then customizing them. And in the next couple of lectures, we'll be taking a look at how to add our models. I'll also include the lecture specifically on how to customize and modify and create your own title block. 51. Base Views, Projected Views & Section Views: So now we are in our two D drawing environment. And in this lecture, we're going to focus on adding a base view, how to add projected views from the base view. Also, we're going to take a look at section views and detail views as well. So let's go ahead and add a base view. If we come up to the top where the tabs are under place views, we've got the option there to add a base view. So let's select that. As we can see here, inventor has automatically selected the assembly that we worked on in the previous section. And that's because I've actually got that part open, which is just down here. Okay? But if you want to show a base view of an existing part or assembly and you haven't got it open, there's no problem. We can just open an existing file, this option here, select its according place, and then if we just select Okay after that, it will appear. Now, we've got a few options here that we can change. We're going to visit these in a later lecture, but for now, let's just click Okay, let's have our base view. We can move this around the sheet, so if we hover over the view, make sure the border is visible, hop down the left mouse button, and we can move it like so. I'm going to place that here for now. So that's how we had a base view. It's very straightforward. And now we're going to move on to the projected views. So a projected view is a view that has been projected from an existing view. So if we come up to our place views again, we'll go on projected view. We then need to select the view to project from. So in this case, in this example, I use the base view. And as we move the mouse around the base view, we can see all these different projections. So a top view, got an IO view, side view, bottom view, and so forth. Let's go ahead and add a side view. I think that's quite important to identify where those bearings sit on this H beam. Once we're happy with the position, left click once. And then we're still in the projected mode, so you can go ahead and add in any other views you want. You want to add an IO or a top view. When you're finished adding your views, just right click and select Create, and there we have our side view. Now, again, we can move this. So if we hover over it, hold down the left mouse button, we can only move it side to side. We cannot move it up and down. And that's because there's a fixed alignment, this existing relationship between the base view and the side view. It's very rare to break that alignment, but if you do need to do so, we just double left click on the side view, come up to the display options, then we untick align to base. Okay. Then if I hold down the left mouse button, you see I can move this anywhere on the page. Going to press Control Z because it's quite important to have that alignment between the two when we're showing the side view and relationships between the base and the side view. So that's how we had the projected views. It's nice and simple. And now we're going to take a look at section views. So again, we come up to place views. If we select the section view, I'm going to add in a section of this part here, which isn't really necessary, but for the purposes of this lecture, I'm going to use this view. So first of all, we need to select a view to do a section view from. I'm going to choos a side view, left click once. And now my cursor has changed to a cross and then I need to identify the start of my section view, so we can see we can actually select midpoints, endpoints of lines and so forth. So for this example, I'm going to hover over the midpoint of this line here and I'm going to extend my mouse out. We can see we've got that alignment there to the center point of the line. I'm going to show you why I'm doing this after or left click once, and now I need to select the end of my section view. So in this case, I want the end to be in alignment with the midpoint of this line. I'm also going to track that out left click once. Now we've got the option if we want to add any more sort of angles to change that section view. But in this case, if we don't want to, we're going to right click and select Continue. Now, if we hover above our section view line, we're looking up essentially from where we drew that line. If we bring the mouse down below the line, we're then looking down, essentially. Now, we wouldn't do this for the assembly, but just for pups of demonstration known to LefClickOce here, and then we can see our section view. So from this line here, which is labeled A A, we're then looking up. And you can see why we started the section line away from this line here because we don't want any of this detail of the section line or labeling to be conflicting with our existing entities of the side view. That's the basics of how to show a section view. We would only do these where detail is necessary, such as some detail being hidden within an assembly or a part in which we can only see it by doing a section view. And the last tool I want to show you in this lecture is the detail view. And again, for this assembly, it's not necessary, but let's go ahead and demonstrate that by selecting the detail tool here. We need to select the view. So in this case, I'm going to select the base view. And then if we zoom in, which in this case, I'm going to choose the center of this circle, and I'm going to draw out a circle. And then when I'm happy with that, I'm going to left click once. You'll see there we've got this preview, left click again, and there we have our detail view. So it's labeled as view B, and then we've got the view B up here. So that is the basics of how to add a base view, how to add projected views, section views, and detail views. And then the next lecture, we'll be looking at how to switch between first and third angle projections. So I'll see you there. 52. Switch Between 1st & 3rd Angle Projections: In this lecture, we will learn how to switch between first and third angle projections. So to demonstrate this, I'm going to add in a base view. So come under my place views, select base. And I'm going to go ahead with the assembly that we did in the previous lecture. I'm going to select Okay, move that just down to the left. And now I'm going to add in a projected view of this, which will be an IOview. So I'll select the projected view and select my base view, and then I'm going to project the ISO view like so. So I'll left click once, then I'm going to right click. Select Create. There we have our ISO view here. Now, we can tell that this is in first angle projection. So if we want to switch to third angle, I'm just going to select both of these views, press delete on the keyboard, confirm that. And then I'm going to come up to manage, and we need to go under the styles editor. So we have a lot of options here to edit different styles. We're going to be covering the core of these throughout the remainder of this course. But for the purposes of first to third angle, we're going to come under standard, come under our default standard ISO. We're going to come under view preferences. And then just in the bottom near the center, we've got the projection type. We've got first angle and third angle. Currently, first angle is highlighted. In this case, I'm going to switch to third angle. So that's now highlighted. Click Save and Close. For as many sheets as I have on this drawing, they will always show the third angle projection. Let's go back to place views. Let's add in that base view again. Let's select Okay. Move that view down there. Go to the projected view, and then I'll put in my ISO view there, right click Create, and there we can see we're now working in third angle projection. And you can switch between those vice versa using the same method. So for the remainder of this course, I will be working in third angle projection, but please use the according angle projection as per what's required by your client or your lecturer and so forth. And then the next lecture, we'll be taking a look at view styles, labels, and leaders. I'll see you there. 53. View Styles, Labels & Leaders: In this lecture, we will learn how to modify view styles and labels. So to demonstrate this, I will input a base view of the assembly we've been working on so far, and I'll click Okay. I'm also going to add in a projected view. So let's add in a side view there. I'll click Projected. Select My view, then move the mouse to the side. Left click once, right click Create, and there we have a base view and a side view. Now, I want to reduce the size of these because they're a bit too big for the sheet size. So to do this, I'll double left click on the border of my base view, I'll take the scale down. So let's make that one to five. Okay. Now we can see the base view. It's a scale of one to five, and so is the side view. And that's because there is a relationship between these two in terms of scale. Now, it's very rare that you would want a projection to be of a different scale. But if you ever do need to do that, I'll show you how. So if we want the scale of the side view to be different, again, double left click. Now we see that the scale is grade out. We're unable to modify that. That's because that relationship is in place between the two views. Now we can remove that relationship. But if we untok this box, we've then got the option to change the scale. So if I say this is one to eight as an exaggeration, click Okay. We can now see the difference in the scales. So I'm going to put that back to scale from base, that will put it back to one to five, keep those two views the same scale. Now for the front view, we can add a label to identify that. So now if we go under label, so just above scale and the view identifier, let's type in front view. And then we just need to make sure that this light bulb is on. So if we left click once, light bulb on, it shows the visibility. Press Okay. Now we've got this label above. We hold down the left mouse button. We can position that wherever we like. So I typically have it underneath the model. It's looking good. So we'll see it now says front view, which is the view identifier, and then it's got the scale in brackets. We can modify this how we need by double left clicking, and then we can add any text in here or any properties. So we've got the scale in there, which we don't really need, so I'm going to remove that. Click Okay. And now I see that we've just got the view identifier in there, reposition there. Now the reason I took the scale out is because in a later lecture, when we take a look at how to customize the title block, I will show you how to input the scale in the title block, and it will automatically detect what the scale is of your models. So it's referenced in this title block here, so we don't need to repeat that information. Let's go ahead and do the same for the side view, then that will left click identifier. Let's go sideview. Then the light bulb on. Press Okay, reposition that. And again, I'm just going to remove the scale there. That's looking good. I'm just going to move these down a bit. Another option that we've got if we double click on our views is the styles at the top here. But to demonstrate this, I'm going to input another projection of the base view, select projected, select the base view. I'm going to project the IoviewR click Create. Put this over in the corner. Now this is far too large. So I'm going to double click on this. I'll input a scale. Let's go for one to eight. I'll also input identifier. Let's go Ioview, turn that on. We can also edit the label using this button here. We click that go to remove the scale. Okay. Press o again. And there, that's a much more suitable size, and I'm just going to move the label to a more appropriate position like so. Now, if we double click on the IO view, again, we've got these style options. So I think it's best to demonstrate on this view here. The very first style we have is hidden lines. But the opposite of that here, which is hidden lines removed. So if we select hidden line and then press Okay, all of the hidden lines will be shown. We can see here the slots are going through. We can see here the underside of the H beam and so forth. Now for this assembly, it's quite straightforward, so it's not really necessary to have the hidden lines. So for this particular assembly, I'll put the hidden lines as removed. One more style I'd like to show you is the shaded option. So if we select shaded and then click Okay, we can now see that the appearance, as per the appearance and material that we assigned when we drew the individual parts is now shown. And this, for me, I think, just helps better communicate with a lien or anybody in production, manufacture each individual part there. But not strictly necessary, but I tend to do it in most of my models. And so that is a summary of how to use the view styles and how to add labels. I hope that all makes sense, and I will see you in the next lecture where we will be adding dimensions and style modifications. I'll see you there. 54. Adding Dimensions & Style Modifications: In this lecture, we'll learn how to add basic dimensions and do some style modifications. So I'm going to go ahead and add a base view again, and I'm going to also add a side view. There is a quick way of doing this, by the way. So instead of coming up to projected view, what we can do is just double click on the base view, then we can click these arrows to the side here. So that will give us a side view. So it will give us a top view, the other side, bottom view. We can add the ISO view other views like so, you click Okay. We've got all of those views, which as a bit too much going to control Z those that we don't need. Put these into a better position, and I'm going to modify the scale again. Double left click, change that scale. Let's go one to five. Now for this assembly drawing, it's essential that we identify where each of these bearing blocks are in relation to the H beam. So to do this, we need to use the dimension tool. So if we come up to our tabs, come under annotate. We have the dimension tool here and a series of other dimension tools. Now, the key dimension tool is the most commonly used one, but we're also take a look at baseline as well. Let's select the dimension tool very straightforward. If we want to identify the position of this bearing block to the start of the H beam, we can just left click once at the start of the beam. And then if we come across and left like start of the bearing block, we'll see a dimension appear. So that relationship between these two lines, we can left click once again and input that dimension there. Do the same for the third bearing block, also the fourth. So we're still in the dimension tool. Left click once again on the end of the H beam, Camacross, left click on the third block. But that interposition do exactly the same process there for the fourth block, that interposition there. Believe the dimension tool, we can right click and select Okay. Now, that's a bit of a long winded way of doing it. I show you a bit of a shortcut. So if I left click once and delete these, the best tool or most appropriate at least to use here is the baseline tool. So by means of a baseline, we select where the baseline is. So we're going to reference this entity here, and then we can select as many other entities as we want. For example, choose our three starts of the bearing blocks. Right click, press Continue, and then we see each of these are referenced from the baseline that we chose here. I'll input those dimensions there. Good. Right click Done. So now the team in assembly will understand the exact position of each of these bearing blocks. So these dimensions here, 318, 636 and 954, each one of them is using a comma as the decimal marker, and they're followed by two decimal places. We can edit these by coming into manage, and then we're going to go under the styles editor again. Now when our box pops up, we're going to come down to the dimension here. Click the plus and then come down to the default Iodimensions. And in here, we can modify the units. So the units here, going to leave those as millimeters. Under the decimal marker, I want to change those from a comma to a period. And then under the linear units, we've got the option to change the precision. So right now we've got two decimal places. Let's change that. In this case, let's just change them to one. Click Save and Close. Now we can see that our decimal marker is a period and that we've only got one decimal place per each dimension. And that will be apparent on as many sheets as we add in here. So no need to repeat the process later on. I'd like to show you as well, about the whole dimension tool. For this, I'm going to right click in my tree, and I'm going to add a new sheet, then I'm going to input a base view. But in this case, instead of the assembly, I'm going to demonstrate using the cast body. Make that a bit bigger in scale. Let's go one to one. Let's also add a top view there. This will be the view that we'll work on for this demonstration. So this is an example in the base view here of where the hidden lines are actually quite useful. You know, it tells us that these holes are through, and also tells us that these slots are through, as well. The one more tool I like to show you is the hole and thread dimension annotation. So to do this, I'm going to select our threaded holes here. So I'll left click on that circle. Then we can bring that out. Let's just say here. And now inventor has picked up that this is a threaded hole. That's got an M 12 by thread pitch 1.7 5-6 H. That's very useful when it comes to threaded holes. An inventor will just pick up that information instead of us having to manually input that later. And there are a few other dimension annotations that we're going to take a look at throughout this course. Be covering those in a lecture later. So those are the basics of how to use the dimension tools and how to modify styles so that we can change the decimal period and the number of decimal points. And in the next lecture, we'll be taking a look at how to add a parts list to an assembly sheet and also how to add balloons, as well. So I'll see you there. 55. Adding Tolerances: In the previous lecture, we learn how to add dimensions, and in this lecture, we'll learn how to add tolerances. So to demonstrate this, I'm going to input a base view, and I'm going to go ahead and select the cast body. So if you haven't got this part open, like I've got it here, then make sure to open an existing file and locate the according part. Change the scale of this so it's a bit larger, easier to see. Let's go one to one. Let's also turn off the hidden lines. So we'll go hidden lines removed, go okay. Now, let's go ahead and add in a dimension, and then we'll add in a tolerance to that. So again, under the tabs, let's select annotate, come under dimension. And let's dimension the width of this part. So 200 mil. Now, this could be considered to be a bit of a critical dimension in that we don't want the width of our bearing block to be wider than the eight inch eye beam. So eight inch, 200 mil. If we have our 200 mil as a maximum, and perhaps we could deviate slightly lower than that. That's in but a tolerance, then. So let's double click on the dimension. Then we have our toolbox pop up. Okay, so B and text come under precision and tolerance. And here, we've got the option to add different tolerance methods. So, for example, quite a common one to use is symmetric. We could put a symmetric tolerance on that for steel. Let's go 0.2. If we click Okay, we'll then see that we've got the dimension, so 200 mil and it can tolerate plus or -0.2. So I could go to 200.2 or to 199.8. However, we don't want this dimension to be over 200 mil, so we want that under eight inch to ensure that it sits nicely on the H beam. But let's see what other tolerance types we've got. One I would tend to use here is deviation. Okay? So here we input an upper tolerance and a lower. So we don't want this to be larger than 200, so let's put in a tolerance of zero. And for the lower, yeah, we could tolerate let's go 40.3. We click Okay. We can then see there we've got the dimension. We can tolerate no more, so we cannot go higher than 200, but we can deviate down to 199.7 mill. Other options exist here and feel free to have a play around with these. So we can put in limits stacked. So in here, we literally show the higher value, so the upper tolerance and the lower tolerance. It's got linear, as well, which are very rarely see this one. Now, we can put a max, and here we're not stating a minimum. So in this particular case, the manufacturers would refer to a general tolerance. So we can add in one of these as an example by adding in some text. Okay, let's put that up here. Title that notes. Let's put in a general linear tolerance. I'm going to use one of these symbols. Let's use the plus and minus symbol. Let's go not 0.2, and let's put a angular tolerance. Let's go two, and then we want another symbol, which is our degrees symbol. It's okay. So what we're conveying in this drawing is that the general linear tolerance is plus or -0.2, which is applicable in this case, because this is a linear tolerance. However, we've then overrided that by stating that 200 is a maximum, and so a minimum, in this case, would be 199.8. We've also got the option as well to add in a minimum can state, yeah, 200 minimum, which in this case, we wouldn't want to do, but just as another option there. So feel free to have a play around with these most common ones that I use, at least anyway, deviation and symmetric, as well, if that deviates from a general linear tolerance or a general angular tolerance. I hope that all makes sense. And again, any questions, please send them to me. But aside from that, I will see you in the next lecture. 