Learn Fusion 360 in 30 days for Complete Beginners! (Part 2 of 3)

1. Welcome To The Course! (Course Introduction): Hey there, I'm Kevin Kennedy. And welcome to Part two of Learn Fusion 3 60 in 30 days for complete beginners. I'm a product designer with over 10 years of cat experience, and I'm excited to give you this beginner fusion 3 60 course, absolutely free for the greater good of the Fusion 3 60 community Now in this course will walk you through the core features of fusion 3 60 while three D modeling familiar everyday objects. This second part of the course covers days number 11 through number 20. And, of course, Part three will cover the remaining 10 days. If you haven't already done so, I recommend watching Part one first to kick Part Two of this course off will start off by three D modeling a dog bowl in day number 11. Also, be sure to check out product design online dot com forward slash fusion High thin 3 64 Helpful Resource Is that all reference to in each tutorial 2. Day #11 - Fusion 360: Dog Bowl: Hey, there's Kevin Kennedy and welcome to day number 11 of Learned Fusion 3 60 30 days. By the end of this tutorial, you'll be able to three D model a dog bowl. We'll take another look at the REVOLVED feature, and you'll also learn how to set constraints. Lock in sketch lines, look at the section analysis and offset and thickened surfaces in the patch. Work space to get started will insert a reference image, which I've attached below in the video description. Now the reference image is half of the dog bowl because we'll use the REVOLVED feature to create the rest of the shape. I'll select attached canvas from the insert drop down list. I'll select the front plane and then I'll select the image from my computer. Now I'll go ahead and rotate this around, making sure that it's right side up. And I'll also set the opacity to 15% after clicking. OK will want to calibrate that image size, so it's the same as our reference dimensions. I'll open the Campuses folder, right click on the image and select calibrate. Then I'll click at the left of our 100 millimeter mark and I'll click of the right and I'll type in 100 millimeters now. After hitting answer, you'll see that the image was resized to the same dimensions as outlined on a reference image. Now, before we start drawing our sketch, I'll double click on the reference image in the timeline to reopen it, and I'll click and hold on this square in the middle, which will allow me to freely drag it around now to make things even easier for us will drag this around. So the center origin of our reference image lines up with our center origin point, and then we'll click. OK, at this point will go ahead and start drawing the outline of the dog bowl. I'll start off by hitting the keyboard shortcut letter l toe. Activate the line command and I'll click on the front face. Then I'll select the origin point and I'll drag over to the right, making this 100 millimeters long. I'll make this vertical line 2.5 millimeters hit the tab key toe lock, the dimension in place, and then I'll create another line. 10 millimeters to the left for the next line. All type in 55 millimeters hit the tab key, and then I'll type in 100 degrees for the angle. I'll hit the tab. Tito. Lock the angle in places well, allowing me to click anywhere without throwing off the dimensions. The next line I'll go over to the left 15 millimeters and then this line heading downwards . I don't know the length of it, but I know it's 100 degrees from the horizontal line. So enter 100 degrees at the tab key to lock it in place, and then I'll select down here. I'll hit the escape key and then I'll reactivate line with Letter L. And they'll create the 10 millimeter vertical line from the centre origin. And then I'll create the last line here, which will close off our profile shape. So you'll see that after I selected where the lines meet the profile shaped turned orange. Now this signifies that it's properly closed. Now, before we start adding fillets, there are a few different things will want to do. First, let's go ahead and activate the trim tool by hitting letter T on the keyboard, and we'll click on the extra part of the line here, so it doesn't mess up any of our fillets, and I'll hit escape to exit the trim tool. Now this point will want to add constraints to some of the lines, making sure that our overall profile shape doesn't get messed up when we go to add fillets . If we look at some of these icons and click on them, we'll see that we already have a horizontal and even some perpendicular constraints. I'll add a few more constraints by right clicking on the line and selecting horizontal. Now, before we add the fillets to this sketch, I'm going to click on the camp's light bulb to turn off the reference image, so it's a bit easier to see what's going on. I'm also going to add a dimension to this horizontal line here so it doesn't change and then I'll activate fill it from the sketch drop down menu. I'll select the first corner type in five millimeters, and then I'll select these top two corners. You'll notice. As we added these fillets, it took away some of the constraints and added, some tangent constrains to our sketch. All right, click toe, Activate Phillip once again, and I'll add a fillip of 2.5 millimeters to this outer lip of the bowl. Now, before we exit this sketch, I'll hover over the entire sketch to select everything and all right, click and select fix slash unfixed. This will lock all the lines of the sketch in place, ensuring that we don't accidentally move any of the lines or change any of the dimensions as we continue to work. Now, you'll see that some fusion users like to fix lines one by one as they draw them, and others like to do entire sketches at once. Now it really just depends on your workflow and personal preference. But either way, it comes in handy, especially if you're going to be working on the same file with someone else. We'll go ahead and stop the sketch, and then I'll activate the revolved tool from the create drop down menu. We'll select the profile sketch we created, and we'll select the center origin line for the Axis. I'll change the operation to new component, and I'll click OK, now that we have the overall shape of the dog bowl will need to make the bottom hollow. To do this, I'll activate the shell tool from the modified drop down list, and I'll click on the bottom plain and type in 2.5 millimeters for the thickness and you'll see the after we click. OK, we've created this nice dog bowl shape. Now sometimes when creating models, you'll want to take a look at the inside to make sure that things are how they should be. Now I want to double check here that this bottom surface is raised off the ground. So all select section analysis from the Inspect Drop Down menu. I'll click on the Y Z plane and then I'll hit. Okay, you'll see. Now we can take a look at the overall shape that we've created after revolving it. And if we go over to the analysis folder, we can talk about this on and off whenever we need it. Now the last thing will want to do is create a rubber band that fits around the bottom of the bowl here, making sure that our dog bull doesn't scratch any nice wood floors. So before we do this, I'm going to fill it the edges of this outer lip, making sure they're not sharp. I'll hit letter F on the keyboard to select. Fill it and then I'll select the top and bottom lines and I'll type in one millimeter and click OK now to create the rubber. Banding will go to the patchwork space, and I'm going to use the offset tool from the create drop down lists. Then I'll select a dog bull as the surface. I'll type in 0.2 millimeters for the offset distance, and I'll set the operation to new component and click. OK, now it's a little bit hard to see what we just did here, so I'm going to rename the components. I'll double click and make the 1st 1 dog bowl, and I'll name the 2nd 1 rubber. I'm also going to right click on the rubber Select appearance and all Dragon drop a soft rubber onto the rubber component. Now, if I toggle the rubber component on and off, you'll see that we have our dog bowl and we have a rubber. But we obviously don't want the rubber to cover the entire surface, so we'll have to trim some of it away. So I'll create a new sketch off the bottom plane and I'll hit letter C on the keyboard for center circle. I'll click on the center origin drag out, and I'll type in 185 millimeters for the distance. Then I'll hit letter E for extrude, and we'll need to select the circle we just created and dragged the arrow up. Now we can select to object from the extent menu and select the top of our dog bowl. That way, we're not cutting any further than necessary. Then all toggle the objects to cut folder and we'll insulate the dog bowl. So you see, this is one reason it's a good habit to rename your components and bodies. It will make it a lot easier to select the right thing when using certain tools. Infusion. Let's click OK and take a look at the result. Now, if we take a look at the section analysis again, we'll see that the rubber band isn't very thick, so I'll select thicken from the create drop down menu. Click on the rubber ban, and I'll make this 1.5 millimeters thick. Now we have a nice protective rubber band around the bottom of her dog bowl. The last thing I'll do here is add the appearance of stainless steel by right clicking on the bull component, and I'll Dragon drop polished stainless steel onto the dog bowl, then also have to reapply the soft rubber to are banding here because the thick and tool created a new body, so we lost the appearance we previously had. 3. Day #12 - Fusion 360: Auger Bit (Spiral Helix): Hey there, it's Kevin Kennedy and welcome today Number 12 of Learned Fusion 3 60 30 days. By the end of this tutorial, you'll be able to three D model in Auger Bit. We'll take a look at how to create a new component, how to use the pipe feature and how to create a sweet following a helix, along with how the loft to a point Before we get started. I would like to say thank you to all of my subscribers who have been watching the series so far. If you're new to the product design online channel, to be sure to hit that red subscribe button right now, and also be sure to drop a comment below with any questions or struggles, you face Infusion 3 60 so I can address them in future videos. Now we'll start off by creating a new component by selecting new component under the Assemble drop down menu. We're going to create a new component because it will group all of our bodies and sketches within the component, and it will give us a few other advantages. Should we create assemblies or need to make copies of the component in the component dialog box. I'll make sure empty component is selected, and it's a good idea to get into the habit of naming your components and bodies as you create them. So we'll go ahead and write out Auger bit for the name and click. OK, now I've noticed a lot of people are confused on the difference between components and bodies, so I'm going to take some time to explain the differences and demo a few different things for day number 13 of Learned fusion 3 60 30 days. Now we're going to create the center rod of the auger bit by using the pipe command. If we select pipe from the create drop down list, you'll see that I can't actually create a pipe without a path for it to follow. So we'll hit close and we'll go ahead and call the line tool with the keyboard shortcut Letter L. And I'll click on the X Y plane. I'll click on this center origin, drag my mouse up and type in 750 millimeters for the distance, followed by the tab Key toe like the dimension in place and I'll click with my mouse and then hit the escape key toe exit the lying command. Now, if we go back to the create menu and select pipe, we can create a pipe by selecting the path or the line that we just created. Chain selection wouldn't matter because we just have one line. But if we had a spine or multiple lines making up our path, then we would have to have that selected if we wanted it to follow the whole line. Now the distance is how far along the path the pipe follows. So if I dragged the arrow up, you'll see the distance changes. But we'll go ahead and leave this at one, so it's set to the full length. The next option. You'll see that I can change the section of the path by selecting a square, a triangle or the circle, which will leave it on for now. Next, you'll see that we can change these section size or the with of the pipe. So I go ahead and type in 38 millimeters for the with all select Hollows or pipe isn't solid, and you'll see that as I selected hollow, it gave us the ability to now punch in this section thickness or the thickness of our pipe . So I'll go ahead and change the section thickness to three millimeters and click OK to exit the pipe Command before we go any further, I'll hit Save entitled this Auger bit and I'll click the blues save button Now, in order to create the sweep, will have to create a helix shaped that revolves around our pipe. And there are a few different ways that we can do this. Infusion 3 60 Unfortunately, Fusion doesn't offer Helix Sketch Command like some other CAD programs, but as the first viable option, there is a free helix plug in, created by Patrick Rains Bury, that allows you to create helix sketches holding to that plug in and the installation directions in the description of this video, if you'd like to play around with it. But for this video, I'll show you the second feasible option, which is to create a coil and then project a sketch from it. So I'll activate the coil future under the create Drop down list, and I'll select on the top plane. Then I'll take a look at this from the top view. I'll select the center of our pipe. I'll drag out with my mouse and I'll select the inside of the pipe, which is at 32 millimeters. I'll change the revolutions toe five, so the auger bit spirals around the center pipe five times, and I want them to go up a little over half the pipe, so I'll punch in 450 millimeters for the height. If we take a look at this from the top of you again, we can see where the coil is compared to the pipe, and we want the coil, the line up with the outside of the pipe. So I'll change these section position to outside, and I'll type in three millimeters for the section size, which is the same thickness we made our pipe. Lastly, I'll change the operation to new body and I'll click OK, looking at the front of the pipe. We can't really see the coil because it lines up with the outside edge of our pipe. So I hit the light bulb for the pipe in the browser. I will also go ahead and rename the bodies by double clicking on them and typing out pipe and coil, respectively. Now to project the sketch. I'll go to the sketch drop down menu. Find the project slash include folder and I'll select Project a Surface. Then I'll have to select the front plane here and I'll select the coil for both the faces and the curves. And then I'll click. OK, at this point, we're done with the coil, so I'll turn the coil off