56. Adding Parts Lists & Ballons: In this lecture, we will learn how to add a parts list and also balloons. Though, as we can see here, I've input three views, so we've got the base view, a side view, and an IO view. They'll have labels. I'm referencing here a scale for this particular view. We've also got the dimensions in place as well. So it's quite critical here that we add in a parts list to identify every part that's in this assembly. So to do this, let's come up to the top under the tab annotate. And if we come all the way across under tables, we can add in a parts list. Let's left click on this one. And here we've got our toolbox where we need to select a view. So in this case, I'm going to select the base view, okay? So that's just a reference to the assembly itself. Leave everything else as the default, select Okay. Then we've got this parts list. Here, I'm just going to place that up here for now. Got a whole series of information here. So we've got the item number, so one, two, three, four. The quantity of the according item, it's reference part number and also description. I'm going to make this a bit more tidy by dragging out the edge of the box there. It's likely that in your case, you won't have any information under part number and description. But we'll take a look at how we do that now. Drag in this side of the box, like so. So if we want to add a part number for each of these parts, so we've got the H beam here, the pillow block, body, the bearing cap, and then the bolts, let's go into the bearing block body. So to do this, we can just quickly double click the description here, it will jump straight into the part itself. Now to add a part number and description, we're going to come up to file. Going to come down to I properties. Then here we can come under the tabs project and status. Let's go into project first. Here we can add a part number. So if I change this, let's go one, two, three, four, five, six, I'll leave the description as the same. Click Apply close. And if we come back into our two D drawing, we can then see we've got the addition of one, two, three, four, five, six on that particular part. So you can edit the part number there, and also the description. Let's go back into You can also add in additional properties as well, stock numbers, project engineer, authority, et cetera, come under status, who was checked by the checked date. We'll be coming back to this when we attend the lecture on how to customize the title block. Okay? But in terms of part number and description, we've covered those, and then also want to just quickly reference material. We've added in a material here, so cast iron and an appearance, which is great iron. Now let's say that we want to show the material. We come up to parts list and double click. A toolbox pops up. Then we can select the first icon here, which is a column chooser. If we select that, we've got another toolbox popping up. If we scroll down, we select material, like add, like, Okay, apply, Okay. Drag that out. Now we can see that we're showing the materials. So you can add as much information as you want under your parts list. But for this particular assembly, I think the information shown here is adequate. I'm going to hold down the left mouse button, and I'm going to dock that, so we'll snap into the corner like so. I'll dock that there. So in our parts list, we're identifying the four individual parts, the according properties related information. But we're not actually showing where these parts are in our views. And to do this, we need to add in balloons. So again, under the tab anoty, come all the way across to balloons, it's a shortcut B on the keyboard. Select that and then we can start with item number one, which is the H beam. We're just going to click once on that part. Going to drag out the balloon, left click again, and right click, continue. Now we're identifying item number one. Item number two is the pillow block or the bearing block. Left click there. Number two, right click, continue. Item number three, that's the bearing cap and identify that in this view here is most appropriate. Place that there, continue. Then item number four is the fastener. That I select the fastener, bring that balloon out, continue. Now we've identified every part within our assembly. We can tidy these up a little bit. Cancel. Let's get out of the balloon. So we can select the balloon number one, hold down Control on the keyboard, and then left click balloon number two. We can align these. So if we right click and align these balloons vertically. So I'll input. There. It's looking nice. We can do these horizontally. Left click, hold down Control, left click, right click line. Go for a horizontal alignment here, input those roughly here. Looking nice. That's how we add parts list, fill in the information, change any of the columns, and also to identify each part within our assembly using balloons. In the next lecture, I will complete the two D engineering drawing for this entire assembly and each of its parts. I'll see you there. 57. Project 7 - 2D Engineering Drawing Bearing Block Assembly: In this lecture, I'll be using all of the tools that we have learned in the previous lectures in order to complete an entire two D engineering drawing for this assembly and its parts. So the very first sheet is the assembly. Second sheet is the H beam. Third sheet is the bearing block. The last sheet is of the bearing cap. So let's start with the assembly sheet. First of all, I'm going to click New. I'm going to select an appropriate drawing. In this case, I'll just use the default So dot dwg create. I'm happy with the size being A three, the border as well, and the title block. I do need to add in a few more sheets, though. I'm going to rename these, so sheet one, edit, call that the assembly. Sheet two. Let's call that the H beam. Sheet three is the bearing block. And Set four is the bearing app. Okay, so we're on the assembly sheet right now. Let's go ahead and add that in. I'm going to select base. I select the part. So I've already got it open down here. So my assembly gonna put in a side view, and let's go for an IO view as well. I'm gonna change the scale there. Let's go one to five. Okay. Now, if we see we're still in first angle, it's not what we want here. I'm going to go to manage styles Editor. Going to come into my standard default standard ISO view preferences, select third angle, save and clothes, re input those views. Side view over there. I'm going to rescale this. Let's go one to eight. Nice. Let's change the style of that view. Let's go shaded. Let's type in here an identifier. Let's go ISO view, turn that on. I'm going to keep the scale there because it's different from the default position the label there. Let's do the same for this view. That down there. Same for the side view. Let's go ahead and ads in some dimensions. Let's do a baseline. One, two, three, Okay? Nice. Go ahead and add a parts list, select that base for you, leave everything as default, place that there. I want to add in the material, column chooser. Go on the material, add ok, applying nice. Let's tidy that up a bit. Now let's add in some balloons. Balloon one. Make these aligned. Let's go the horizontal alignment. Okay. Let's do the same for these two. So control, click both align, go vertical alignment. I want to change my styles here, I want to use a decimal point. One decimal place is only required. Go in the dimension, default, period, one decimal place. Save. That's looking good. Okay, so that's it for the assembly. Now move on to the H beam place views, base. I go to select my H beam, structural beam, but in the base view, the front view, but in a side view. Let's go with an IO as well. Keep the ratio one to five. Reposition those. Change the scale there. Let's go up for one for eight again. Pull that ISO and that on. We're going to leave the scale in there. Position that. Change the style as well. Let's go shaded. Move that down slightly. Add in the front view. In the side view label. Take out that scale as well. You need to add in some dimensions here. Let's go into annotate dimension. We can just select this one line here. We got the length of our eye beam, which in this case, is 1,000 mil or 1 meter. Let's go from the top to the bottom, give that an overall height, 200 mil or eight inch. Let's also identify the thickness here. Let's also put in a AD as well. So for the radius here, we can just select on the RAD. Then we'll see the dimension appears with an R in front of it indicating radius four mil. Now, I beam is purchased or H beam is purchased in standard sizing. So you just go for eight inch I beam, and the dimensions would be according to however they're manufactured. So you wouldn't typically state such dimensions here. But for the purposes of this lecture, I'll add them in anyway. And let's also dimension the width here. Let's go over 200. Okay. That's looking good. Now let's go on to the bearing block, place views, base, cast body, in this case. I'm going to change the scale there. Let's go one to two. Looking nice. Let's project that. Double left click. Select the arrow there. Let's put in an IO as well. We also need a top view because there's quite a lot of detail which we're showing here. Arrange this IO first. Let's go shaded. Call that IO view. We don't need to show the scale here because we're going to leave that as a ratio of one to two, and that's aligned then with the base, the side, and the top view. Change the style of that shaded. Looking nice. Add a label to the top view. Top view. Then the light bulb on. Okay. No keep that to the top. Side view. I don't want to show the hidden lines here, so I'll select that view. Click off the style from base. We're just hidden lines removed. I want to keep the hidden lines in here, mind. Now we can go ahead and start adding some dimensions. So let's go to annotate dimension. Start with the si view first. Here, we're going to add in this dimension. So 54 mil. Going to add in the 14 mil here. A going to go for the with 46, that label. Again, go on dimension tool. Let's start with our front view. Let's do a total length of this 200. I want to indicate the center line of these slots. So to do that, we're going to use a new tool, which is the center line bisector. If we select this, then select one end of our slot and the other one, got the center line up here, repeat the process via the other side. And then I want to dimension between these two center lines. Bring that down 154 looking good. I also want to show a center line for this arc to do that. Let's select the center mark, like so looking nice. Again, we'll dimension this. Let's dimension the RAD. Put that in there. Yeah, 24 radius, okay. Dimension this height, 16. Now, I don't like that 16 being there. It's not too visible. So I'm gonna hold down the left mouse button, and I'm actually going to drag the dimension away.'s position that roughly there, maybe pull this in slightly. That dimension back like so. I want to add in a center line as well for these through holes here. So let's go on the center line bisector. L two inner lines on both sides. Let's put in a dimension between these center lines. At mil. That snaps in place looking good. Let's come into the top view now. Now, same for the holes, I want to add in some center marks, so I'll left click once there here. Also on the arcs of the slots like soap. Come back to the dimension tool. Start with the slots. So we'll do the width of these 12, do the distance from the center line of this arc to the sight line here 18, tidy that up, so I'm going to hold down left mouse button, move that dimension there much more visible. I want to use the hole and thread dimension tool and then select the hole here, that identifier there. So 12, 1.75 thread pitch dash 68, right click. Okay. Let's go ahead now and let's move this out the way. Let's add in a dimension between these two outer vertical lines. I'll be 60. Let's go between the endpoint of this arc to the endpoint of this arc 1,000.2. Let's now input a ad on this arc here. Let's come out radius 50. We also need to define as well the width of the slot. In this case, it's ten mil. Move that dimension out a bit more tidy. That's looking good. And then we can dimension as well. This drop or recess, six mil. A move that dimension out looking nice. That's looking good. Let's move on to the last sheet, which is the bearing cap. Again, place views, pace. Let's go on the cap ratio here. Let's go for one to one. Keep the hidden lines in there, double click, add in a side view. Also an ISO view. Let's go for a top view as well. There's quite a bit of detail going on here. Do the ISO view first. Et's work on the front view from here. So quite a few dimensions to add. Let's go annotate dimension. Start with this distance here. 12 mill. Then need to define from here to here, which is 20. Need to put in the center line for the through holes. Use the bisector center line. These two, these two I got a dimension between these two. Should be 80 mill, that's right. Dimension between the center line and the beginning of this arc six mil. Move that dimension over slightly. Then you add a radius here, 24 mil Alsd this arc here, add in the center line for this arc. Then let's just add the last dimension, which is this line here, six mil. Looking good for the front view. Let's move on to the top view, so we'll put a label in there. Actually we keep that up there. Let's go dimension. These through holes. You need to put a center line on those, one, two, looking good, adding some more dimensions then. So we've got this arc here, which is a Rd of 50. Then we also need to identify this rat here, which is, in this case, it's 20. We don't need to show the hidden lines here. I don't think they bring too much value. So in that case, I'm going to remove the style from base, remove the hidden lines, press o Looking good. Let's finish off with the side view, double click. Go on the dimension. Let's give the depth at width, in this case. Let's also give the distance here 16 mill. And let's remove these hidden lines as well, remove the link, burn off the hidden lines. And there we have the bearing cap. So just so that you're aware of all the dimensions I put in, I am referencing the PDF that I showed you at the start. So normally it would take me a bit more time to do this, but I'm just quickly doing that for the purposes of this lecture. But there we have the entire to the engineering drawing for this assembly here. Or assembly drawing, identifying each one of the parts, the according details, and then we go into each individual part, identifying those dimensions, any relevant details there. We can also add some text as well. So for example, under the bearing block, if this is cast, we might want to add some text. So shortcut T on the keyboard. So if we can put in some text here, let's say, I don't know, no shaft edges, et cetera, et cetera. Okay. We can modify that text by double left clicking, selecting that, and then we can change any of the properties here, so we can make that five. Well, we can change the font for us, okay. And we've got some quite exaggerated text just in the bottom right there. So that is a very quick overview of all of the tools in which we've covered in the previous lectures relating to TD engineering drawings. I hope that's all clear. And once again, any questions, please do send them to me. But aside from that, I will see you in the next lecture. 58. Customizing the Title Block: In this lecture, we will take a look at how to build and design your own title block for two D engineering drawings. So this lecture I actually created around two years ago. It was for a group of students. They were studying automotive engineering for a university in the States. I had a lot of good feedback, and it's still very much applicable. And so feel free to design the title block as per your needs, if it's to impress a client or for your boss or your lectra if you're at university. Once you finish, do remember to select File and then save as, and then save as a template, save it in the according location, and you can access that for all of your future TD engineering drawings. So let's begin. The title blocks, there's only one available, which is this one. And if we insert, this is fairly bland. I don't particularly like this one. So I'm going to delete that. And instead, I'm going to right click on the older itself. I'm going to select define new title block. So this is where we will design our own title block. So to do this, we use the standard sketching tools, and we will draw in the title block and add the appropriate text. So in this tutorial, I will be redrawing my title block that I use in my lesson plans. Feel free to copy this, and you can add or change it appropriately. So I will go ahead now and draw the frame for my title block. I will speed the video up for this. So that is the complete frame for our title block. I'll now go and input the appropriate text boxes for this. So to do this, we'll select text up here, and then we'll just click once roughly where we want that text to go. And so in this case, I'll input title. I'll put that in capitals, and here we can change the font. So here, I'm going to go for size 2.5 and click. Okay. And then I'll just dimension that based on its anchor point, which is here. I'll just go ahead and input all the remaining textboxes, so I'll speed up the video again. And There we have our text boxes in place. And now I'm going to go ahead and input a logo. So to do this, I'll go to insert and then image, and I'll select my logo. That's looking good. Now, let's just check what this looks like. So let's go up to Finish Sketch. I will save this title block as let's just say example block. I'll click Save. And if we zoom out, double click the middle mouse button, if we go over to our drawing resources folder, we can see that under the title blocks, we have our new example block. So if we want to insert this, let's right click and select Insert, and inventor will automatically position it in the correct place, which is in the bottom right hand corner, in this case, that's looking good. Just a few more things to add, such as the projection mode. So for me, this will be third angle projection. And then the units, again, in my case, I work in millimeters, so I will go ahead and input them now using these sketch tools. Okay, that is looking good. Before we do any more work on this, let's save it as a template. So let's go to file and hover the mouse over Save As, and then we'll select Save copy as template. We'll select that. And our inventor will open up the location for our template. So let's call this example, TD template. And let's click Save. And now, if we go back to our home screen, so I'm going to select the home icon down here and then we'll go to New again. We can see here we have our example Tod template ready to go and we'll select Create. And here, this is our template. And next, we need to add the smart text to identify the properties that are currently missing. So to do this, let's go over to our drawing resources folder, and we can go under Title blocks under our example title block. We can right click and select Edit. And here, let's put in the Smart text for the title. So we'll select text. We'll click roughly where we want that to go. And to Smart text, we use these three boxes here. So we identify the type, the source and the property, and then we click Add. So for the title, this would come under the standard I properties in relation to the primary or the attached model. The property here would, of course, be the title. If we scroll down, we can see that there. Click Add, change the sides to three. And as you can see here, we have title, which is in parentheses, which indicates that this is smart text. Let me finish the sketch there and press. And you'll see this is empty, and that is because we do not have a model. Let's put in a basic model, so I'll put in this steel plate. That's okay. I just tidy that up. If we look now at our title block, we can see that the Smart tech has recognized this part as being stainless steel plate. So if we go into that part, we then go to file and I properties, we go to the summary. You can see the title is stainless steel plate. Let me change that. I'll put with say, jacking hole. Press Okay, just click Save then we go back onto the drawing and we can see that Smart text has picked that up. That's excellent. Let's do the same for material. So again, we'll right click on the title block and edit, enter in the text. So for material, again, standardized properties of the attached model, and we'll select material, d, change the size. Finish. Yes, and we can see here it's identified the part, it's mild steel. Let's say that we want to change that. So let's go to our material, and we'll go to, let's say, stainless steel, S if we scroll down, we can see yet, the Smartex has picked that up. That's great. Now let's do the drawn by and approved by. So again, we'll right click and select Edit. Add in text. Let's do the drawn by first. So this would come under the standard properties of the current drawing. So this is the engineer or the designer, rather, who is creating this drawing. Add that person in and enter three, and we'll do the same for the approved by. So again, it'll be under the current model, and the property here would be the engineer approved by. At that in, change that to three. Press Okay. We'll finish this sketch there. Click, Yes, you can see, it's drawn by. That's me. That's Chris and approved by. That's Dylan. If we want to change these, we can go to Flee properties. And under project, we can identify the designer here. So let's change. Let's just write my short name so that's Chris. And then for status under the engineering approved by, we can just put Dylan. It's okay. And so, yeah, we can see that the Smart tech has picked up these changes. Under scale, we can do that by right clicking and going edit and adding in text here. The scale would be in relation to the sheet properties. Again, the current drawing would be the initial view scale. So we'll add that in. Just finish sketch there. Press, yes, and we can see that the drawing sorry the model being displayed now is a scale of one to one. Let's change that to, let's say, one to two. If you go down now, the Smart text has it get picked that up. And last but not least, we have the sheet. So we'll right click on our title block and edit, add in the text here. And so if a sheet, I will do the sheet number over the total number of sheets. So I'll show you how to do that. That's, of course, in relation to the sheet properties under the current drawing. This will be the sheet number. Add that in. We'll then add a space and a forward slash, and then we'll go to the drawing properties and add in the total number of sheets. Just change that to size three and press Okay. Roughly position that. Just finish sketch. But yes. We can see here that this is sheet number one of two. And if we go over to our model browser here, we can see there are two sheets that are currently on sheet one. And so that is how to add the smart text to the properties that are shown here. If you have any questions, please ask them in comments section, and I'll reply as soon as I can. But aside from that, I will see you in the next tutorial. Thank you. 59. Section Introduction - Additional Useful Content: This section includes a series of practice exercises that utilize the various tools covered in previous lectures. These exercises were created for students in the USA to practice and prepare for CAD exams. They received a lot of positive feedback and are intended to be beneficial to you as well. Each example is explained step by step, detailing the tools and techniques used to generate these sketches, models, and assemblies. 