in the browser by hitting the lightbulb icon. We'll want to create a rectangle shape that will sweep around the Helix sketch that we have . First, I'll create a new plane off the path by going to the construct menu, and I'll select clean a long path. Then I'll click on the Helix and I'll click. OK, we'll right click on the plane and hit. Create new sketch. Ah, hit letter L on the keyboard to call the line Command. I'll go over to the right 113 millimeters. Hit the tab. Key toe lock the dimension in place and I'll click with my mouse. I'll go up 3.5 millimeters, hit the tab key and click with my mouse. I'll go back to the left. 113 millimeters hit the tab key and click with my mouse and I'll go down to connect the lines and close off the profile, which will be signified by the orange background appearance. Now. It can also add some extra constraints by holding down the shift key and clicking both of the horizontal lines. Then, all right, click and select the parallel constraint. All right, he saw hit Stop sketch in the toolbar, and then I'll activate the sweet command from the create drop down menu. I'll start off by selecting the profile that we just created. I'll select the coil as the path now, at this point, you can see that it doesn't have enough to create this sweet, so I'll switch the type from single path to path plus guides surface, and then we'll select the bottom of our pipe as the guide surface. I'll make sure that the operation is set to new body and I'll click OK, then, before I forget or rename the body by double clicking on it in the Fusion 3 60 browser and all type out metal spiral. Now taking a look at the bottom of her auger bit, we don't want the dirt to come into the pipe here, so we'll go ahead and create a comb shape with the law feature. I'll take a look at the bottom of the pipe and holding down the shift key. I'll select these two circles will project them by going to the sketch drop down list. We'll find the project slash include folder once again, and this time I'll select Intersect because we want the circles to be on their current plane. All select the bottom of the pipe, and then I'll click OK on the Project Dialog box. We'll also need to create a point that will loft to and will want it to be away from the end of the pipe here. So I'll select Offset Plane. I'll click on the bottom of the pipe. I'll punch in 25 millimeters for the distance and I'll click. OK, then. All right, click on the plane and select. Create new sketch. I'll go to the sketch, Drop down menu and Select Point, and I'll click on the center origin. Now we have our profile, and we have the point that will off to. So I'll activate loft from the Create Drop down menu, and I'll select the profile and then I'll select the point. I'll make sure the operation is set to join and I'll click. OK, I also want to add a nice champ for to the beginning of the blade here. So I'll select champ for from the modified drop down list and I'll select on the top line. I'll make the distance three millimeters and I want the angle to go back a bit further. So I'll change the champ for type from equal distance to two distances and then I'll make the second distance five millimeters and I'll click. OK, now I don't want this video to get too long, so I'm not gonna worry too much about the top mechanism. But I'll quickly create part of where the Auger bit hooks up to machine by using a center circle with the keyboard shortcut letter C and I'll create one to the outside of the pipe and will create another to 50 millimeters. And then I'll hit letter E to extrude this down 70 millimeters and we'll set the operation to join and click OK, Lastly, I can right click on the component, hit appearances and search for steel. I'll simply drag and drop polished steel onto the model. I'll double click on the material to change the color to red. 4. Day #13 - Fusion 360: Difference Between Bodies and Components: Hey there it's Kevin Kennedy and welcome to day number 13 of Learned Fusion 3 60 30 days By the end of this tutorial will have a solid understanding of the difference between bodies and components. Also, be sure to watch to the end where I'll discuss the dubbed rule number one of fusion 3 60 Now I've noticed a lot of explanations. Forget to talk about one important thing, which is the difference of bottom up assemblies, verse top down assemblies which may help. You better understand why fusion 3 60 s set up the way it is. So let's take a look at bottom up assemblies first. Now, this is the traditional assembly modelling technique. And if you're coming from Autodesk inventor or another CAD program, then you're likely already familiar with it. The essence of the bottom up assembly technique is that each part is created individually and then all of the parts are inserted into an assembly document and constrained to each other. There is no link between parts, so the parts fit together because you designed them to fit together. And if you change one part, you better know which other parts will be affected by the change and make sure that you update them accordingly. On the other hand, we have top down assemblies, which means you start with an assembly file and you build all of your parts within the context of the assembly itself. Now fusion 3 60 falls into the top down assembly category, which is why you'll never see create new assembly under the file menu. But you will an Autodesk inventor in solid works. The benefit of top down assemblies is that we can reference other sketches and parts, so if we change one thing, the other features change accordingly. Now this is a great way of ensuring that parts that need to fit together always fit together without you having to go back and manually edit them each time. Now, this top down technique is intuitive and much quicker, but it does still have a few drawbacks. You can still get yourself into a pickle, especially with large assemblies that contain many different components, which is why I recommend a plan out your model before you even start your very first sketch already. So now that you know Fusion 3 60 is based on the top down assembly technique. Let's take a look at the difference between bodies and components. Bodies could be seen as modelling tools. You use separate bodies toe. Add or remove geometry to achieve the final shape of your design. An example of a body could be a ceramic mug. You would create one body for the cylindrical part of a cup and another body for the handle and, of course, joined them together. Contrary components represent real world parts. You can think of them as things that are manufactured with multiple pieces. You'll want to use components when you're designed. Consist of multiple parts that may be assembled toe one another. Now a good example of a component would be a door hinge as it consists of three different components one for the left wing of the hinge, one for the right wing, and the third is the pin that holds the hinge together. Now let's take a deeper dive into both of these concepts. With bodies, you'll create a new one any time you turn a sketch into a three D object. If we take a look at the ceramic mug once again you'll see that the downside the bodies is that they can't be copied to another file unless it's indirect modeling mode now. This is mainly because copying the Parametric timeline could be difficult. So if for some reason you do want to copy of Body two completely different file, then you'll have to change it to direct modeling mode by clicking on that little settings icon in the lower right hand corner. Then you have to select Do Not capture design history and click Continue, and, as you will see, it will delete the timeline. So if I go to copy this mug again toe a file that is also indirect modeling mode, you'll see that now it will actually let me paste it into the other file. Now, with that said, if you're planning on copying, you should make it into a component, and we'll discuss that in just a bit. Before we do that, let's take a look at a few other cons in regards to bodies. First off, they won't show up in a parts list, which could become troublesome if you need to create a drawling that includes all of the parts. Second pattern bodies lacked independently from their parents, so if you alter one of these bodies, you'll notice that others don't change. Whereas if I had made them components and I alter one, then the other two will update accordingly. Now, if we take a look at the screws that our bodies will notice that components can be created from anything that is in the body folder here. But components cannot be created from sketches, so if we right click, you'll see that there is no auction to create a new component. But if we right click on the body that we can create a new component now, in order to turn a body into a component, it does not have to be closed. And in fact, there are three different types of bodies. Infusion 3 60 We have solid or surface bodies. We have school, two bodies and we have mesh bodies. Now there are two main ways we can create a component from a body. We can either right click on the body and select, create components from bodies, or we can go up to assemble and hit, create new component, select from bodies and will select the body. And then we can hit. Okay, now, another quick thing to note. If I select two bodies here, that does not mean it will put them in the same component. If I go ahead and do that, it will actually create two different components. And if we take a look at it in the browser, will see the bodies here now. Another thing to note is that they're both labeled body number one. So this is where the dubbed rule number two from the Fusion 3 60 form comes in place, which is to always always rename your components and bodies right after you create them. And it's even a good idea to get into the habit of renaming any sketches, decals or any other layers you may have is well, so what the heck, er components. And why should we use them instead of bodies? If we take another look at her door, Hinge example, we'll see that components contained bodies, and they also contain sketches, planes and other objects. These three components of our door hinge makeup our assembly. Now, in the beginning of this video, I talked about bottom up first top down assemblies. I mentioned that fusion 3 60 is the top down assembly type because we can create all of our components within the same file, and they're driven by one another. So if we look at the browser tree will see that we have the master assembly at the top, and then we have the components nested underneath. We'll also see that the assembly is signified by the three cube icon. The components are one cube and a body is a cylinder icon. Now let's take a look at some or advantages of using components over bodies. First, you can drag bodies and other objects from one component to another in the browser. Ah, component can also contain other components, which is often referred to as a sub assembly. Components allows to use joints to assemble and create mechanical relationships. So we take a look at this door, hinge example. You'll see that it moves based on the joints I applied. But if I created this with bodies and not components, then I would not be able to apply these joints. Another trick and handy thing with components is that you can activate components, which offers many advantages. So if I click on this little circle icon toe, activate it and take a look at this component that I can focus solely on it and other components will be shown with some transparency. Now the advantage of activating components means that all the bodies, sketches, components or any other features that I create will automatically be nested within that component. Lastly, and probably one of the most important things about components is that they can be reused or copy and pasted in a design so we can do this by right clicking on the component and selecting copy and paste, and we can duplicate them as many times as we would like And as we discussed earlier, Component instances update when a change is made toe, one of them now having a basic understanding of the difference between bodies and components leads us to the dubbed rule number one from the Fusion 3 60 Forum, which is to always start your file off with a new component. Now Rule Number one was created by the Fusion 3 60 community on the forums, and the idea is that if you always start with a component, you'll never be kicking yourself in the foot when your browser tree is messed up because you're trying to create components after creating your bodies. So let's go ahead and recap everything. It's okay to use bodies if you're just creating a small, simple or quick model for something like three D printing or something just to play around with while you're learning fusion 3 60 Specifically, if you know you don't plan on using it for any assemblies, and you don't need to copy it. Otherwise, it's a good practice. Get into the habit of always using components at the beginning of your design, which will ensure that you can successfully create joints, subassemblies and assemblies without any major headaches. Now, as we looked at previously, it is possible to create components from bodies. But again, it's not recommended to do afterwards because it won't always work, and sometimes it will cause a lot of heirs in your model. 5. Day #14 - Fusion 360: Flat Head Screwdriver: Hey there, it's Kevin Kennedy. Welcome to Day number 14 of Learned Fusion 3 60 in 30 days. By the end of this tutorial, you'll be about a three D model, your very own screwdriver, which, of course, could be three D printed and actually used. We'll take a look at how to create components driven off of previous components, and we'll cover the three point arc sketch feature. We're going to start off by modeling the handle of the screwdriver as one component, And then we'll create a second component for the shank of the screwdriver to create a new component. All select new component from the assembled drop down list, and I'll double check that empty component is selected before we hit. OK will follow Rule number two, a fusion 3 60 which is to always name your bodies and components all type in handle for the name. Make sure activate is selected so we can start working on the component right away, and I'll click OK in the new component dialog box. Now let's start to create the handle by using the cylinder tool from the create drop down list. After selecting cylinder, I'll click on the front face. Click on the center origin, drag out with my mouse, and then I'll type in 28 millimeters for the width. I'll hit the tab Key toe lock the dimension in place, and I'll click with my mouse to snap the circle in place. Then I'll make the length 100 millimeters and click OK, toe exit the cylinder feature. And before we do anything else, I'll rename the Body cylinder by double clicking on it in the Fusion 3 60 browser and I'll type out cylinder. Also, click on the Save Icon, type out slot head screwdriver for the name and I'll click the blue save button. At this