60. Coil Command - Modelling Springs: In this tutorial, we will learn how to draw a conventional spring using the coil command. So I have opened up a new part and I will start a two D sketch. We can select any plane here. In this demonstration, I will choose the XY plane. And first, we'll start by drawing a vertical line about the origin. We can draw this at any height. So I'm going to input 10 millimeters. And this line just represents the axis of the spring. We'll then draw a circle to the right of the origin. This will be 15 millimeters. I'm going to put a horizontal constraint between the center point of the circle and the origin, like so, and then going to dimension between the origin and the center point at a distance of 50 millimeters. We'll then go on to the three D model tap and we'll select the coil command. And here we have our dialog box. So our profile has already been selected, which is the circle here, that's correct. And for the axis, we'll then select our ten millimeter vertical line here, we can see a preview of how the spring will be. Under behavior, we can select the variables we wish to input. So, for example, the pitch and revolution, revolution and height or the pitch and height. For this demonstration, we'll select the revolution and height. So in the revolutions, we'll input six revolutions and for height, we'll input 200 millimeters. We then have the option to add a taper if we want. So, for example, if I enter 15 here, we can see a 15 degree taper, like so, but a conventional spring will not have a taper. And the rotation, sorry, we can add either a left hand or right hand rotation. Let's stay with the left hand rotation. If we click Okay, you can then see our conventional spring like so. If we look at that from the right view, we can see that the top and the bottom of the spring do not have flats, so this is not common in a spring. So to enter these, we can right click on the coil feature and select Edit feature and add in a close start and also a close end. We can input the variables here, flat angle and transition angle. So I'll input both 135 degrees for the flat angles and 50 degrees for the transition angles, and we'll select ok. And here we can see flats on both the top and the bottom of the spring, which is more representative how the spring will come into contact with the top and bottom plates. That concludes how we draw a conventional spring using the coil command. I'll see you in the next tutorial. 61. Loft Command - Loft Modelling: In this tutorial, we will draw a basic part using the loft feature. So we will start by drawing in a number of planes, and then we will draw a sketch on each of those planes, and then we will loft between those sketches. So let's select the plane. In this case, let's select Let's do the XY plane. I'm just going to turn on the visibility, so right click visibility. Then let's go a three D model, and we've got a plane, and we'll offset a new plane from the XY plane. Let's do a distance here of 25 mil zoom out a little bit, and let's do exactly the same from this plane. 25 mil, and then just one more time from our new plane here. It's 25 mil. Let's input our last plane. So we offset from plane, and we'll choose the original here, so this is the default XY plane. And here we'll select -200 millimeters and press Enter. So here we have the five planes that we'll use for our part in this tutorial. Let's start on the default plane. Let's start a two d sketch. And here we use the two point center rectangle from the origin, and we'll input a square here, which will be 60 millimeters to press tab and then enter 60 again. So there we have our first sketch. Let's finish that sketch. Then let's select this offset plane here, create a two D sketch. And here we will input a circle again from the origin, we'll put in here 50 millimeters in diameter, finish that sketch. Then we'll start a new sketch on this plane, which will be again a circle, but in this case, it will be 85 millimeters. Finish that sketch, and then we'll just input the final sketch here, which will be an offset of sorry projection of this circle here. So another 85 mill circle you could draw instead. So we will begin to loft between these four sketches here. I'm just going to turn off the visibility of each of these planes. Okay, so we've got a three D model, and we'll select the loft command. And here we will select our sketches that we want to loft between, so we'll select all of our sketches here. Then we'll select okay. As you can see here, we have the sort of handle element of our part. We just need to draw the final geometry on this plane here. So let's select this sketch. Start at two D sketch. I'm just going to rotate the ViewCube, like so. And here we'll draw in another two point center rectangle from the origin, and we'll dimension this as 150 at length. Breast tab, we'll enter in a height of 5 millimeters. Press enter. I'm just going to rotate the model there, and then we want our final loft to be between this sketch and this face here. So we've got a three D model. Select the loft command. I'll select this sketch here. Then over here, we'll just select, this profile. Now we can see that's the correct loft that we want. That's okay. I'm just going to hide that plane. And then, yeah, there we have our part that's been created using the loft command. I'm just going to touch this up a little bit with the Fillet tool. I'm going to drag cross these edges here. I'm going to input a five mil fillet. It's okay. Go to the home view. There we have our completed part. If you have any questions about the loft command, please post them in any comments section. But otherwise, I will see you in the next tutorial. Thank you. 62. How to Split Bodies: In this tutorial, we will learn how to use the split command. This can be used to either split faces or to split solid bodies within a model. And so as we can see here, I have drawn a basic part, I've drawn in a sketch profile on this plate and here we will use that as our split line. So let's go to three D model, and under the Modify panel, we'll select split. We have a small dialog box pop up. Now, first, we need to input our tool. This can either be a plane or a sketch profile. So I will select the sketch profile that I drew in here. I'll select and then for faces, we need to select which faces that we wish to split. And so to start with, I'm just going to select these three faces here. I select Okay. And as we can see, I've split these faces up, so I've got a total of six faces now as they intersect with our sketch profile. I'm going to delete that, and I'm going to re select our sketch profile, but instead, I'm going to select all faces. So every face that's intersected by our sketch profile will be split. Like the exact same principles as before. We have two faces based upon where our sketch profile has intersected the model. I'm just going to show you one last demonstration, which is by turning on the solid selection. So first, let's select the tool. Let's use the same sketch profile again. And under solid selection, inventor has already selected this solid for us here, we know that because under the solid bodies folder, there is only one solid to choose from. We have some behavior options here. So if we wish to discard one side or the other, we can do so. But for this demonstration, I will keep both sides and select Okay. And now, if we look at our solid bodies folder, once again, we can see there are now two bodies we can choose to change their visibility. And we can even apply different properties to each of these solid bodies. For example, if I select solid body 18 and solid body 19, we can see here that I've applied two different appearances to each of the bodies. But that's a summary of the split command. If you have any questions, please put them in the comments section, but aside from that, I will see you in the next tutorial. Thank you. 63. Condensed Summary of Inventor: Welcome to this beginner friendly tutorial for Autodesk Inventor. This video will guide you through the absolute basic tools and features required to sketch three D model and assembly parts in Autodesk Inventor. By the end of this video, you'll know how to create simple three D parts and assemble them. We will go step by step and draw a basic bracket with some through holes and a Shamford corner, as we can see here. Then we'll draw a standard threaded hex key bolt. And finally, we'll create an assembly file consisting of one bracket and two bolts like this. So let's get started. Let's open inventor software first. Once us done loading, we can see the home screen. In the center, we have all of our recent files. They could be parts, assemblies, or drawings, et cetera. At the top, we have an array of options for customizing and changing various settings. And on the left, we have options to open existing files or create new ones, which is what we're going to be focusing on today. Let's start by clicking on New here we are presented with a selection of templates. At the top are the part templates, then the assembly templates, drawing templates, and so on. It's important to choose the correct template as this will define the file type, the units, and other attributes. We want to start with a part file. Now, personally, most of my work is in metric units, so I mean millimeters, kilograms, et cetera. I will therefore choose a standard millimeter part template. However, if you want to draw in inches, imperial, then select the English folder here and you'll be presented with the imperial options. Once you've chosen your template, click Create. Now we have opened a Part file. Let's take a quick look at the interface. In the center, we have the three D environment. This is where we will be sketching and three D modeling and is the main focus of part files. On the left, we have our design tree. This is where all of our sketches and features will be shown, and it enables us to edit these, which we'll be seeing later. And at the top, we have a series of tabs. The main two our sketch and three D model. And each tab is a series of tools relating to the tab title. We'll be using the core of these today to sketch and model our components. On the right hand side, we have our viewing tools and most importantly, the view cube, which we'll be also using today. Let's start by sketching and three D modeling the bracket using these dimensions. First, we need to break the component down into features and sketch and three D model these individually. We'll start with the base, then the vertical walls, then the extrusion holes. And finally, we'll add some radii to the sharp edges, and we'll also change the appearance and do a basic render. Now let's get started with the base of this bracket. So if we come up to three D model, we've got the option there. Start two D sketch. Let's click that. And then you'll see we have three planes. We have the XY plane, the Y Z plane, and the X Z plane. We need to choose one of these to sketch on. So for the base, let's go for the X Z plane. Let's click that. And then we come back up to our tabs. Come under sketch, and you'll see a whole series of sketch tools here. We're going to start with the basics, which is the rectangle tool. Now, we do have the option here for different types of rectangle tools. We've got slots and polygons as well. We're going to start with the absolute basic, which is a two point rectangle. Now, let's come to the center where we have this yellow dot. Let's click on that and bring this out and we can just click that so that we have a rectangle. We're still in the rectangle tool. So if we keep on clicking, we'll be creating more rectangles. What you can do if you are in the rectangle tool is just right click and select Okay, and there we have our rectangle. So to bring that to the center, we can double right click on the middle mouse button, and we can zoom in and out with a mouse wheel. So we want to dimension this. So let's come up to the again, under the sketch tab, let's go to dimension. And let's select this line here. We'll click and then we'll see the dimension as per the drawings 80 Mill. Okay, it's looking good. Again, double click on the middle mouse button, zoom out a bit. We're still under the dimension tool. Let's click this line, put in the other dimension here, which again, is 80 Mill. And there we have our basic square. Right click, press Okay. We want to put this circle in the center. Alright, so we've got the circle tool here. Again, under the drop down, we've got different tools, but we'll start with the center point circle. So let's just click anywhere inside the square, open that up, and it's got a diameter of 30 millimeters plus enter. I want to get out of that tool, so right click, preso. But now this circle can move absolutely anywhere, which we don't want. We want that to be in a fixed position. So again, let's choose the dimension tool up here. Click that circle. Let's go for the top line. Let's put in the dimension, which in this case is 40 millimeters. All right, let's do exactly the same with this line here. Again, that's 40 millimeters, and now that's in the center. Right click. Okay. And we know now that our sketch is fully constrained. The square can't move or the circle can't move. Because if we look down here, we'll see it says fully constrained. So everything's fixed, everything's engineered well there. Now the next feature we need to add is this Shafer in the corner. So to do this, there are different ways. But for simplicity, we'll just come to the line tool. We're going to select the generic line, and we're going to snap to this line here, and we're just going to snap anywhere on this slin like so, right click. Okay. Then we're going to click the dimension tool, click the end of this line, and let's go for the corner down here and input this dimension, which is 20 mil. We'll do the exact same process over here. Input this dimension, 20 mil. And there we have the profile that we need to extrude. So to do this, let's go on finish. So we see finished sketch. We'll click that. Okay. Again, double click on the middle mouse button, zoom out a little bit. And then we'll come over to three D model. I see, we have a load of three D model tools here. Let's click on the most commonly used tool, which is extrude. And we're going to extrude the profile which we want. We're going to come back to this toolbox in a second. If we move the mouse over this profile, this is the profile we want to extrude. Also got the option of this profile and this one as well. We don't want to extrude either of these. We only want this profile here, so we'll click now let's look at this toolbox. So we've selected one profile, which is correct. Okay? And under behavior, we've got different directions. The default, we can choose the opposite direction, okay, like so, we can choose a sorry symmetric, o? So that's extruding in both directions, and then asymmetrical. So we can extrude so much in one direction and the other. Let's just go with the default, right, then put our distance in. So as per the drawing, this is ten. But you can change that if you like. I'm going to go with ten. I'm going to click Okay, and there we have the sort of generic base feature there. I want to show you the view cube quickly, which is over here. And if we left click and drag this, we can view it from all sorts of different angles. Okay, we can also click on the according faces or the arrows so we can see everything from a different angle. Alright, so that's the base feature done. Let's move on to the side walls. But for these side walls, nice and easy. First of all, we need to define the plane in which these side baalls will extrude from. In this case, it's this plane here. So different ways of doing this, but what we can do is left click. Got a series of options here to edit that feature, which we don't want to do. We do want to create a sketch on this plane, though. So let's create so let's click Create sketch. Okay, I'll use the middle mouse button, bring that back to center, and we'll see we're looking directly at the face we want to draw on. Let's come up again to the sketch tools, select the rectangle tool. I go to start from this corner here, we're going to bring this over and snap anywhere on this line here, right click. Okay. Select dimension, and let's dimension the distance between these two lines. So that's the thickness of the wall, which in this case, is 10 millimeters. That's one wall, right click. Okay. Again, let the rectangle tool start from this corner and come up anywhere. Snap on this line here. Let's go dimension between these two lines here, and it's the same thickness of ten mil. Okay, right click. Okay. Let's now extrude these. Three D model extrude. We need to select the according profile. So we want this profile. We also want this one and this one as well. Back to our box. So we've got our three profiles selected. It's the correct direction. We don't want to be extruding in the other direction. We want to bring these up by 40 millimeters, input 40, press Enter, and there we have our side walls. We've got our side walls. We need to input a fillet on this edge here. Now if we look around the back on this edge here. Okay? So go back to the home view under three D tool. So we've been using the extrusion tool. This time we're going to use the fillet tool. Let's select that. We've got our toolbox pop up. Now we need to select the edge that we want to fill it. Let's select this one. Okay? And as for the drawing, it's a five mil fillet. Let's put five in plus enter. It's looking nice. Got a fillet on the back of 15 mil. So let's take the ViewCube, turn this around, choose the Fillet tool again. Got our input 15 mil, select this edge there, preso. Just click on the home button, and there we have our two fillets and our two sidewalls. That's looking good. Now, let's go ahead and add the extrusion holes to these two faces here. We're going to be using quite a lot of tools that we've learned already. But this time, instead of adding material, we're going to be removing. So let's start by left clicking on the plane we want to draw on, and we'll create a sketch, bring that to the center. Go up to the sketch tab, kind of select a circle. We can draw that anywhere on this face. We're going to diameter that 15 millimeters as per the drawing. Right click, okay? I want to dimension this, so I'll select the circle and the top line. That's dimension that that's 20. Okay? And then exactly the same from this line here, which is 35. Okay? Now, if we look here, we're fully constrained, that's all good. Let's press finished sketch. Okay? So we've got our geometry there and our profile in the center. Let's go on three D model. And then we'll select the extrude tool. But in the tools box here, we've got our profile already selected. Great. But this time here, we want to flip the direction. Now, what you'll notice here, if I rotate the model, it's actually cutting material. We know that as well because down here on the output, the output is to cut. So it's actually removing material as opposed to joining or adding material. So if you click Okay, we've now got our through hole there. Let's do exactly the same on this face here. So we're left click, create a sketch, then the center, circle, 15 mil, dimension, circle to line 20 circle to this vertical line, 35, right click Okay, finish. G3d model, and we'll extrude that again. And this time, yeah, we can either select change the direction, so automatic cut or we can just select cut. We recognize to remove material there. Click Okay. Home screen, and there are we have our two holes there. Now, in the final stages of this part, let's go ahead and add some radii to these sharp edges that we see here. Let's also change the material, the appearance, and we'll do a basic render. Let's start with the radii. We'll go up to three D model tool, and we'll select fill. Okay, now on this, I recommend putting in a one mill fillet, and we just want to select certain edges. Now, there are different tools that we can use to select. So we can select individual ledges, or we can select loops. So a loop would be like we see here. It's like looping where that edge kind of leads to and would radio all of that. For simplicity, I prefer just to select individual edges. So I'll select this one here, this one, this one, these guys also do the holes Okay, so we see a preview there. Those are all the edges that I want to select, and we'll press Okay. All right. So we got rid of those sharp, inner edges. That looks good. Now, let's go ahead and change the material. So for this, we go up to the very top here and we've got our material selection. So let's open this up. I'm going to apply it, but it's up to you. You can choose what you like. I'm going to apply a stainless steel. We see a nice sort of visual appearance there. In terms of color, again, up to you. We'd go for sky blue, dark. It looks quite nice. Then let's go into view, visual style. And let's do a very, very basic rendering of this. So in the view tab up