point, we could leave a basic cylinder shaped for the handle, but it would work better and be more ergonomic if we cut some grooves in it. To do this, I'll look at the handle from the back side. Then I'll hit the keyboard shortcut letter C for center circle and I'll click on the back face of the handle. What I want to do here is draw a circle extrude cut it, and then I'll pattern the cut feature around the handle, so I'll just click on the left side here at the edge of the handle where the centre circle function will snap into place and I'll make this circle six millimeters. Now I'll hit the keyboard shortcut letter E for extrude, and we'll extrude cut this 75 millimeters and then I'll click. OK, toe exit the extrude command. I'll activate the circular pattern feature located in the Pattern folder under the Create Drop Down menu. You'll see that after we activate the pattern feature weaken. Select the pattern tight, all select features as the patterns hype. And then I'll select the extrude feature in the timeline below. For the Axis, I'll select the center access of our handle. And remember, if you ever can't select the access here in the canvas because it's blocked by a body, you can select the access in the Fusion 3 60 browser. Now we want this pattern to go all the way around the handle, so make sure full is selected as the type, and then we'll set six for the quantity or the number of times to pattern. Looking at the model, we can see a faint preview of the pattern, but let's go ahead and click OK to see the results now. One thing to note here. We could have used the sketch circular pattern and pattern the circle around before we extruded it. But I recommend using the pattern feature under the create drop down list wind possible as it will perform much better infusion 3 60 especially when dealing with larger and more complex patterns and assemblies. Now the main reason is because the sketch tool is trying to render all of the geometry, whereas if you look at the sketch of our pattern feature, it's simply rendering the one circle. And the pattern feature is mimicking the extrude cut. At this point, I want to add a nice fill it or rounded edge to the back of the handle. I'll select the keyboard shortcut letter F toe. Activate the Philip Command. I'll select all six of the outside edges, and I'll type in 10 millimeters for the distance. And, of course, you can always type in mawr or less year. It really just depends on how much you want the back of the handle to be rounded over. We'll click OK to exit the Philip Command. Now I want to add a rounded div it to the front of the screwdriver. Your thumb and forefinger have a nice and ergonomic place to rest. All right, click on the Y Z plane in the Fusion 3 60 browser and I'll select Create Sketch. We're going to use this center plane because we're going to draw on the lips and then we'll revolve it around the cylinder. I'll select the Ellipse tool from the sketch drop down list, and I'll click just above the handle. Now I'm not sure exactly how far down and once ago, so I'll just go down six millimeters and I'll go to the right about 21 millimeters as we can always go back and change the dimensions. Now I'll select the Revolved tool from the create drop down list. I'll select the Ellipse we just created as the profile and once again will select the center access of our handle. I'll make sure that my operation is set to cut and I'll click OK to see the results. Now, Looking at this David, I may decide that I want to go down a bit further. If so, I'll double click on the sketch in the timeline to edit the Ellipse. I'll change the height here to eight millimeters. I'll hit Stop, sketch and take a look at the new results. All right, he saw her handle is coming along nicely so far. The last thing will want to do is add some nice fillets or rounded edges to it, and then we'll proceed on to make the shank and tip of the screwdriver. I'll hit the keyboard shortcut letter F toe. Activate the Philip Command and I'll select the front circle of the screwdriver at a fillip of 1.5 millimeters and click. OK, I'll hit letter F again, and I'll select these circles on each end of our div it and I'll make these one millimeter and click OK. Lastly, we'll go ahead and add some nice rounded edges to our grips here, clicking letter F to activate the Philip Command. All select all six of the grip edges and then I'll punch in 2.5 millimeters for the fill it distance. I'll click OK, and then I'll right click on the edge here and I'll select Repeat, fill it. Select all six of these corresponding edges. I'll make this edge. Round it off with one millimeter and then I'll click. OK, now the last thing will want to do with our handle before we're done with a component is to add a whole for a screwdriver. Shank. I'll have to keyboard shortcut letter H for whole, and I'll click on the front face of our handle. Now the whole should have snapped to the center origin. You'll see if I drag this whole around, it will snap right into that center origin point. We wonder. Hold to go halfway into the handle and the whole dialog box. I'll make the length 50 millimeters on Make the width of the whole seven millimeters and then I'll change the drill points of flat click OK to exit the whole command, and we're now officially done with the handle of our screwdriver. At this point will want to create a new component for the shank of our screwdriver, but first will want to activate the top level. Components are new. Component is nested within it toe. Activate it. I'll click on the little circle to the right of our file name and once activated, all select new component from the assembled drop down list, and I'll rename this one shank and click. OK, now you'll see in the Fusion 3 60 browser that the shank and handle components are nested underneath the screwdriver assembly. I'll make sure that this Shane component is active before we start doing any work, and then I'll select the face of our whole this way, if we change the whole dimension later on, our shank dimension will update accordingly, just like we talked about in day number 13. All hit letter E for extrude. And then I'll make the distance 150 millimeters and click. OK, now let's click on the circle next to the handle components reactivate. It will take a look at our hole size. I'll double click on the whole feature and changed the with to 10 millimeters and then click OK, then I'll reactivate our assembly and you'll see that the with of our shank did update accordingly. As we expected, I'll go ahead and click undo to revert back to the original size. Now all we have to do is create our screwdriver tip, which will create a new component. For this time. I'll use another method. All right, click on the top assembly and select new component. I'll double click on the component in the browser and type in tip for the name. I'll select the front face of the shank and click letter E on the keyboard for extrude, and I'll punch in 10 millimeters for the distance. I'll make sure new body is selected and then I'll click. OK, and before I forget, I'll find the body in the browser and rename it to slot Head Tip. Now we're going to create the slot or flathead tip by cutting at this cylinder from the side. All right, click on the Y Z plane and select Create Sketch, then all activate the three point arc from the sketch drop down list. For the first point, I'll select the front edge here where it snaps in place. I'll select the top line where snaps in place, and then I'm just going to put the third point where it creates that nice arc of the Flathead. Now, at this point, will went toe fully definer sketch so we don't mess it up. If we change dimensions and any of our other components, I'll hit Letter D to activate the Dimension Tool. I'll click on the end of the three point arc here. Click on the center origin of our tip, and I'll make this 0.5 millimeters and then hit the escape key to exit. Now you may have noticed that the other end point moved down, so I'll select this in point of the Ark and holding down shift. All select the corner of the cylinder. Now I'll click on the horizontal constraint icon. This way, it's always in line with the thickness of the tip. Even if we change our dimensions now, in order to extrude cut, the shape will have to close off our profile so we can hit letter L for line and then draw a horizontal line. And we can also draw a vertical line connecting the endpoints once again before we cut. This will also want to make sure that all of our lines are black, indicating that they're fully constrained using D on the keyboard for dimension. I'll select the horizontal line, and I'll make this nine millimeters. Then you'll notice that the ark is still blue because weaken dimension the radius of it. So we'll click on the Ark and then hit Enter and you'll see After that, our profile is fully constrained, as as black lines all the way around. Well hit letter e for extrude Select the profile and I'll change the direction here to two sides. We'll need to change the operation to cut and for the extent of each side will select all. Now the reason we're selecting all is again for the purposes of our dimensions. If we decided to make this shaft thicker than are cut here will update accordingly and we won't have to go back and manually at it. This extrude feature I'll click OK toe exit extrude command and now will want to select Mir from the Create menu will change the pattern Type two features and will select the extrude in the timeline for the mid plane. I'll select the XY plane in the browser and then I'll click OK to take a look at the results. Now we're essentially done with our slot head screwdriver. We can reactivate the top level component to take a look at it, and of course, we can always select a component hit letter A for appearances on weaken drag and drop the appearances onto each component 6. Day #15 - Fusion 360: Painter's Tripod: Hey there it's Kevin Kennedy and welcome to day number 15 of Learned Fusion 3 60 30 days. By the end of this tutorial, you'll be able to three D model a painter's tripod for three D printing. If you're not familiar, a painter's tripod is a pyramid that you can rest items on with minimal contact, allowing you to paint or stain both sides at once. We'll take a look at how the loft to a point the project sketch feature the mere feature using mid planes, and we'll talk about setting up our file so we can change the dimensions without causing any heirs to get started. Will create a new component by selecting new component from the assembled drop down list. All title this painters tripod and click OK, now we'll start to create the pyramid by sketching a triangle for the base well hit letter L on the keyboard for lying, and I'm going to select the top plane. I'll click on the center origin, and I'm just going to drag my mouse out and click three times, creating a closed profile triangle shape without worrying about the size and the shape while holding down the shift key. I'll select all three lines, and then I'll select the equal sketch constraint so you'll see that this immediately made all three lines in equal size. And if I click on this point and dragged the triangle, it will resize all three at the same time. I'm gonna hit the letter D on my keyboard for Dimension, and I'll select this top line and enter 60 millimeters for the distance. Now, after punching in the Dimension, you'll see that the other lines changed to 60 millimeters as well, along with that adding the dimension also fully constrained or triangle sketch, which is signified by all the lines turning from blue to black. Now, if I try to drag any of the points around, it won't let me. All that I can do is change the dimension number, which is what we want. So we know this triangle won't change size or shape unless we want it to. Before we go any further, let's go ahead and save our design. I'll click on the Save icon, type out painters tripod and I'll click the Blue save button. Now we're going to create an offset construction plain and which will create a points on before we use the law feature. I'll select the offset plane icon in my toolbar or from the Construct Drop Down list, and then I'll select on the triangle sketch. I'll type in 50 millimeters for the offset distance and then I'll click. OK, we'll right click on the plane and select Create sketch. Now. We could just insert a point here, but instead I'm going to first project the sketch so we can reference it. I'm going to hit the keyboard shortcut letter P for project, and then I'll select the three lines and click. OK, and I'll show you. Why am projecting this sketch in just a minute? First, I'm going to hit Letter X for the construction line and you'll see in the sketch palette that as I keep hitting the X key, it will toggle the construction line feature on and off. So I wanted to be selected Blue, which is on, and I'll then hit the keyboard letter l for line. Now I'm going to draw to construction lines from the Vertex of the Triangle to the opposite midpoint, giving us the exact vcenter oId, or the center of the triangle. Now all select the point feature from the sketch Drop down menu, and I'll select where the two construction lines intersect and it should snap into place for us. I'll hit the escape key to exit the point command, and now we're going to loft from our base triangle to the point that we just created I'll select Loft from the Create drop down menu. I'll select the triangle profile as the base, and then I'll select the point. And it should connect the loft without us having to create any additional guide rails, and we'll go ahead and click OK in the loft dialog box. Now, before we go any further, I'll show you why I projected the sketch to create our midpoint. So the reason I did that is sore. Midpoint is driven by the initial triangle sketch. If we double click on the original triangle sketch and change the dimensions 200 millimeters and then click stop sketch. You'll see that the midpoint is still exactly in the center. Now, if you remember right after our initial sketch, we used the offset plane feature. So if we want to manipulate the height of our triangle, all we have to do is double click on the offset plane in our timeline, and we can change the dimension and click OK. If there's one thing that I want you to learn in this tutorial, it is the idea that you should always be setting up your models, where you can go back and edit or change sizes without causing any crazy shapes or heirs in your model. Now I know for this pyramid shape, it may not seem like that big of a deal. But as you start to create more advanced components and assemblies, keeping this in mind will save you a ton of time and you'll hopefully avoid a lot of frustration. I'm gonna go ahead and click, undo a few times until we're in the original dimensions and then I'll click Stop sketch. Now we'll want to show out this item so we're not wasting any more three D printing filament that we need to. I'll select Shell from the modified drop down list, click on the bottom surface of