here under visual style, we can select, like, without edges, so we just see it shaded. Obviously, with the edges, various other options here. We can see a wire frame assembly and so forth. You can play around with these. A basic render. Let's go to realistic. And then let's change the lighting as well. So typically, we're on default IBL. For this, I'm going to choos Photo Booth. Then click on ray tracing. Then we'll see down here, we've got different options. Depends on your computer hardware. I recommend going for a low quality ray tracing. Otherwise, it's quite demanding on the hardware. As you can see, that's already complete, and we've got there. Yeah, quite a sophisticated looking model. Okay? If you want to come out of the rendering, again, we just click ray tracing there, then we're back to the standard appearance. We can put some edges on that. Okay, so that's it for the bracket. Now, let's move on to the bolt. So let's come to the home screen. Now, the quick way to do this is to come up to the top and just select home. Okay, now we're going to go a new. We're going to come under part again and select the same template. So in this case, standard mill for me, click Create. Now we're in the part file. Now, the bolts quite straightforward. I'm going to start with the threaded parts the same process. Let's come under three D model and go to start two D sketch. Got our planes again. Let's choose the X Z plane once again. In this case, we'll come up to sketch. We're going to start with a circle, start right in the center that yellow dot, it's called the origin. We're going to put the diameter of the threaded part. So the shanks 15 mil. It's okay. Right, click Okay, finish. In a three D model, extrude that part. We're going to extrude that by the full length, which is 30. A double click middle mouse button. Now I want to add that hamper to the bottom side here. So this is a new tool. We've used fillet already. Now the tool next to it is Shampa, so let's click that. Now, this shampa is two mill, a two mill by two mill. So got two mill selected already, which is great. I'm going to click this edge here. It's apply to two mill, like a pio. Now, if we look around there, we can use the ViewCube. Yeah, that's looking good. Now we want to create the head. So let's select this plane here. That's the plane we want to draw on. We'll go and create sketch. Okay, use the circle tool again. Start from the origin once again. The outer diameter is 25 mil. Plus okay. Right click. Okay, finished sketch. Red model. Let's extrude not by that much. Let's extrude that by five mil in total as per the drawing. Got a chamfer on there again, another two mill hamper. That's on this edge here, plus a pi. Okay, that's looking good. Now we want to add a thread to the threaded portion here. So right next to Chamfer, we've got the thread tool under three D model, so we'll select thread. We got our toolbox here. So it was asking what face do we want to apply a thread to? This is the face here. We click here. And then we need to define the thread. So antimetric typically isometric, the size or the diameter, so M 15, in this case, and the thread, the thread as well, which is 1.5 mil. Direction, we can go left or go right, behavior, we can do the full length or we can add just a shank there followed by the thread, so we can select 20 plus okay. And there we've got our visual thread. Now, we just need to add the hex key on the top, so right left click there, create a sketch. Now, we've used the rectangle tool before, and if we click on the drop down, we've then got polygon option. You can choose the number of sides. In this case, we're going for a hex, so six sides. Select the origin once again. I'm just going to I just draw it this big. There's no issues, press done, apply dimension. So yeah the flat to the flat. And that is a total of ten mil. Press okay. Let's go finished sketch looking good. Let's go three D model. We want to remove material there, so we don't want to use this type of extrude. We want to flip that, okay? And that's got a depth of five mil, so it's okay. There we have our hex key right there. Okay, let's go ahead and apply material to this. I'm just gonna get four. I just gonna stain the steel. Looking good. Okay, let's save the part, and let's move on to the assembly. So to create an assembly, we're still in a Part file. We need to exit this. We need to go back to the home. So on the top left here, we've got the home icon. Let's click that. And then we'll go on New again. So we're going to open up a new template. But this time, instead of a part template, we're going to open up an assembly template. So again, I'm coming under metric, and I'm going to select the standard millimeters template here. Okay, I'm going to see here it's an assembly uses millimeters. Click Create and now we're in the assembly file, okay. So in terms of user face here, again, in the center, like the main focus, we've got the three D environment. The left hand side, we don't have a design tree as such. It's more of like a parts tree. So it lists all our parts, the relationships between them, any constraints that we give them, which we'll be doing later. At the very top, we've got a whole series of tabs and options for us there. But again, today we're just focusing on the absolute basics. So we want to place our existing parts in here, which you've saved already. So we're going to come up under the assembly tab. We're going to place, okay? And then just locate the parts that you've made, okay? So I'll insert the bracket. Okay, now, if I zoom out, you'll see a bracket will be inserted, and then I've got the option to insert as many of these as I need, but we only need one of them, of course, so rest control Z, if you accidentally click anymore. So we put our bracket in, fantastic. Now let's put our bolts in. So again, place, find the location of your bolts. Okay. Click Okay. And then we want to have two of these, right? Now, in terms of inserting these, we have a few options before we click. We can actually rotate these around the according axis, okay? So if we right click, we can actually rotate around the Y, the X, or the Z. In this case, I want to rotate around the X axis. Okay? So this bolts go to sit somewhere here. I'm just going to throw it over there for the time being. And then this one here, I'm going to rotate around the Z, and that's going to sit somewhere there. So I'm just going to throw that in there. Once we're done, we right click Okay, now you'll see that we can move these two parts, but we cannot move the bracket. That's because it's the first part that we entered, and so it's fixed in position. But we know that because in the parts tree, where we see are three parts here, okay? So in this case, the bracket, I've called part five, and then part six of the two bolts. Next to these, we can see a black dot, okay? That means it's fixed, and then a white dot. And that means that it's not fixed, it's sort of fully constrained, and it's still mobile. So what we need to do now is position these in the recordings. So this one in this hole, this one in this one here, we want to have these, fully constrained and fully fixed. So to do this, we use what we call constrains. Okay? So if you select constrain, we've then got a tool box pop up where we need to select two faces and then give those a relationship. The default relationship is met, which is the most common one we use. Let's go with that first. So the first selection, okay, is going to be the axis of this bolt here. So we hover our mouse over, and we'll see that inventor recognizes that we want to select the axis, which is correct. So we'll click there. Alright. And then under selection two, okay? We're then going to select the axis of this hole here. Alright. We don't want to select any of these faces. We just want the axis there. Let's click there. All right let's click Okay, let's have a look at this. So now you see that the axis are constrained. They are concentric with one another, but we've still got all this movement, which we want to. We want to fix that permanently. So we rotate the model. So I do this on the keyboard with shift and then middle mouse button. You can use the ViewCube. Okay. So let's go on the constraint tool again, rotate that model. And let's select the flat of the bolt, and then select the flat of this face here. Okay? And now we'll see that that bolt is sitting comfortably in that hole. Alright, we can't move it in or out or up and down. It's fixed in there. However, we can still rotate it, like as you're seeing here. So let's put a constraint on. Now this time it's not a mate constraint. This time we're going to input an angle constraint. So we select that and this here, there are different solutions, so a direct angle, undirected, explicit reference vector. In this case, most common, most basic is direct angle. Just going to select any one of those flats, and then I'm going to select this face here. See the angle is zero degrees, so that face is it's parallel, essentially. But we could put an angle there if you want, like 25 or let's go 45. Okay, we're going to stick with zero. It's okay. That's looking good. And now, if we look at our parts tree, we'll see that part six, which is the spot here highlighted, I've got a black dot next to it. So it's now fixed. It's unable to move at all. Do the exact same process for this bolt here. So again, constrain, select the axis of the bolt, select the axis of the whole. Okay? Yeah, fantastic. All right. Let's move that out. Constrain, select this face first, then the flat of the bolt. Okay. Okay, that's nicely fixed there. I'm going to put the edges on, so view visual style with edges. You can see that a bit more clearly there. Still rotating. Let's put in the angular constraint. Let's go to assemble, constrain, angle. Let's go direct, select any flat, select the top. It's okay. On the home view. And now we see all three parts have a black dot next to them, and that is assembly complete. So from here, what we can do is a nice render if you want to use this. I know in a presentation or you're doing any marketing content, going to show it off to your boss. Click the View Visual style realistic. I like to use photoboth personally. I think they give nice lighting for rendering and I'm going to go on tracing. Okay, just give that a while to load. Again, I'm going with a low quality ray trace. And that is our rendering complete. That's looking pretty nice. Yeah, good job, everybody. Just before we finish, I want to quickly cover the parts tree and what we can do in terms of editing. But if you come under here under this folder, relationships, we open this up. We can actually see a list here of all of the constraints that we've applied, and we can modify or edit these, can delete them, et cetera. So if you want to have a play around with those, you can select the edit and adjust them accordingly. Also the origin. So this shows you the three planes. You can use these in assembly files or in part files as well. So they'll show you the three default planes and also the three axis and the center point or the origin, as I call it. And then we've got the individual parts here. So, yeah, you can right click and delete these. You can also open them up and you can see the constraints that have been applied specifically to that part. So in terms of modification, we always come back to the design tree, and it's exactly the same in a part file. So I come back into the file of the bolt. And we can see here that we have yet the origin. So we're seeing the three original planes and also the axis origin. We can then also see all of the features. And if we open up each feature, we can see the sketches. And we can modify any of this at any time by right clicking to edit sketch, or if we do this on a feature, we can edit the feature. Okay? We've also got the end of parts. So, for example, I can move this. We kind of go back in time, and so we can go to specific parts in our model, and yeah, just take a look at what we were doing there. If you have any questions about the topics we've covered today, please post them in the comment section, and I will respond as soon as possible. I hope you found this session valuable and that it has enhanced your skill set in Autodesk invento. This YouTube channel offers many other tutorials, so please feel free to explore those as well. And if you could like and subscribe, it would greatly support the channel, wish you all the best of luck with your endeavors, and I'll see you later. Thank you. 64. Condensed Summary of 2D Drawing Creation: In this tutorial, we will learn how to create two D engineering drawings. This is a preview of what we'll be doing today. So here, I've got a three page engineering drawing. The first page, as we can see is the assembly. The second page is of the individual part, in this case, the bracket, and a third page here is of the pin. So by the end of this tutorial, you will be able to create and customize drawing sheets, add moral views and edits, switch between first and third angle projections, edit decimals, precision and tolerances, and modify styles, text, and add parts lists. Be doing this step by step with this assembly here. If you would like to do it with the same assembly, you can use these dimensions and model these two parts up and assemble them. So to begin, let's come up to the top left. Let's click on NU, then we have our templates pop up. We don't want to part or an assembly. Let's choos a drawing template. In this case, I'm going to chose an ISO. You'll see here, we've got options for dot DWG and also dot IDW, as well. I recommend going with DWG, as this is more cross compatible with the other Autodesk software such as AutoCAD and Fusion 360. If you do want to have your own customized template like I've got here, I've got a separate tutorial on that, you can have your own title blocks, own borders, et cetera. Okay. But for now, I'm going to go at so dot dwg. Click CRE and now we're in the drawing file. So first of all, let's take a look on the left hand side. We see here we've only got one sheet in here. If we want to add more sheets, we can right click and select new sheet. Okay, if we want to select sheet one again, we can double click on that. Also, if we right click and select Edit sheet, we can change the title here. I'm going to call that assembly. We can also change the size as well, so I typically draw an A three. Over here, we've got the orientation. So if you want to portray or a landscape orientation, and then we can select where the title block with all of our relevant information will go, so I typically do the bottom right that's got a revision as well if you need to use that. So click. Okay, then sheet number two, I'm going to do the same. I'm going to edit that. That's going to be the bracket. Okay. It's going to be A three, as well, exactly the same. Then I'm going to add one more sheet. I'm right click Edit sheet. Call that. That's going to be the locking pin. Okay. All right, so let's come back to our assembly. Now, first of all, we have the title block down here. This is the generic title block that's supplied. I never use this. Again, if you want to create your own custom, do watch the video on that links in the description. But for the purposes of this tutorial, I'll stick with the one here. If you do want to do any quick edits to it, just come under drawing resource under title blocks. Right click on the title block and select Edit. And then we can edit anything about this. So we've got the smart text in here. We've al got all the lines, all the borders, et cetera, okay? So we'll click finish. Once you're done with that, I don't need to save any edits there. So let's go ahead and add the assembly to our first sheet. So to do this, we come up to place Views, and then we select base. Now, inventors automatically selected my assembly already. That's because I have it open already in Inventor, but if your part is closed, it won't appear here. In which case, click on open an existing file, locate the file, select open, and then it will appear. Got some styles that we can have a play around with here, so we can do a shaded view. So this is already shaded here so we can see the appearance, and turn that off for now. We've got the hidden line removed or we can add the hidden lines under scale, we can change that if we want, so we got 1.0 plus o. And there we've got our view. If you want to add a projected view, there are different ways to do this, we can double click on the view, and then we can project the side view or the top view using these arrows that we see here or I can do an ISO view like so o. So you'll notice here that this is first angle projection. I just turn on shaded so you can see a bit more clearly. This is third angle projection. But if you want to work in first angle, it's an easy switch. So if we delete those Okay, come up to manage, click on Styles Editor, come under the standard under default standard, view preferences, and you can switch to first angle just here. I normally work in third angle, and I'll stick to that for this tutorial, so save and close. Let's put that view back in, so base. I want to have an IOview on this page, right? I want to bump that up a bit in size. Let's go for 1.5. I don't want to have the front view, so I'm going to just click Delete on that. Okay? So delete that view, place this roughly in the center. I want to turn shading on. It's looking nice. Now I want to identify these individual parts. So to do this, I want to have a Ps list. Let's come under annotate at the top and come under parts list. And here we need to select either a document or the view itself. So I'm going to select the assembly. Okay, that's looking good. Let's click Okay. Now we can just left click and put that anywhere. Now, if we hold down the left mouse button, we can then snap that in any of the corners. I'm going to go for the top left. A bit more information in there, so it's double click, right click on one of the columns on column chooser. I'm going to add in material. Solet material add, click Okay. Okay. Make that a little bit bigger and move that re snap that to the corner, like so so here we're identifying the items, so it'll be balloon one and two, the quantity of those within the assembly, the according part numbers, description of each and then material. So we need to identify item one and two. So to do this, let's go to annotate, select balloon, and let's click on the bracket here. Okay. Let's put in balloon one. Right click Continue. And then for the pin itself, let's click on that and then we're going to put in pin two. We can adjust these. So, for example, if I want to move this around, we can hold the end of the arrow and reposition that. I do the same for the pin. Now, if we watch the arrow head on the pin here, it will turn to a circle. Now, a circle will only appear when it's in contact with a face only, and an arrow will appear when it's in contact to an edge. So it's just a way of better communicating what you are trying to identify. Looking good. Let's add a view to that, as well. So I'm going to come down here and collect, toggle the visibility and press Okay. All right, so it says, yeah, view ten and then the scale there. All right. So I can change that double clicking on this. I'm going to call that view one, put a space there. So it's saying view one is the scale 1.5 to one, in terms of its size. Add a bit of information here. Again, I don't like this title block. I always use my own custom one, do watch the tutorial in the description for that. But for the purposes of this tutorial, just go ahead and add in some of the smart text information. We come under file, come to I properties, and add in the company, spot your name wrong. And like, Okay, there, click Apply, okay. And now we can see the Smart tech has pulled in the company, who it was checked by, who it was approved by and the date. Then we've got today's date and the sheet number as well. Again, any more information on this, do check out the tutorial in the description. Okay, so let's move on and input the other two sheets. We've got the bracket and the pin, double click on the bracket. Again, place views, not projected. Let's click base. Now we need to select the base part. So here I've called it bracket one, two, three. Okay, let's recognize that. When I put an aside view, a top view, and I go for an IO as well. I drop those down in scale a bit. They're a little too big. Let's try 1.2. Yeah, that seems okay. Alright, with the EO view you always like to have that shaded. And for the purposes of this drawing, we don't really need hidden lines. We can see enough detail there. That's okay. All right, that's looking good. Let's go ahead and add some dimensions then. So we come to annotate, click the dimension tool. Alright? I'm going to dimension the total width of this part, just 60. Now, immediately, we can see there are two decimal places and also using a comma, okay? So if we want to change that, again, we'll come on to manage Styles Editor. Will come under dimension, open that up, come under the default. So in this case, the ISO. Then we've got some units here. So I'm going to use a period as the decimal marker. And in terms of precision, I'm just going to go for one decimal place. All right, we can do the same there if we're using angles as well. So saving clothes. Okay, so I got my period and just one decimal place. Now I'm going to go ahead and add in the remaining dimensions. Now here we want to identify the dimension of this inner radius here. So I'm going to select that radius and just come out. Inventor will automatically recognize that and put an R in front of the number, so it's radius. In this case, it's a two mill radius. Press okay. Now I've got the same radius on both sides. Not really that necessary, but just for clear communication. I'm actually going to enter by two indicates that both those radii R two mill come on a dimension, I'm going to do exactly the same for the outer radius. So in this case, it's four, double click on that, but times two. Okay. And now I want to put in this angle here. I want to put in a tolerance on that as well. So dimension between these 290 degrees is looking good. I want to take off one of these decimal points, so manage styles editor. Come on the dimensions again, and then one there. And I want to put a dimension on this, so I'm going to double click and here I have a lot of options. So I can come under precision and tolerance. I can put in a symmetric tolerance there. So yeah, plus or minus. And in terms of degrees, let's just go for for one degree. That's okay. We can see we've added that tolerance in there, and you can do the same with linear dimensions as well. So if I double click this, we can choose the types. I go for a deviation. So in terms of the overall height of this thing, we can put that at zero. So that's the maximum it can be a 60 millimeters, and that could drop down to. Let's put minus let's go 1.4 mill. Okay? So that can then drop down to 58.6 millimeters, but only has an upper tolerance of 60. Okay, ain't going to round off the dimensions for this final piece. Now, for the Shampa here, we could use the dimension tool, but in this case, I'm going to recommend using the ShampTol. This is just really useful. So we click the ShamfTol we select the Shampa itself, and then we select the reference edge. So in this case, I'll select this vertical edge. And here we can see that inventors then calculated as to what that Shampa is. But in this case, it's a ten mil Shamp by 45 degrees, so it's ten mil vertical and ten mil horizontal. Okay. I'm going to also add in center mark as well. I'm going to do that on the through hole, so I click Center Mark just here and add that right there. And then if I delete these two dimensions, we'll see a bit more clearly the center mark right there. Another useful tool is to add text, Okay. So anything we want particular to highlight or make a note of, we can select the text tool, which is under the Annotate tab, click anywhere. Here, we can change the font, the size as well. We can make it bold, et cetera. Then we can reposition that, so just hold it down, put it in an appropriate place. Okay, that's looking good. Now let's go ahead and add the final sheet, which is the locking pin. We double click on that. Put it in a base view, find the locking pin, locate the file, click open, put it in an IA view and a side view, change that scale. In this case, I'm going to use two, position those. Okay, so that is a very quick overview of the basics of putting together a drawing. So we just have a quick recap. We've got the assembly sheet here, identifying each other parts, and then we go into those individual parts. So sheet two, we're identifying the bracket, according dimensions, tolerances, any notes we can make. And you can add to this with more information that you need. And on the third sheet, I've got all the information of the pin. Okay, I hope you find that tutorial useful. And yeah, any questions, please put them in the comment section and I'll reply as soon as I can. Aside from that, thank you very much and have a nice day. 65. Section Introduction - Practice Exercises: This section includes a series of practice exercises that utilize the various tools covered in previous lectures. These exercises were created for students in the USA to practice and prepare for CAD exams. They received a lot of positive feedback and are intended to be beneficial to you as well. Each example is explained step by step, detailing the tools and techniques used to generate these sketches, models, and assemblies. 66. Sketching & Extrusion Modelling: In this tutorial, we will draw this part in four stages. In the first stage, we'll model the base, and in the second stage, we'll model the back feature. The third stage will be this feature, and the very last stage will be this rib feature here. So let's go to start a two D sketch, and we'll start this on the base plane. That's the X z plane. I'm going to rotate the ViewCube anticlockwise, like so. I'm going to use the rectangle tool. We'll start from the origin, and we'll use the dynamic input boxes to enter a length of 96 and a width of 64. Like so. And then we'll use the create line tool. We'll draw a straight line here. So this will be the slot that's cut out. So that's 20 millimeters in length. Hold down the left mouse button to draw in our arc, then close off that sketch like so. I'm going to dimension this arc here. So this is a radius of 16/2, so that's eight. Then we'll position this according to this line here directly in the center. So that would be this dimension divided by two, let's enter, there we have our slot in place, and this feature is now ready to be extruded. So we'll go into three D model, select extrude, select that profile there, and we'll extrude that by 16 millimeters according to the drawing. We'll press Okay. Go to the home view, and there we have our base of the part here. Next, we have the back feature. We're going to draw on this face here, create a new sketch. Draw a rectangle for this, start in this corner. Like so. I'm going to use the colinear constraint. You position this line collineally with this line here, and then go into dimension between these two lines as 16 millimeters. And there we have fully constrained that sketch. So again, we've got a three D model, and we'll extrude that, and that is at a height of 30 plus 34, that's 64 -16. That's 48. Press Enter. Then we need to put in this Shapa feature on this edge here. So to do this, we'll select the Shafer tool. And here we'll select two distances because as we can see in the drawing, we have one distance being 20 millimeters and the other being 30. We'll do distance one as 20, distance two as 30, and then we'll select the edge just here. Yeah, we can see those are the correct dimensions and press Okay. And there we have the back feature. Now on to the third stage. So we'll draw this on this face here. Go create sketch. And for this, we'll use the line tool, start in the corner here, and we'll come up at 26 millimeters, come across at 40 -24/2, that's eight. And then again, we'll hold down the left mouse button and put in our arc. That can be any dimension for the time being. Do the other eight millimeter flat there, come down to this line, and then we'll just close the sketch like so. Dimension this arc here, so that is a radius of 24/2, that's 12 millimeters. And there we are fully constrained that feature. So we go to extrude that. So like the profile flip the direction, we'll extrude that at 64 -22. That's 42. Press Enter. We're going to the home view. Now we just have the final feature, which is the rib feature. So again, we'll rotate the model. We want to draw on this face here. So left click the face, select Create sketch. There are different ways to draw ribs. Go to use the line tool for this one. Come up the corner here, join to this corner, this corner. Then I'm going to right click Select close. Now I fully defined this profile here. So we're going to three D model and extrude that. Again, we'll flip the direction, we'll extrude that at a distance of 12 millimeters as in the drawing. We'll press Okay. We'll go into the home view, and as we can see, we have now modeled this part completely. If you have any questions, please post them in the comments section, and I will respond as soon as I can. I'll see you in the next tutorial. Thank you. 67. Sketching & Modelling Utilizing Fillets & Radii: In this tutorial, we will model this part in three stages. First, we'll start with the base feature, then the more complex feature, and finally, we'll draw this front feature just here. So first, let's start a two D sketch or select the X z plane. I'm just going to rotate the ViewCube anti clockwise 90 degrees. I'll start with the line tool from the origin, we'll draw in the width of this part, which we can tell is 60 millimeters. Then we'll draw in the length of the square section, which is 70 millimeters. And then we need to draw in this arc of 60 millimeters. So hold down the left mouse button. We'll draw in the arc like so, and then we'll finish off this sketch, select ok. And here we are fully constrained this sketch. We need to draw in the through hole. So for this, we'll draw a circle on the concentric with this arc here. So the diameter of this is 16 millimeters. And then we can go ahead to the three D mol tab and extrude this profile here by 10 millimeters. That's correct. Then we just need to put in the cut out of the back section. So for this, we'll go onto the front view, and we'll start a sketch on this plane here. We'll draw in a rectangle starting from this corner. So using the dynamic input boxes, we have the dimensions 8 millimeters, and that would be ten minus six, so that's 4 millimeters. We'll go into three D model, and we'll extrude that. Profile has already been selected, and we'll select the cut output here, and we'll select through all. So here we're cutting through all of the available geometry. And there we have the base feature, so that is stage one complete onto the more complex feature. So for this, again, we'll go onto the front view, and we'll select this plane here, create a two D sketch and here we use the line tool, so we can start anywhere on this line. That will come up by 13 plus 32, so that's 45. And then we have a arc feature. So again, I'm going to hold down the left mouse button and draw in my arc and just roughly finish that summer over here. Right click, press Okay. And then I'm going to dimension that arc. So that has a radius of 20 millimeters. And then I'm going to put in the through hole about the center point of that arc, which is a diameter of 18 millimeters. I think so. And then I'm going to select the vertical constraint tool. I'm going to select the endpoint of this arc and the endpoint of this line here. And then I'm going to draw a line which joins those two together. And finally, I just need to put a dimension in from this line here and to this line, which is 20 plus 12 plus 32 millimeters. Then we have fully constrained our sketch, so we can go to three D model, and we can extrude that or select the profile, rotate the part like so. Then we extrude that. I'm going to select two. In this case. I'm going to select this plane here. There we go, and we'll select Okay. And now we just need to cut out this section here. So for this, we'll draw a sketch on this plane. Left click once, create sketch. I'm going to put it in a rectangle here that we can put it in any dimensions, and then we'll dimension the width to be that will be 60 -7.5 times two, so that's 45 again. And then the distance from the edge to the outer edge. So the wall thickness of this loop is 7.5 millimeters. And then we'll dimension the bottom of this rectangle to the base here. That will be 13 plus ten. That's 23 millimeters. And then finally, we just need to dimension this line. It can be any dimension, providing that this top line is above the top line here. And so we will extrude, select that profile, and again, we'll select the cut output. I'll select through. As you can see by the preview, this is correct. We'll select okay. And from here, we need to put the through hole in on this surface. We'll select here, create a new sketch. I'll select the circle tool. We'll input the circle here, which is 18 millimeters diameter. Then I'm going to dimension that from this line here. So that's 30/2. It's 15. I'm going to dimension that from this top line here, that is 45/2, 22.5. We're going to three D model again extrude cut and again through all. That's okay. There we have our through hole there. We have one more through hole, which is on this face, and so we'll select here. Create sketch again. But in the circle, this time it's 10 millimeters diameter. I'm going to dimension that from this edge here. That will be 30/2, that's 15. Then from this bottom edge here, we have a dimension of 15 millimeters as well. So again, we'll extrude, cut through all. That's okay. There we have our through hole. So just onto the last stage, which is the front feature, which is just here. But this we'll draw on this plane here, select the create sketch, and we'll draw in a rectangle, starting from this bottom corner. We'll finish it over here. We'll select the collinear tool, select this line. Make that collinear with this edge here. Then we'll select the dimension tool, and we'll dimension from the top to the baseline at that's 13 millimeters according to the drawing. And then we just need to input the arc. So for this, I'm going to use the circle tool instead of the arc in this case. I'm going to start the circle at the midpoint of this line here. I'm going to draw it down until it's concentric this line here. I'm just going to make sure that's concentric. There we go. I got a three D model to extrude. We're gonna select the according profiles. So the profiles we want to extrude are these two here, and the distance is 12 millimeters. That's Okay. And there we have our completed part. If you have any questions, please post them any comments section, and I will reply to them as soon as I can. I'll see you in the next tutorial. Thank you. 68. Extrusion Techniques for Removing Material: In this tutorial, we will draw this part in three stages. The first stage will be the center and the front extrusions. The second stage will be the rear features, and finally, we'll input the through holds and the rib feature. So let's start a new two D part. We'll go to start TD sketch. I'll select the base plane here, which is the X z plane. And first of all, we're going to draw two circles at the origin. The very first one here has a radius of 30 mill, that's 60 mill in diameter. Then the concentric circle to that has a diameter of 40 millimeters. We can go ahead and extrude that profile there, that is at a height of 60 millimeters, yet, which is correct. We're then going to rotate that part. Going to draw a sketch on this plane here. So here we'll draw another two circles, and this will be the through hole here, which is 20 mill diameter, then we'll draw another circle which will have the arc in place, which is 23 mill radius. So that's 46 mill in diameter. Just use the horizontal constraint to make sure that that center point of those circles is horizontal with the center point of these circles. And then I use the dimension tool to dimension in between these two circles. We know that is a dimension of 75 millimeters. And then we just need to draw in two lines here. I draw in one line and the one down here as well. I'm going to put equal constraint between those two lines as they are the same length, and then we're going to put a tangent constraint in between this line here, this circle. And because they are equal, the same will form on the other side, and there we have a fully constrained sketch. What we can do is just use the trim tool and trim away this part of the circle here. And then we can extrude that profile. We want to extrude that in the opposite direction so we can select Drew that by 15 millimeters. Like Okay, onto the rear features. So stage one is complete onto stage two. Stage two starts on a plane that's 15 mil from the base, which is essentially this plane here. So we'll select that plane, select two D sketch. Just flip the ViewCube. We're looking at this orientation. Then we'll go ahead and model in a rectangle. We can put that anywhere for the time being. We can dimension the height of that, which is 60 millimeters. I'm going to use the constraint tools here. So we're going to use the coincident constraint between this corner point here. The center and the circumference of this circle here, exactly the same on the other side. And there these two lines are then tangential to this arc because this circle is 60 mil diameter. Well then dimension the length of this arc here, which from the center point to the back is 75 millimeters per center. And then we can go ahead and extrude that profile. That's in the correct direction. And yeah, the correct distance as well, 15 millimeters. We can then go ahead and start a new to Di sketch on this face here. We'll draw in a rectangle. We'll start at this corner here. Going to use a colinear constraint between this flat line here and this flat line. Then we'll dimension between these two lines as 15 millimeters. Then we'll go ahead and put in one more rectangle like so. Just mention this. So that is 10 millimeters. Going to put in a coincident constraint between this endpoint and this circle, exactly the same between this endpoint and this circle, and then we know it's positioned in the center. We can then go to three D model and we can extrude those two profiles there, so we'll select both of those. We'll extrude those at a distance of that's 45 -15. So 30 millimeters let's enter. And there we go. That's the rear feature. Now we'll start to put in the through holes at the back. So for this, let's rotate the model and we'll start the sketch on this face here. The two circles, drawing these anywhere. I'm going to put equal constraint between the two. I'm going to dimension one of them as a diameter of 16 millimeters and due to the equal constraint, they will now both be 16 millimeters. We know that the distance between the two center points is 35 millimeters. Then we know they're positioned in the center, so we can distance the center point of this circle to this endpoint. That end line as that would be a open brackets for this. There's 60 -35. That would be then half then we use the horizontal constraint between the two center points, ensure they're in the correct position. Then finally, we'll just dimension them from this top line here, which is 15 millimeters. There we are. They are fully constrained. We can go ahead to three D model and extrude those. We'll select both the profiles. Then we'll select the cut option. And under distance, we'll select two. Then if we rotate the model, we will extrude to this face here. That's okay. There we have our two through holes. Okay, onto the very last feature, which is the rib, which is just between these two parts. So for this, we'll go to the model browser. We'll click the plus icon next to the origin, and there we have the three default planes. So we'll select the XY plane here. We can right click and select New Sketch. And here we will draw our rib feature. So I'm just going to draw that in roughly, explain why shortly. We'll then dimension that. So the baseline here is 25 millimeters, and the vertical line is 40 millimeters. Like so. And then I'm going to put it in a coincident constraint between this endpoint and this line here. Then we just need to position this accordingly, so we need to move it roughly over here. However, if we only touch this endpoint to the circumference of this circle, the rib will not be in full contact with the face of the circle. And so what we're going to do here is we're going to draw in a new line we white the way down, then we'll right click on that line, add it as a construction line. We're going to dimension. I just rotate the model here. I'm going to put a dimension between the endpoint of this line and our newly found construction line input then 0.5 millimeters. And then let's have a look at that from the front face. So we can see here that our line is now essentially in the circle that we already have. Let's go ahead and extrude select that profile. Under direction, we'll select symmetric, and under the distance, we can see here that the wall thickness is 10 millimeters. Then we'll press Enter. And as you can see here, because the sketch was inside this geometry, we've now got this nice arc going on here. If we go to the home view, you can see we have now completed our part. If you have any questions about this tutorial, please post them in the comments section and I will answer as soon as I can. Thank you very much, and I'll see you in the next tutorial. 