the pyramid and then type in 2.5 millimeters for the thickness and I'll click OK, one of the last things will do here is cut out some circles on the side again. This is going to help us save on filament, and it really shouldn't take away much of the shape string. And for those of you who are familiar with three D printing, you likely know that a circular shape like this could be printed without any problems. Since each layer comes out just a bit further, I'm going to hit letter P for project and I'll select one of the sides of the pyramid, then all select all three lines that make up the face of the triangle and then click. OK, I'll hit Letter X to turn on the construction line, and I'll hit Letter L to draw two lines from a vertex to the opposite midpoint. Once we have our Century oId or center point of the triangle, I'll go ahead and click X on the keyboard again to turn off the construction feature. And then I'll hit the keyboard shortcut Letter C for center circle. I'll select where the lines meet. I'll drag out with my mouse and I'll type in 25 millimeters if the tab key toe lock the dimension in place. And of course, click with my mouse to set the circle in place. Now to cut this circle away, all hit letter E for extrude select the circle and for the extent will want to select to object which will allow us to select the inside of the triangle surface again, ensuring that if we change the shell thickness or anything else with the model, then we wouldn't have to go back and edit this extrude cut as it should always go to the inside surface that we selected. Looking at the extrude cut preview you can see that are cut looks right, so we'll click OK to close extrude dialog box. Now we could create the other two holes one by one following the same steps that we just completed. Or we could also mere the extrude cut onto the other two sides of the pyramid. If we take a look at the pyramid from the bottom, it may seem a bit tricky because if we mirror feature straight across, they'll end up at the Vertex of the pyramid and not the face of the pyramid. Therefore, we're going to have to create a few mid planes that we can reference before we use the mere command to create the mid planes. All select mid plane from the construct drop down menu, and all we have to do is select the left face and the right face, and you'll see that it creates a nice mid plane directly in between the faces we selected. So let's right. Click on the bottom face and select repeat mid plane and then we'll select are left face giving us a mid plane between these other two faces. Now we can go ahead and near the extrude cut to the other side's also like Amir from the create drop down menu. Then, in the mere dialog box will need to select features as the pattern type, allowing us to select the extrude cut in. The timeline for the mere plane will select either one and will change the compute option toe optimize because it uses the least amount of code and it will run the fastest. Although I should note the optimized doesn't always work for more complex, smeared objects. Also, go ahead and put a more detailed right up of the three different compute options and the comments of this video. Now, if we click OK, you'll see that it's successfully Meers our extrude cut. I'll select the extrude cut in the timeline right click and select a repeat Mir. This way our pattern type and object are both already selected for us, so we'll just have to select our other mid plane. And that will change the compute option to optimized again and click OK, now the last thing will want to do here is at nice rounded edges to our model Before we export for three D printing, we can hide these planes out of the way by selecting them and hitting the keyboard shortcut , letter V toe view or hide objects. We'll hit the keyboard shortcut letter F for fill it. I'll select the three lines that make up the top of the pyramid as well as all six edges of the circles. Once everything selected, I'll enter 1.5 millimeters for the Philip Radius to give it a nice and subtle rounded edge , and I'll click OK, toe exit the Philip Command. Now, if you do have access to a three D printer and wanna print some of these out, then you can simply right click on the component and select save as STL. From there, you'll have to select the component or the object, and you can either click OK to save the file to your local hard drive. Or you can check send to three D print utility and select your three D printer slicing software. Now I'll go ahead and select Cura, and if I click OK, you'll see that it should open up the file in the slicing software. 7. Day #16 - Fusion 360: Manually Adding Constraints: Hey there it's Kevin Kennedy and welcome to day number 16 of Learned Fusion 3 60 in 30 days . By the end of this tutorial, you'll have a solid understanding of how to manually apply sketch constraints. Infusion 360. Now you may have noticed in the sketch palette. There are a number of different sketch constraints in this video. I'll explain what constraints are, why you should use them, and I'll walk you through each constraint by demo ing What they do to get started all open up the constrains demo file, and I'll put a link to this demo file in the video description so you can follow along in practice. Using these constrains, I'll double click on the sketch titled Constraints Demo, located in this sketch folder of the Fusion 3 60 browser, and double clicking will activate and open up the sketch. Once the sketches opened up, you'll see this sketch palette dialog box. Then, if you look at this sketch palette, you'll want to make sure that your constraints list is toggled to open. So if I just click on the arrow here, you'll see that it will toggle from open to close now, before I cover what each constraint does. It's important that you understand what constraints are and why you should be using them. Constraints allow you to relate one sketch entity to another sketch entity. If you look at the sketch constraint icons in the sketch palette, you'll see that the sketch kin trains use geometric expressions with the exception of Fixed Slash unfixed. Now let's talk about why to use thes sketch can trains. These sketch constraints allow you to maintain certain behaviors when the sketch is updated . Constraints help the sketch stay intact, ensuring the elements don't break apart or move toe unpredictable areas. So to recap this, you'll want to use sketch constraints to maintain the shape of your sketch. So your sketch stays 100% predictable, with emphasis on the 100%. Because if you're constraining and dimension ing your sketches correctly, then you should always know what is going to happen when you make a change within the sketch. Now let's walk through these constraints to show what each one does, starting from the top and working our way down the list. The first constraint we see is coincident, which forces the geometry of to sketch entities to touch now to activate any constraint will have to click on it in the sketch palette, and you'll notice it shows its active by the blue highlight toe. Add a coincident constraints. We can either select a point or a line if I select this line first, then you'll see that as a hover over all the other lines. It on Lee shows the points in this case. Points are all that I can use to complete the coincident constraint. I'll select the end of this line, and then you'll see that the lines are joined together. You'll also notice the cliff icon that represents the coincident constraint was added. So we know