69. Multi Stage Modelling - Parts: In this tutorial, we will model this part in three stages. Stage one, we'll draw the cylindrical feature at the bottom, and stage two, we'll draw the upper feature, and then stage three, we'll draw the join to finish it off. So let's start a two D sketch. And for this, we'll start on the Y Z plane. We'll start with those two circles at the bottom for the cylindrical features, so like 60 mill diameter. Then there is an inner one of 32 mill diameter. We can go to three D model and we can extrude that, select that profile. That's an extrusion of 50 millimeters, which is correct. For the second stage, we'll do the upper feature. So for this, we'll draw on this plane here, the left click once, create a sketch, and then we'll start with the through hole and the arc. So for this, the through hole has a diameter of 20 mill, and the arc has a radius of 20, so that's a diameter of 40. Let me use the vertical constraint, the center point of these circles to the origin. I'm going to use the dimension tool between the center point of the circles and to the origin as 80 millimeters. Then we'll just finish this off with the line tool, so we're drawing these two lines which connect these two circles. We use the tangent constraint. Make sure those lines are tangential to both circles. Then we use the coincident constraint, make sure there is contact between the endpoint lines and the circles. Then we're drawing the flat across here. That is a dimension from the center point of this circle to the line of 40 millimeters. Now we have fully constrained our sketch. We've got a three D model and we'll extrude those profiles, flip the direction. Again, the 50 millimeter extrusion is correct. There we go. Now we need to extrude cut the section out here of this feature. So for this, we'll go into the plus next origin or select the correct plane, which is the XY plane, right click New sketch. Drawing this rectangle. And notice that I can't see the sketch behind this feature. So for this, we'll hit F seven on the keyboard. We'll dimension that accordingly. So from this line to the edge is 50 -25. That'll be divided by two, so that's 12.5. As for the width, we have 25. And from the line here to the center point of these circles is 25 millimeters. So for this, I'm going to project the geometry of the two circles. I'm going to draw in a construction line from the center point of those two circles. Going to select that line and put in a lock constraint. Then dimension between the center point of the circles and this line at 25 millimeters according to the drawing. Then finally, we can put in a dimension for the height, which can be, let's just say 60 millimeters, in this case, as long as it covers all of the geometry we wish to cut the three D model we'll extrude, select both profiles, both directions. That's cuts through all there we go. There we have the cut out center section. And finally, we just need to put in this join. So for this, we cannot use an existing plane as none of them are in the correct location. So we'll go to three D model, go on the drop down and mid plane between two planes, we'll select this as our first plane. This is our second plane, and there we have a plane for us to draw on. So let's left click once on this plane. Create a sketch. Then we'll just draw from this endpoint here to this circle, then exactly the same on the other side. Let's use the tangent constraint again between the lines and the circle. And now we are fully constrained. Also going to project the geometry of this circle and this line here. Let's go on three D model and extrude that profile. We want that in both directions. It has a total width of 15 millimeters. Let's enter. I'm going to right click on the working plane, turn the visibility off, go to the home view, and there we have our completed part. If you have any questions, please post them in the comments section and I'll reply as soon as I can. I'll see you in the next tutorial. Thank you. 70. Modelling with Pitch Circle Diameter: In this tutorial, we will model this part here. So I've started a new part. We'll go to start two D sketch, and we'll select the base plane here, which is the X z plane. For this, we'll start with the bottom feature, which is the flange. So we'll start at the origin. We'll draw that circle in at 100 millimeters diameter. We'll then draw the through hole in. So again, start from the origin as a diameter of 30 millimeters. Then we need to place our mounting holes around here. So these are placed on a pitch circle diameter of 70 millimeters. I'm just going to right click on that and slat construction. We'll use the circle tool, and we'll draw in the first through hole, which is 12 millimeters. Then we'll just use the vertical constraint between the center point of this circle and the origin, and then it's fully defined. Then we can use the circular pattern tool, select the according geometry. So that's this circle. And then for the axis, we'll select the center point here. Six instances is correct and at a angle of 360 degrees, so we'll select okay, there we have our fully defined sketch. So we can go to three D model, we can extrude this, like the profile, and that's at a distance or 15 millimeters. That's correct. Press Okay. Now we need to draw in the cylindrical part. So for this, we'll select this face, create sketch. Go to the circle tool, start from the origin, and that has a diameter of 50 millimeters pre center. Then we just need to project this circle here to maintain that through hole. Three D model extrude, select that profile, and that's extruded at a distance of 70 millimeters. Press okay. And then we just need to draw in the final feature. So for this, we'll draw on this plane here, a left click once, create sketch. Then we'll start by drawing in the arc and through hole circle. So the through hole circle is a ten mil diameter, and the arc has a radius of 13, that'd be 26 mil diameter. We'll draw the exact same on the other side and use the equal constraint between the inner circles and the outer circles. These circles have a distance between one another at 100 millimeters, which is the diameter of this outer circle here, so we can use the coincident constraint between the center point of these circles and this circle here. Then finally, we just need to put in the horizontal constraint between this circle and the origin and this circle and the origin. We'll then go ahead and project these two circles here. So that's the 25 mil arc, you can see in the model, and also this through hole here. As I say, we need to maintain that. Then we go on the line tool. Just drawing some rough lines which we will go on to use the tangential constraint afterwards to put them in the correct position. So select the tangential constraint and strain this line to this circle, like so, and then to this smaller circle as well. Just before we extrude that, I'm going to right click on this circle, select it as a construction line. Then we're going to three D model and we'll extrude. This I'm going to look at the top view. To select the according profile, so we need these two circles. These two parts, this part here. Home view. That's correct. And that's an extrusion distance of 15 millimeters. That's okay. Look at it from the home view. There we have our completed model. If you have any questions, please post them in the comments section, and I will reply as soon as I can. I'll see you in the next tutorial. Thank you. 71. Tactical Sketch Modelling & Extrusions: In this tutorial, we will model this part here. So let's start by starting a two D sketch on the base plane. So that's the X z plane. Then we'll start with the arcs at the rear side. We'll start on the origin, and that has a radius of 25 mill, so diameter of 50. And then at the front, we have also arc with a radius of 25, so we're drawing a 50 milliameter circle. I'll use the horizontal constraint between the two center points, make sure they are aligned, and then our dimension between both circles at 60 millimeters, like so. Then we can use the line tool. And we'll join these circles together by the top quadrants and also by the base quadrants as well. Then use the tangential constraint, make sure the lines are positioned correctly. There we go. Fully constrained sketch. And then we use the trim tool for these two arcs here. Take those out. Next feature, we'll input the slot. So we'll take the center to center slot tool, and that starts at the center point of this circle or start there. It has a length of 12 millimeter. Then it has a radius of six millimeter, so we'll enter 12 mill there. Like so. And then we just need to enter the through hole on the other side, which has a diameter radius of ten mil, so diameter 20 mill. And that sketch is now fully defined. We can extrude that profile, select that profile, and the distance is 12 millimeters. That's okay. And now we need to take out the slot on the underside. So for this, let's choose the appropriate plane. In this case, it's the Y Z plane. So we'll right click there, create a new sketch. And for this, we'll draw in a sort of two point center rectangle. We'll start that at the origin. There's a total height of six mill, this slot does, so we'll then put 12 mill there. And then for the length is 20 millimeters. We've drawn that in place. We've got a three D model extrude, and that profile has been selected. We'll select the Boolean cut, and we'll do that in both directions, and we'll go through all. If we rotate the part, we can see that's taking out the correct geometry. We'll press Okay. There we go. That's our slot on the underside done. And now we need to do the extrusion about the slot here. So for this, we'll draw on this plane, create a new sketch. I'm going to project the geometry about this existing slot. I'm going to use the offset tool and offset that. So the outer slot has a 12 milliradius, so we need to offset that by 6 millimeters. Then we can go on three D model and we can extrude that profile there, and that is a height of 4 millimeters per center. There we have our slot extrusion just here. Now the last feature is on the rear side, so we'll draw this on the same plane. We'll draw in a circle radius 25 mill or 50 milldiameter circle. Now, through holes already there, so let's project that geometry, then we can three D model and extrude that profile. We'll extrude that by that's 20 millimeters. Center. Now we need to take out the slot in the center. A number of ways to do this. Let's draw on this face, reach sketch. And for this again, we'll do a center two point rectangle. Let's draw the total length that's 70 millimeters. And for the width of the slot, it's 12 millimeters. There we can go to three D model and extrude, select that profile, select cut, and the distance there is 6 millimeters. I say okay. And there we have our completed model. If you have any questions, please post them in the comments section, and I will reply as soon as I can. I'll see you in the next tutorial. Thank you. 72. Sweep Modelling: In this tutorial, we will model this flanged pipe bend. So let's start a two D sketch. We'll start on the XY plane. The first of all, we'll sketch in the path to which we will sweep. So we'll start with a line from the origin and draw that horizontally at 150 millimeters. We'll then use the tangent arc, start that from the endpoint of this line. We'll use the dynamic input boxes here. So the sweep profile has a radius of 260 millimeters, and it is a 90 degree bend. So enter 90. That's okay. Then we just finish off that path with the line tool, the vertical line at 150 millimeters. That's our path complete, then finish the sketch. Now we just need to put in the profile which we'll sweep across. So we'll go to the plus icon next to the origin folder, and we'll select the plane that's perpendicular to this sketch. We'll right click on the YZ plane on new sketch, select the circle tool, start from the origin, and this will be the outer diameter of the pipe. So we can see that's 290 millimeters. And then we'll just finish the sketch there. We'll go to three D model. We'll select our sweep command. Profile has correctly been selected. And then we need to select our path, which is the path we drew here. And the preview here is correct. Press Okay. And then we'll choose the shell command, we'll select the faces to remove. Then we'll select the wall thickness, which is 290 -210, which is 80, and then we'll divide that by two. But that's 40 millimeters. We'll press Okay. We have here our completed pipe section. We just need to add in the flanges. So add in the flange here first. I'll select this face create sketch. And for this, we can use the two point center rectangle from the origin. This has dimensions of 360 length by 360 height, enter. Then we just project the inner diameter there with which we will three D model and extrude that profile. But this has a thickness of 50 millimeters, that's in the opposing direction, so we'll flip that. We'll just make sure that the output boolean is joined, so we're adding material here. It's okay. It's our first flange face. We do exactly the same on the other side, create sketch. For this, we'll project this inner circle to use its center point Use the two point center rectangle tool again, 360 by 360. Then three D model extrude that profile, flip the direction. Want to add material, select o. Got our two flanges now, we just need to input the mounting holes. So let's start on this face here, create sketch. And we can see that the mounting holes are 260 millimeter spaced and 50 millimeters dimensioned from the edges. So here we can use, again, the two point center rectangle from the origin, and this has 260 by 260. And then we know that each of these corners is one of the holes. So we'll just draw in one of the circles, draw on this corner here. But this is the larger circle, which has a diameter of 60 millimeters. And then we can use the circular patental for this circle or select the axis to be the origin and the number of instances to be four press Okay. We'll then select the square lines, right click Add them as construction lines, and then we can go ahead three D model and extrude the four circles there. So we want to subtract material, and the depth of this 60 millimeter hole is 10 millimeters. Okay? And then we just need to do the through holes. That will be on this face here and create a sketch. I'm going to project the inner diameter of the circle so we can later use the center point there. Or use the circle tool. We'll make that concentric with this hole here. That's a diameter of 30 millimeters. Then we'll go ahead and circular pattern this hole around the center point of this circle with four instances. I'll press Okay. Then we're going to three D model, and we will extrude or select those four circles. Then we just go extrude cut, and we'll select to rotate the model, and we'll cut to this face here, like so. We'll select kay. Then we have four mounting holes on this flange. Then we do exactly the same process on the flange at the top, create sketch. Go to project this circle here. G to draw in the two point center rectangle 260 by 260. D in one circle on the corner, 60 millimeter diameter, a circular pattern, that geometry, about the center point, four instances, press o. I'll make that square construction. We model extrude. I just select those individually, so one, two, three, and four, we will extrude cut by 10 millimeters. That's correct. Then we'll just draw in the through holes. Again, I'm going to project that geometry. Use a circle tool, concentric with the existing circle, 30 millimeters, circular pattern, select that profile, select the center point of the larger circle as the axis, and four instances, press oa3d model, select those four circles. We'll subtract material, and we'll go to, and we'll select this underface here. Okay. There we have our flanges complete. Next thing to do is to add in the Shampa of the inner diameter of the pipe. So we select edge, this edge here. That has a Shampa 10 millimeters press. Okay. And the very last feature will be the fillets on the edges of the flanges. So we'll select each of those edges. Then we'll input the radius of 20 millimeters, okay? And there we have our completed model. If you have any questions about this, please post in the comment section, and I will reply as soon as I can. I'll see you in the next tutorial. Thank you. 73. Visual Thread Modelling: In this tutorial, we'll model an M 12 hex head bolt. So to do this, let's start a two D sketch. We'll start this on the Y Z plane. We'll start by going into our drop down and we'll select the polygon tool. Start this at the origin, and we'll draw in a six sided polygon. We'll click Done. And then we'll dimension the WAF. That's the width across flats as 18 millimeters. I'm just going to put in a constraint between the top point and the origin, and then it's fully defined. Let's go to three D model and extrude that. We'll select that profile. We'll extrude that head by 7.5 millimeters. Okay. And then we'll put in the rounds on each of the edges. So to do this, let's start on this plane, start a new two D sketch. We'll draw in a circle starting at the origin, and then we'll put in a tangent constraint between the circle and any one of the flats. That should be fully constrained as so. And then we'll go to three D model, and we'll select Extrude. We'll select that profile. And in this case, we will intersect with the existing hexagon. But we'll put in a taper of 45 degrees. And so anything that this extrusion will intersect, we will keep. So essentially, this is a technique in which we can add in the rounds on each of the corner points. Select the okay, and there you can see, we have those faces here. Okay, onto the other side, so we'll create the shaft and add the thread on this face. To do this, we'll sketch a circle again at the origin, and this is an M 12 bolt, so that's a 12 mill diameter circle. We got a three D model. We'll extrude that. It's M 12 by 40 mil length. So we'll add put zero on the taper, and we'll add 40 mil to the length of the stud. And then we will use the fillletTol on this edge here. We'll put in a one mil fill and then we just need to put in the champa on this edge here. So this is 12 -10/2, so that's a one mil champs Okay. And last of all, we just need to input the thread here. So we've got a three D model. We'll select the thread command, have our dialog box pop up here. So let's select the face, which is this one here. Then let's select the type of thread. So typically, I would use an isometric. I'll select that one, and it's an M 12 thread. And here we can choose the pitch. So I'm going to choose a 1.5 mil pitch, and then we'll select Okay. And that concludes I the model our M 12 by 40 fully threaded bolt. If you have any questions, please post them in the comment section, and I will reply as soon as I can. I'll see you in the next tutorial. Thank you. 74. Revolve Modelling: In this tutorial, we will draw this part here. So this is somewhat similar to a piston head and can be modeled using a single sketch profile and the revolve feature. So let's start a two D sketch. We'll start that on the XY plane. We'll start at the origin, drawing a vertical line, which will be the radius of the inner arc there, just 13 millimeters. Then come across for our taper. Then we'll dimension between the endpoint and the origin, the width of the part, which is 50 millimeters. Then again, we'll dimension from the origin to the endpoint of that line. It's radius, which is 19 millimeters. Back to the line to the end point of this line, we'll go vertical here, that's 80 millimeters. Then we need to put in our two grooves. So here we'll come across eight mill. We'll drop down by six. Then the width of our groove is 12 mill. Come back to the top six mill. The distance between the two is 50 -24 -16, that's ten. I'll come down with the six mill. The width of our second groove, 12 mill, back to the top will be six mill. Then finally, we can finish off the profiles there with eight mil dimension. We'll put in the vertical line here. Now just put in a vertical constraint on these two lines here which are not fully defined. Now they are fully defined to a dimension between the endpoint of this line and the origin, that will be the radius there, which is 79 millimeters. Back to the line tool. Come across horizontal, we don't know the length of this, but we'll put in the lines like so. Then we can use the dimension between this flat and this one here as 20 millimeters. Then we just need to put in another taper here, which will be parallel. So we'll select the parallel constraint with this slide here. So we'll select both of those lines. They are now parallel. And we'll also put in the vertical constraint between the origin and the endpoint of this line here. So then we just need to dimension the radius of this arc here, which is 33 millimeters. Then we can use the line tool to finish off our sketch profile. Finally, we'll put in another line starting at the origin, going horizontal. Put that as a construction line. Then we'll go to a three D model and we'll revolve this profile about our axis of revolution here. So let's select revolve. Inventor has correctly selected this profile here. We'll then select the axis this construction line. Then we can see the preview of the part is correct. Need to change the angle here to 270 degrees, and we'll flip the direction. Like so. We'll click. Okay. There we have the completed part. If you have any questions, please post them in the comments section, and I'll reply as soon as I can. I'll see you in the next tutorial. Thank you. 75. Advanced Sketch & Modelling: In this tutorial, we will model this part here. You'll see that I have not used dimensions in this part, and that is because there are just too many dimensions to input into a single schematic, such as above. And so for the dimensions, feel free to either pause or play the video in slow motion, then you'll see the dimensions as I put them in throughout the model. So having a look at this model, it's slightly complex. We have a number of sort of mating components and quite an awkward flange geometry there. So let's begin by drawing that. Let's go on TD sketch. Start a TD sketch. We'll start this on the z plane. And we'll start with the larger of the two circles, which has a rat of 52.5. We'll multiply that by two to give the diameter. And then we'll input the PCD, so that's a pitch circle diameter that lies on a 90 1 millimeter that's a 91 diameter millimeter circle. Put that as a construction line. And then we just input some of our through holes here. So on the top quadrant of the PCD, we have eight millimeter diameter circles. So I just use a vertical constraint between the center point and the origin. That's now fully constrained. Then we'll circular pattern, this eight milldiameter hole about the origin, when we use eight instances which are equa spaced across 360 degrees of revolution. Okay, there we have our mounting holes. We're also drawing the through hole here. So this has a Oh, sorry, this will be the inner diameter of the pipe, which in this case, is 30 millimeters. And now that's fully constrained. So we can move on now to the smaller circle to which we'll draw in. This has a rad of 40 mil, so that's a diameter of 80. It's also got a pitch circle diameter of 66 mil. Just going to right click and identify that PCD as a construction line. And now we need to position this. So this circle here is positioned 30 degrees. So to do this, let's draw in two lines on a larger circle. One horizontal and one at a angle like that. We'll then identify these as construction lines, and we'll put in a 30 30 degree angle between the two. Then we'll just draw in a construction line on this circle here. I'm going to put a collinear constraint between this line here and this line. And then we know that this circle here is constraint to this 30 degree angle. And then we'll put a dimension between the two center points, and that will be 91 millimeters. Okay, so our circles are positioned. We're now putting through holes on this PCD here. We'll start at the top quadrant, and again, that's 8 millimeters, and there are eight of them, then the vertical constraint between the center point and the center point of the larger circle. Circular pattern of this circle and for our axis, which is the center point, eight instances, and again, aqua spaced across 360 degree revolution. Well, then choose a line tool. We'll just join up these two circles. I use a tangent constraint to put this line in the correct place. And then on the other side here, we have a that's an eight millimeter radius. So for this, I'll draw in a circle of 16 mill, and I'll put that circle tangential to both the larger and the smaller circles here. And then we'll use the trim tool to tidy this up a bit because the sketch is getting a bit messy. So we'll take out the lines that we don't need. I want to take out this line here. And they're going to take out this 16 mildimension, which was the diameter, and we'll put in the ad of eight mill. We'll also put in the through hole of the pipe, which will spawn from this area here. So again, that's 30 mill diameter. And now we are ready to extrude our flange face. So we'll select that profile, and we'll extrude that by do 10 millimeters. Press okay. Okay, that's looking good. And now we need to sweep for these two pipes. So for this, we can use the XY plane, do a new sketch on here. I'll start the line from the center point, this circle, which I'm going to project the geometry of. Choose a center point of this line, like so. Go back to the front view. I'll draw a vertical line, and then draw in an arc come across like so. Use a tangent constraint between the arc and this line here. We'll put in the radius of this arc here, which is 40 millimeters. We'll put in the dimension from the endpoint here to the base point. That is 60 millimeters. Then we'll finally just put in the dimension from the endpoint of this line to the origin there at 143 millimeters. And that sketch is now fully constrained, so we can finish that sketch. We can start a new sketch on this plane. We'll draw on the circle. So this will be the outer diameter of the pipe, which in this case, is 40 millimeters. We've got a three D model, and we'll sweep, select our profiles. Select both of these profiles here. Select the path So yeah, looking at the preview, that's correct. No press. Okay. And then next we'll draw in the flange, which is just positioned here. So for this, we've got a three D model. We'll offset a plane this plane here. I'll be in the minus direction. I'd be -3 millimeters. Then select that plane. And we will create a two D sketch. We'll use the two point center rectangle for this tool. We'll start from the center point, the dimensions of the flange are 60 by 60. Then you need to put it in our fillets. So the fillets are, sorry, the rads on the corners a eight mill radius. I'll select each of these corners, like so. Right click. Press Okay. I'm just going to hide this plane. Now we start to drawing the mounting hole. So let's draw in two of these. They're all 8 millimeters. Constrain them to these lines here. Then we dimension between the that's the wrong dimension. Dimension between the two center points. As 44 millimeters, and then we'll put it in a vertical constraint, again, between the two center points, and now they're fully constrained. We're just going to mirror these across. We'll draw a vertical line down, put that as a construction line, and we'll go to mirror, select that two circles for the mirror line, construction line apply. Now we have our circles. We can go ahead and extrude that flange extrude that in the opposite direction. And this has a depth of 8 millimeters. Okay. Then we have our flange face there. Just gonna put it in the fillet detail on these two edges here. They'll both be 3 millimeters. Okay. And now we need to draw in the other pipe, so we use the same method here, so that'll be the sweep command. So first of all, let's start by drawing the path. This we'll need to input a new plane. So we need to cross this with a point that we'll input, which will be at the center of this circle here. So we'll project that geometry, put in a point. Just going to finish the sketch here. Then going to input a new plane, be parallel to an existing plane, and it will go through the point which we just drew in. So we'll select parallel to this plane, and we'll select this point here, and as you can see, we now have a new plane in which we can sketch on. We do two D sketch. Start with the line tool. And before we do that, I'm going to hide this sketch here. We no longer need that.G to sketch 14, edit that sketch. I'm going to project the geometry of this circle, so we have a flat line. Then from the center point of this flat line, I'm going to draw vertically, like so, and I'm then going to put in a arc. I'm going to make a horizontal constraint between the endpoints of this arc. I'm gonna put in a vertical constraint on this line here as well. That's dimension this RD here. So this is 22.75 millimeters. Then we need to put in a distance of this line here. So this 85 from the base. So I'll select the top point in the base here at 85 millimeter. I'm going to hit F seven on the keyboard, get a cross section view, see what's going on here. I'm going to extend this line down to the origin. So to do this, I'll project this geometry. And then continue this line to the origin like so. And that's our path complete. So we'll finish the sketch there. I go to hide this plane, so right click, press V. Let's draw our profile to which we will use to sweep. So this will start from the center point. So again, I'm just going to project that geometry. This will be the outer diameter, so we're getting 40 millimeters. Got a three D model, and we'll sweep those two profiles. I'll select the path to be this path here. Yeah, that preview is correct. Press Okay. Looking good so far. Now, let's use the shell command. There we go. Then we'll select the faces to which we wish to remove. So we'll select this face, this face here, and this face. In the thickness, in this case, so the OD is 40 mil, the ID is 30 mill that's of both pipes and so the wall thickness is 5 millimeters. Input fives okay. Then we can see we have our holes here, which is correct. You can see also the hole that the join here is correct also. Let's tidy this up with some fillets. We don't like to have these sharp edges. Put in some four mill fillets on both of these edges. Also the external ones here. And also the joins about the flange face like the ply. But one more fillet here, which I have a one mill ad on this edge here. Okay. Now we have our completed part. Just to check that it is correct, let's go to view. Let's do a half section view, start at this pace here, and we'll just run through the model and make sure everything is as it should be and particularly around the join of the two pipes here, so that is correct, exactly what we want to see all smooth edges so that we're getting lamina fluid flow, no turbulence. We'll just go back in the opposite direction. A flange. And there we have our completed part. If you have any questions about this, please post them in the comment section and I'll reply as soon as I can. I'll see you in the next tutorial. Thank you. 76. Assembly Constraining & Movement: In this tutorial, we will model a door hinge, and so we will draw the metal fabricated part, and then the pin, and then we'll form an assembly of these parts together. So let's start with the metal fabricated part. Start a new tudi sketch, here we'll choose the X z plane, and we'll draw a two point center rectangle, starting at the origin. So the length of this will be 100 millimeters. Press tab. Then for the height, we'll input 40, okay. Let's put some fillets on these two upper corners. So we'll select the filllet command. We'll put it in a five mil fillet, select these two lines and then these two. Then we'll finish the sketch there, do them out a little bit. Go on three D model, and we'll extrude that by 1.5 millimeters. Okay. Next, let's input the mounting holes. We'll draw a sketch on this face here. And for this, I'm going to draw in a construction line just to help me better position these holes. I'm going to dimension that construction line from the top line at 15 millimeters. Just right click on that that construction line. I select the circle tool, and we'll just roughly put in the mounting holes. Use the horizontal constraint between the center points of the upper circles and the center points of the lower circles, as well. Then we'll dimension one of these circles to be six mill. We'll put in equal constraint between this circle and all of the others so that they're all six mill diameter. Let's then dimension this circle from this line as five mil, and from the side there can be 12. The same for this upper circle. So from the center, 5 millimeters, then from the origin, we'll choose 12 millimeters. Same for this one here. So from the origin, 12 mil. We've already got the five mil dimension there as they are constrained on the horizontal between the center points. And for the last circle, we just need to constrain it from this line at 12 millimeters. Then we can go ahead and three D model and we can extrude cut those four profiles there. We select cut, we'll select through all. Okay. There we have our mounting holes. Let's just add a Shamp to the top edges of these holes. We'll use the ShamfTol. We'll use 0.5 millimeters or select the top edges of all four holes. Okay. There we go. We have our mounting holes complete. Now for the next sketch, we'll select this plane here, create two D sketch. We'll input two circles. The first will be ten mill in diameter. We draw a circle concentric to that at six mill diameter. Let's then put in a coincident constraint between the corner here and this outer circle so that they are touching. And then we can dimension between the center point of this circle and this line here. We'll do that at 0.5 millimeters. And then we'll select the line tool. We'll then put some sketching here. So we'll start at this corner point just to this circle. And again, we'll put another line roughly there. One more down here. And then we use the dimension constraint between these two lines. Let's put that as 1.5 millimeters. Then we can use the trim tool, trim away these two lines and also this line here. Then we can use the Fillet tool. Let's put a one mil fillet on this corner here. So this one here like soap, we'll finish the sketch there. Then on three D model, we'll extrude that profile, flip the direction, and we'll input a length of 25 millimeters. Okay. Looking good. And then let's repeat this feature. It's got a three D model, and we'll rectangular pattern, select that feature there. And for the direction, we'll select this line, but we'll flip its direction instances of two, that's correct. And then for the distance, we'll put 50 millimeters offset. Okay. I'm going to turn off the edges for this. Okay, that's looking good. And next, we need to draw the pin. So for this, let's do this on the XY plane. We'll start with a circle from the origin to be ten mill in diameter. Go on three D model, and let's extrude that by 2 millimeters. That's okay. Then we'll select this face here, left click once, create two D sketch. Again, we'll select the circle tool from the origin. We'll position this as 6 millimeters. Then three D model, extrude that by 100 millimeters. That's okay. I'm just going to put an appearance on that. Let's go with a glossy black. Okay, and then we can save that part and we can form our assembly. And here, I've opened up a new assembly file, so let's go ahead and place our parts. Select the sheet metal component first. Then we'll just input one more of these parts. We're back on place, and we'll put in the pin as well. Looking good. Let's go ahead and re rotate this part here so that it is in the correct orientation. And I'm going to do exactly the same for the pin as well. So free rotate. Rotate that roughly 90 degrees. Then we're going constrain, and we'll constrain the axis concentrically of this face here and this face, apply. Then we'll just go ahead and constrain this face here to this face here. Apply. And then we'll do the pin. So yeah, again, we'll select the axis of the pin and the axis here. Then we'll select the face of the pin and this contact face here. Apply, okay. There we have our completed hinge. If you have any questions about this, please post them in the comments section, and I'll apply as soon as I can. But I will see you in the next tutorial. Thank you. 77. Advances Modelling Example: In this tutorial, we will model a caster wheel. So typically, we would draw the parts individually and then constrain them together in an assembly file. But for the purposes of this tutorial, I'll just draw all the parts into a single part file. So let's start with the frame of the caster wheel. So we'll start a two D sketch, and we'll select the X z plane. Then we'll look at this from the top view, and we'll use the circle tool from the origin, and we're drawing a circle with a diameter of 50 millimeters. Then we'll go on three D model, and we'll extrude that profile, rotate that. Extrude that again by 50 millimeters. Let's put in a fillet of, let's do 5 millimeters on this edge here. Okay. Looking good so far. Then we want to offset a plane. So we'll offset plane, and we'll do this from the Y Z plane. We'll offset that by 32 millimeters. Look on that plane and create a two D sketch. And here we'll draw a two point rectangle. The height of this will be 45 millimeters and the width will be 38 millimeters. Let's go ahead and position that. So let's project this geometry, and then we can use the collinear constraint between that projected line and the top line of our rectangle. And then we can use the dimension tool and dimension between the sideline here of our rectangle and the endpoint of this projected line here. And here the dimension will be 6 millimeters. The cylindrical part has a diameter of 50 mil -38 mil from that, which is length width of the rectangle, and then we divide it by two. So 12 to by two, that's six. That's then fully constrained. We'll call on three D model. I extrude, select that profile. We'll flip the direction, and we will extrude that too and we will select this face here. And as of the preview, that's exactly what we're after. I said, Okay. I just want to hide that plane, so we're going to right click on it, and I'm going to hit V on the keyboard, which is visibility. Take that out. Next, we want to cut away a part of this profile. So let's start a two D sketch, and we'll do this on the XY plane. That's correct. And I'm just going to hit F seven on the keyboard. So yeah, we can look at exactly what we're drawing on. We'll draw a line from this line here to the corner point this corner point, then we'll close the sketch or dimension between this corner point and this top line here is 10 millimeters. Then we have a fully constrained sketch. Three D model, and we'll extrude, we'll select that profile. We want to extrude cut we want to extrude it cut in both directions. We're going to hit symmetric. We're going to hit through all. Then yeah, we're cutting away all of this profile here. We'll press Okay, as you can see all of that geometry there has been cut away. That's great. Now we want to apply a draft angle to this face here. If we're going three D model, we'll use the draft command. For the pull direction, we'll select this face here, and for the faces to draft. This will be at a 20 degree draft angle, which is suitable for what we're after. We'll select this face here, and we'll press Okay. And then we'll tidy this up a bit using the fillet command. Let's put an eight mill fillet, which is quite sharp for this edge here. That looks good. We'll add another fillet or 5 millimeters. We'll select this edge, this one, Arc, edge here, then this edge. Yeah, that's looking good. Let okay? The next, we need to use the shell command. So we'll select remove faces, and we'll select the automatic face chain command. So make the workflow a bit more efficient. We do a thickness of 2.5 mil. Then we'll select this face here. Because we have automatic face chain selected, it's gone and selected all three of these faces here, which is correct. We want those to be removed. We'll hit Okay, looking nice. Let's do our through hole on this face here, so this will be for the pin and for the wheel. To do this, I'm going to project this archea, and I'm going to use the circle geometry on this center point here for a ten millimeter diameter circle. I'm going to extrude cut. I'm going to select through all Okay Okay, so that's the frame complete. We now need to put in the caster wheel. So we will revolve this. So to do this, we need to input a plane. And we'll do this parallel to an existing plane and through a point. So we need to identify that point. I'm going to turn on, so I'm going to edit the sketch of these through holes, and I'm going to input a point, the center of this circle. I'm going to finish the sketch there. I'm going to turn on that sketch, so I'm going to right click and hit visibility, and now we can see that point there. Let's go and input our plane. We'll do parallel to plane through point, parallel to the W one is it? It's the Y Z plane. And then the point. I'll select this point here, as we can see that plane's in the correct position. This is the plane in which the axis and our cross sectional profile of the wheel will lie on. I'd like to select that plane two D sketch. I'm going to hit F seven on the keyboard once again. There we go. Got to turn off that sketch that we no longer need. I'm also going to hide the visibility for the plane we're working on. We don't need to see that. We're going to project these two arcs here. We're going to use the center points of these lines to input a center line. So this will be the axis of revolution. I go to trim away that line there. There we go. I want to put in a lock constraint on that line. I don't want that to move. And then we can begin to draw the cross sectional profile of our caster wheel. So let's let the line tool throw a straight line, roughly down here like soap. Then we'll put in a three point arc starting at the end point of that line. Again, just roughly over here. We'll use a radius or 40 mil then we'll draw a straight line coming down, so we're drawing that at ten mill, then we'll come across to be on par with the origin. But that's looking good. Then we'll just draw a straight line coming all the way up. Finish off that profile. I got a dimension between this line here and this line here at 1 millimeter. I'm going to put a fillet in of, let's say, 5 millimeters on these two lines here. Okay. And then I want to mirror this line, this arc, this line, this arc, and this line. I'm going to mirror them around our center line here. Press Okay. That's the cross sectional profile of our wheel. So all we need to do now is to revolve. Select those two profiles. And for the axis, this line here, review looks good. Okay. There we have our wheel. That's looking nice. I'm just going to change the appearance of some faces here. So I'm going to hold down control, select these faces, change those appearances to, let's say, red. Let's do our through hole on the wheel now, so we'll select this face two D sketch. Project this geometry here so we can use it center line. I saw CenterPoint. Draw an eight mill circle here on three D model. I extrude that profile. We want to extrude cut. I want to go through going all the way through the wheel. There we have our through hole. Looking good. Now we need to input our pin. For this again, we'll use the revolve command, and we'll do this on the plane, which we input earlier. We're doing a new sketch. I'm going to hit F seven. Directly at the plane we're drawing on, and I'm going to use the same tactic as before. So I'm going to take these two arcs, reject them. I'm going to draw a line between the center point of both these arcs. W axis of revolution. I'm a offset that line, sorry, by 4 millimeters. They're going to put a lot constraint center line there. Come over to one side, zoom in a little, and let's use the line tool extend this line here by 4 millimeters. Want to select this line here, check that line. Use a three point arc, start at the end of this line, position it on the projected line. We'll input a rad of seven mil. Okay, we can't input a rod of seven mil. Let's try that again. 7 millimeters. That's good. Then let's use the dimension tool between the endpoint of that line and this line here. Do that 2 millimeters. There we have what would be the dome of our pin. Let's put a mirror line in the center here and put that exact geometry on the other side. Let's select the line tool coming at the center point of this line going this line. Now we'll use mirror mirror, this arc and this line. We'll mirror them about mirror line here, press apply. That's looking good. That is a construction line, and we'll project this line as well, like we did on the other side. That completes the profile, reading model revolve. Select this profile, center profile, this profile here. For the axis, we'll select our axis here. Okay. And there we have our pin in the center. It's looking good. I'll select those two domes. Again, I want to put on them a red appearance. Write that again. Yeah, there we go. And the last feature to add to this is the mounting plate on this plane here. So let's create a two d sketch this from the top plane, rotate that 180 degrees. And we use a two point center rectangle, start at the origin there. The width will be 80 and the height will be 60. Let's put in eight mile fillets between these lines here. Then that's three D model and extrude that profile. But let's only extrude that by let's say sheet metal, 2.5 mil. Good. There we'll input our mounting holes. So these would typically be slot on a caster wheel. For this, we'll use the center to center slot command. For distance, we'll use 8 millimeters for the diameter dimension, so enter ten dimension between the top line and this line. A five mill dimension there. The center point of this arc and this line here. Let's do let's say ten mil let's use a line command and draw in mirror lines. So drawing a vertical line and a horizontal line. Both those lines, put them as constructions. Like the mirror tool again, select our slot, mirror it about the vertical mirror line. The two slots. I'll select those two slots, mirror those about a horizontal line by four slots available. Get a three D model. We'll extrude those four slots. You want to cut them. And we can either extrude them by 2.5 mil or I prefer to extrude two face like this face here. Press okay. There we have our four slots in position there. And that is our complete caster wheel. If you have any questions about this part, please ask in the comments section or apply as soon as I can. Aside from that, I'll see you in the next tutorial. Thank you. 78. Flange/ Mating Face Assemblies: In this tutorial, we will model a basic flange coupling. Let's start a new part, and we'll select star two D sketch. We'll do this on the XY plane or start off by drawing the flange itself. So let's do this from the origin. Let's use an OD of 165 mil. Then we can draw in the PCD, that's a pitch circle diameter, which in this case, we'll choose one, two, seven mil. On a right click on that PCD and identify it as a construction line. Then we can go ahead and input our mounting holes. So let's just throw in one here. So let's do a 16 mill mounting hole. Let's put a coincident constraint between the center point of that hole and the PCD, and then a vertical constraint between, again, the center point of that circle and the origin. So that's now fully constrained. We can go ahead and circular pattern there. Let's select the hole as the geometry to pattern. And for the axis, we'll choose the origin. We want to have eight instances, and these will be across the 360 degree revolution. Press Okay. Let's go ahead and three D model extrude that. Select that profile. I will extrude that by as 18 millimeters. Okay, next, let's draw a sketch on this face here. So left click ones, create two D sketch. Select the circle tool again, start from the origin. This has an 80 mil diameter. We'll go a three D model but extrude that profile by 100 mil. Okay. We can then go and put in the wall thickness. So let's select this face, create two D sketch. Again, we use the circle command, and we'll draw in a circle here. Actually, no, let's reject the existing geometry, then we can offset that by the wall thickness. So in this case, 8 millimeters, got a three D model and extrude this profile here, I would extrude cut. We'll go through all. Okay. There we can see we have our through hole. Let's put on some fillets on this part. Let's go fill a two mill fillet on this edge here, and then we'll add a one mil fillet on this edge and this one here. Okay. That's looking good. Save that. And then we'll move on to the assembly. And here, I've opened up a new assembly file. Let's go to place, and let's input our flange here. So I've called this part flange tutorial. That's okay. But yeah, we'll insert two of these, so we'll put one grounded. And then for the other one, let's just rotate that so we can right click and rotate about the Y axis. Let's do this twice so we can rotate 180 degrees. Then we'll left click once again, but roughly in position. I'm just going to go to view and put on shaded with edges. Then we can go and assemble and use the constrain between the center point of this flange. Sorry, the axis of this flange and the axis of this one, click apply, move that to the correct position, and then we can constrain any one of these mounting holes with its opposite on the other side. So let's choose this one, click Apply. And then just one more constraint will be the mating constraint between this face here and this face here. Okay. It's now fully constrained. Next, we need to insert the fasteners. So for this, instead of drawing the fasteners themselves and inserting them, we can actually choose fasteners from the orthodex library. So under place, we'll go place from content center. And here I'm just going to turn on a filter, which is the ISO, so it's going to mark out the IO parts, and we'll choose bolts. For this, we chose hexed bolts. And here we'll choose let's go to Io 4014, presso. Left click once, and then we can define the bolt we want to input. So we do 16 mill through holes, so let's choos an M 16 thread. For the nomal length, we'll choose 65 mil. That's fine. Again, let's rotate this around the Y axis by 90 degrees. Left click once. Then let's go ahead and constrain that to position. So we'll select, first of all the axis of the bolt and the axis of the through hole. Let's apply that and then we'll mate this face here to the bolt face apply. Then one more constrain we'll add to prevent the bolt head from rotating. So we will select the X z plane and constrain that. We'll use the angle constrain, the directed angle this face here, zero degrees. Press okay. Now that bolt head can no longer rotate. And pattern that. So we'll select that bolt, circular pattern. And for the axis, we'll select this cylinder here. For the number of instances, we'll select eight. And for the angle, so we want to have one bolt at every 45 degrees, which is 360/8. It's okay. There are all our bolts. That's great. We do exactly the same for the nuts, as well. So place from content Center. Let's go nuts. We'll chose a hex nut and IO 4032. Left click once, and 16, press okay. Now, I'm just going to click anywhere, Constrain. Let's choose the axis of that nut with the axis of this bolt. And again, a mating constraint between this face and the face of the nut. It one more constrain in between this face of the nut and this face of the bolt head. I'll be an angle, a directed angle. Okay. And exactly the same. So let's pattern that nut, for the axis, let's choose the axis of this cylinder. Again, eight instances spread across 45 degree intervals. There we have the fastness complete. That is the end of the tutorial. If you have any questions, please post them in the comments section, but aside from that, I will see you in the next tutorial. Thank you. 79. Engine Valve Modelling & Sketch Constraints: In this tutorial, we will model a engine valve. And so to do this, we will draw the profile of the valve, and then we will revolve around that. But let's start a two D sketch, and we'll select the XY plane. We'll start at the origin, and we'll draw in a straight line, which will be vertical, so this will be our line of revolution, and we'll put it in a height of 90 mill for this demonstration. Go to the top of that line, and again, we'll select the line tool, and we'll come across horizontally by the radius. So that'll be four mill then we'll come down vertically at 2.5 mil and we'll come into the profile then at no 0.5 mil. And so from here, let's select the three point arc. Although just before that, I'm going to move this dimension out of the way. But yet, three point arc, we'll start at the endpoint of this line, and we use the dynamic input boxes to identify the other endpoint of the arc. Over this, we'll enter five mill and then press tap on the keyboard and enter 90 degrees. And now we just need to input the radius. So in this orientation, we'll put in a rad of 5 millimeters. That's looking good. Then let's just come out of the profile by that 0.5 milt. Then we can come all the way down, just position the line roughly down there, and we'll just apply the vertical constraint to that line, make sure it's vertical. Again, let's use the line tool, and we'll start from the endpoint of this line. We'll come across here by 28 mil, and then we will come up by 1.5 mil. Going to move that dimension out of the way. We just want to draw in our line here, which will be at an angle of 135 mil. Let's press tab and enter 135, press Enter. And then we can use the dimension tool between the endpoint of this line here and the baseline. This will have a height of 4 millimeters. And then all we need to do now is to put in our arc. So to do this, let's use the tangent arc. It'll be tangent from this end point of this line. It will finish on this line here. Let's put in a dimension on that ad of 16 mil then we have our profile complete. That's fully constrained. Let's go to three D model, and let's revolve that profile. And for the axis, we'll select our 90 mil line. So this one here. Review looks good. Press okay. And then we have our engine valve. If you have any questions, please post them in the comments section, but aside from that, I will see you in the next tutorial. Thank you. 80. Multi-plane Extrusions: In this tutorial, we will model a generic camshaft. So let's start a two D sketch, and we're going to sketch the profile of the lobe on the XY plane. We'll start by using the circle tool from the origin, and we'll draw in a circle of 35 millimeters. Just above that, let's draw in another circle. That would be 8 millimeters in diameter, and let's use the vertical constraint between the center points of both circles, and then we use the tangential constraint between both of these circles so that they're in contact like so. Let's use the line tool now and just draw a line anywhere between the two circles and just the same on the other side. Again, we'll use the tangential constraint between this line, this circle and with the smaller circle as well. Repeat the process for this line. And then we have our profile of the CaM lobe. Et's go to three D model, and we'll extrude all of these profiles. Extrude them by 20 millimeters. Okay. That's our first lobe. Let's draw the other one. So let's offset a plane, select this face here. We'll offset that plane by 80 millimeters. That's okay. Then select that plane, create two D sketch. We're going to project the profile of the lobe which we drew before, like soap. I'm just going to hit F eight on the keyboard, and I'm going to delete these projection constraints, and that gives us freedom over this profile, and then we can rotate that. Let's use the rotate tool, and we'll draw a box around our sketch. And for the center point, use the center, and let's input 180 degree rotation. Click appl. Let's finish the sketch there. Right click on that plane, and we'll turn off the visibility. So right click and press V, and then once again extrude that profile 20 millimeters. That's correct. And we have our two lobes. Let's go ahead and put in the camshaft now. We'll start a two D sketch on this face here. Draw a circle from the origin. Let's do this 25 millimeters. Go on three D model and extrude that profile. I've calculated this at 180 degrees. Then let's extend that shaft from this face. So we'll create a two D sketch here. We'll project the shaft and extrude that profile there, except we're going to do this by 40 millimeters. Okay, that's looking good. Go ahead and tidy this up a bit, so let's put some fillets on this edge and also the same edges on the other lobe. Is a one mil fillets? That's okay. Let's put it in a hamper on this edge here. It's a two mill hamper, and we'll put in a mounting hole on this face. So let's go to create two D sketch. Put a circle in there, let's do 5 millimeters, let's extrude that's extrude cut. And just for visual, we'll just extrude cut that by two mil that's looking good. Let's go ahead and mirror. So let's choose the mirror command. And for the features, we'll select every feature we have. So the first lobe, the second lobe, have one part of the shaft, the other part, billets of the lobes, hampor of the shaft and the through hole. Sorry, the extrude cut on the shaft here. And a mirror plane, we'll rotate the part, and we'll select this plane here. Review looks good. Let's hit Okay. And then let's just apply some appearances to make this a bit more aesthetically pleasing. Let's select all the lobes, hold down control, keep drawing boxes around each of the lobes. Under the appearance menu, we will select the glossy black appearance. And then let's do the same process for the shaft. So select all the components of the shaft. And for this appearance, let's use let's use semi polished Save. That looks good. And there we have our camshaft. If you have any questions, please put them in a comment section, but aside from that, I will see you in the next tutorial. Thank you. 81. Loft Modelling Example - Mounted Hook: In this tutorial, we will learn how to draw a wall mounted hook. To start with, let's draw the base plate. So we'll go to sketch. We'll start a new two D sketch. Let's do this on the Y Z plane, and we'll select the two point center rectangle tool. We'll start this at the origin, and we'll input a height of 20 mil and a width of 60. Let's then go a three D model, and let's extrude that profile by 3 millimeters. Press Okay. And let's go to the three D model tab and start to apply some fillets. Let's make these ten milads we'll apply these to both of the bottom corners just here. Press Okay. Looking good. We now need to identify where we want our countersunk holes to go. Let's select this face, create sketch. Then we'll then put these four points. We can just put them anywhere for the time being, and then we'll select the dimension tool dimension these up. So from the top line, this center point of this countersunk hole will be 5 millimeters. And then from the sideline here, it will be, again, 5 millimeters. From this hole down to the bottom line, it will be five mill. And then from the sideline here will be 15, exactly the same for the ones on the other side. So let's take the horizontal constraint, make these two horizontal, make these two horizontal. And then we just need to dimension this one from this line at five mill and this one from this line at 15 mil. And there we have fully constrained the center points of all of our four holes. So let's finish the sketch there. Let's go the three D model, and we'll select the hole command. For this, so, yep, inventor has already selected the positions. Another type of hole. There'll be a through hole, and there'll be a seat which is countersunk. Termination will be through all, and that's the correct direction. We want this dimension here to be 6 millimeters. And this dimension down here is 3 millimeters with 90 degrees, that's correct. Let's press Okay. We now have our four countersunk holes for mounting this to a wall. And next, let's draw the sphere at the top. So for this, we'll go into the origin folder, and we'll select the XY plane. Let's right click on that, select the new sketch. Let's put in the circle, which will become the sphere. So this is a diameter of 15 mil. Then we can dimension from the center point to the very bottom of the plate. That'll be 60 mill. And then, again, from the center point to the front face of the plate. This will be 70 mil. Sorry, it's 17 and then we can put a line in from the top to the bottom of the circle, and this will be our line of revolution. We can go to three D model and select the revolve tool, can select half the profile, and then select the line of revolution and press Okay. And there we have the sphere of our model. And next, we need to model the arm of our hook. So for this, let's select this face here. We'll go on to create sketch. And we're just going to draw in a triangle, like so. So we'll do two lines there, join those up. Let's put an equal constraint between these two lines here so that they are at the same angle and the same length. Let's then use the vertical constraint between the origin and the join between the two lines. And then we can input a dimension between these two endpoints here, which will be 16 millimeters. That's looking good. And so the idea here is that we will use the loft command to loft from this triangle profile here up to an eclipse profile, which will come on a separate plane which we'll input now. But let's select the XZ plane, and then we'll create a new plane. We'll offset that from the plane at 44 millimeters. Press okay. Got our new plane here, and we can see that it intersects the sphere. Let's select that plane, create Tod's sketch, and let's select the circle tool and go into Eclipse. Let's start this from the center and define our first axis point and our second axis point, and then we need to dimension these two. So this dimension here will be 3 millimeters, and this dimension here will be 4 millimeters. Then need to project the geometry of this sphere. So let's select the circumference. Then we can select the coincident constraint and put a constraint between the two center points. So the center point of the sphere and the center point of our eclipse, like so. That's now fully constrained. Press finished sketch. It's looking good. Let's right click on this plane, press V on the keyboard, hide that. Let's just go into sketch 13, edit that sketch. Let's just right click on the circumference of the sphere and put that as a construction line. Finished sketch. There we go. Now the only thing left to do is to put in the guides. And so to do this, let's start a new sketch on the XY plane. Let's go a new sketch. Now I want to select my eclipse, and I want to project that geometry. So I'm going to select the eclipse here. As you can see, we've now got this yellow line which we can use as reference. So let's go on the Arc tool in the front view. Let's select this corner here, and we want to go right to the end of our eclipse. And for the radius here, we'll input 70 stay using the arc tool, and we'll go from the bottom corner at this time, and we'll go to the end of our eclipse, which ends just here. We'll then put a rad of 100, that's okay. And these are two guides, which will be used for the loft tool. So let's finish the sketch there. The very last thing to do is to get a three D model, select the loft to. And first, we need to identify our sections. So let's add two sketches. Number one will be sketch 11. And the second one will be our Eclipse, which is this one here. And for the rails, we'll just identify these as being sketch 15, which are the two radii lines here. It's okay. Now you can see the preview looks good. Select okay. There we have our completed wall mounted hook. Any questions, please put them in a comment section. But aside from that, I will see you in the next tutorial. Thank you. 82. Modelling a Spanner: In this tutorial, we will model a combination spanner. So let's start by a two D sketch on the Z plane, and we'll start with a horizontal line, which will be 110 mill in length. And then we'll just right click, put that as a construction line and select the coincident constraint, and we'll put that constraint between the center point of the line and the origin, and we use this as the basis of the construction of this combination spanner. On the right hand side, we have a circle here, and then we have a hexagonal profile. So the circle is 16 mil. Then for the hex profile, select the drop down on the rectangle tools, we'll select the polygon tool. Make sure it's six sides, start the origin here, draw up, like so, and we'll put another one in like that. Let's put a horizontal constraint on one of the hexes and then a vertical constraint on the other one. That's dimension between the endpoints of this one as ten mil, and then we'll just do two points of the other one. Again, there's ten more. I'm just going to go ahead and remove the lines using the trim tool, so we'll select the individual lines here, which we don't need. That's looking good. And now coming over to the other side, let's do the other head with the profile there. So this is made up a series of eclipses. So if we go on the drop down of the circle tool, we'll select the ellipse, we'll draw in three of these. So we'll start at the end point of our constructional line. We'll just put them as a slight angle. We'll put in one ellipse put in the second one there, and then the third one, like so. And then we'll just put in a line from the endpoint of our construction line to the top of the first ellipse, same to the second one and the same to the third. I'm going to right click on each of these lines and put them as a construction line. And then we'll put one more line in from the endpoint at this construction line, and we'll put that also as a construction line, and then we'll dimension between one of the construction lines and this one as ten degrees. So that's our angle, and then we'll go ahead and we'll dimension the axis of each of the ellipse. So we'll start with the smallest one. So the major axis is five, and the minor is three. Then we'll go for the center ellipse, but the major in this case is 11, and the minor is nine. Then for the largest one, this will actually be the minor in this case, which is 11 due to its orientation, and the major will be 12.5. It's looking good, so we've got our three ellipses in there. Let's use the line tool from the top of our smaller quadrant. We'll just bring that out. We'll use the tangential constraint between that line and the eclipse. We do exactly the same on the other side. Use the tangent tool between that line and the eclipse. I'll just put in a parallel constraint between the two lines to make sure they are parallel, and then we'll use the trim tool and take away these two lines here. Also going to take away this arc, this one, and also this one. So now we can start to see the foundation, at least of our spanner. Go ahead on the three D model tool tab and select the extrusion tool. Go on to the top view, rotate that, and we'll select the profiles we wish to extrude. So we'll take these two, this one, and we'll take this profile as well. Let's extrude these by five and select Okay. We have two heads and the profiles. Now we just need to input the body. And for this, I recommend inputting a plane. So we'll do midplane between two existing planes. Let's select this one as the first reference, and this one as the second. We have our plane, put in the center there. Let's left click on that and create a new two D sketch. And for this, I'm going to draw in a two point rectangle. Dimension, the height of this is ten.'s a coincident constraint between this corner, this ellipse and this corner and this ellipse. That's looking good. Let's go ahead on three D model. Let's extrude that, select the profile. We'll select a symmetric in terms of the dimension, direction, and we'll select that as 4 millimeters, press okay. Let's now use the Phillip tool. Let's select all of our corners. Like so, and we'll input here 15 mill. There are 15 mill fillets. Let's right click on that work plane, press V on the keyboard, hide the visibility. Then we just need to put in the depressions on this face and this face. Let's create a two D sketch on this face. Then for this, we'll use the center point slot tool. We'll start this at the origin and we'll come across about 35 mil, and that will have a diameter of six looking good, that's fully constrained. Again, three D model. Let's extrude, cut that, let's extrude cut that by 0.5 mil plus o. Now, we need to do the same on the other side. So to do this, we're just going to mirror this feature. So let's mirror we'll select that feature. So in this case, extrusion six, and we'll mirror plane, we'll select the plane in which we input before. So W plane two, select the ok. And then we have the depression on both sides, and there we have our completed spanner. Thank you very much, and I'll see you in the next tutorial.