which areas constrained now that we've added coincident constraint. Weaken dragged this horizontal line up or down and you'll see that the vertical line will always stay connected. The next constraint is co linear, which forces two lines to share a single access, and they could be at any angle. They don't have to be horizontal or vertical lines. I should also point out that the order in which you select the lines does matter. The first entity you choose will remain in place and the second entity will satisfy the constraint. If I want the top line to be on the same access as this other line here than making sure Colin Ear is active, I can simply click on the first line that will be used as the access. And then as I click on the second line, you'll see that it moved to the same axis and added the colon ear. Google. If now, to escape the constraint feature, I can either hit the escape key on my keyboard. Select be constraint again or I can click the selection button in the toolbar. And if I drag one of these lines around, you'll notice that they will now always stay on the same axis. The next constraint is concentric, which forces circular sketch elements such a circles and arts to share a comment. CenterPoint. So if I wanted to ensure that this circle has the same centrepoint as the Ark, I can activate the concentric constraint by clicking on it. Then I'll click on the entities and either order. If I select the Ark and then select the circle, you'll see that now both energy share the same Centrepoint, which is represented by the concentric cliff. I'll hit the escape key to exit the concentric constraint. I'll go ahead and select the midpoint constraint Now. The midpoint constraint, which is represented by a triangle, will come up often as you draw lines. Infusion 360. The midpoint constraint allows us to force the end point of a line to the center point of a line or art. If I select the end point of this line and then select the bottom line, you'll see that snaps to the midpoint and the triangle or midpoint cliff now appears. The next constraint in the sketch palate is fixed slash unfixed. If I select it and click on a line, you'll notice that it turns green, which denotes that the line is fixed notice. While the position of the line itself is fixed, the in points can still be adjusted now. Personally, I wouldn't recommend using the fix slash unfixed very often, because if the rest of your sketches constrained and dimension properly, then you should be able to update your sketch while knowing what will happen to your sketch . The problem with fixed, lush unfixed is that if you have a line or multiple lines fixed, then you won't always be able to update them without going ahead and unfixed ing them first . And sometimes this can get really messy, especially in larger sketches. The next constraint is the parallel constraint, which makes any two lines parallel to each other. I'll click on the parallel constraint to activate it, and then I'll select these two lines and you'll notice that now, if I dragged them around, they will always stay parallel to each other. The next constraint, all click on, is the perpendicular constraint. The perpendicular constraint forces two lines to remain at a 90 degree angle to one another . An important thing to note is that the perpendicular constraint does not have to be used on lines that air touching. If I select the left vertical line and then select the top right line, you'll see that it made them perpendicular to each other. You'll also notice that because these two lines were Colin ear with each other there now, both perpendicular to the left line, even though only one is directly constrained, as represented by the glitch here. So this is a good example of how constraints could be used in conjunction with one another to constrain sketch entities and amore efficient manner. The next constraint all activate is the horizontal slash vertical constraint, which forces a line to snap to either horizontal or vertical, which ever orientation is the closest. If I click on this middle line, you'll see that snaps to vertical on Google if appears next to it now, the horizontal such vertical constraint can also be used to make points line up with one another. If I select the center point of the circle and then this endpoint of the line, you'll see that there now horizontal and because our arc in circle or concentric the Ark went ahead and moved along with it. Next I'll activate the tangent constraint, which creates Tangent C or a curve touching a line segment at a single point. Now Tangent C is supposed to create a relatively smooth transition. The tangent constraint will create this smooth transition between a line and a circular element for us. I'll go ahead and add change. It constraints to the Ark and the nearby lines by selecting the Ark and then the right line . Now I'll do the other line by selecting the ark again and then the left line, and you'll see that now we have both of lines tangent to the art, as represented by the Tangent Cliffs here. The next constraint all activate is the curvature constraint. The curvature constraint makes the curvature at the transition point equal. Essentially, the curvature constraint can help make organic shapes more smooth, so you likely won't be using it very often compared to some of these other constraints to demo. This constraint will have to draw a spine connecting to the Ark. Also, Lex spine from the sketch Drop down menu. And then I'll draw spine from the edge of the art to some of these other points. And I'll just drag some of these handles here. So it's not a straight then tell you see what the curvature constraint does. I'll select the spine and the Ark. Why holding down the shift key and I'll click the curvature comb in the sketch palette. Now the curvature combs will help. You better understand the transition point of the spine and the ark. If we look at where they meet, you'll see that the curvature comb is not continuous because the transition is not smooth and flips to the other side here. Now, if I select the coverage of constraint and select both sketch entities, you'll see that the comb will change toe have a fluid or smooth transition from the ark to this plein. Now, let's get rid of this coverage of Qom by hitting the escape key to make sure we're not in another command. Then I'll select the arc in the spine, and I'll select the courage or comb icon to turn it off. And I'll hit the escape key once again to clear all commands. The next constraint activate is the equal constraint, which forces two entities to be equal in size. I can select the two horizontal lines at the top, and you'll see that it forces them to be the same size. If I hit the escape key and drag this right point around, you'll see that not only do these two lines state equal in size, but they will also follow all of the other constraints that we have applied to them. The last constraint all activate is the symmetry constraint. The most important thing to note with the symmetry constraint is that it requires three mouse clicks. The 1st 2 clicks will be entities that you want to be some metric, and the third selection will be the entity or line that you want it to be symmetric about. So I'll go ahead and click on this top line and this other line here, I'll click this line in the middle for the line of symmetry. Now you'll see if I hit the escape key and drag this top line around, both lines will stay some metric from this middle line. Now, before I end this video, I'll show you a few other quick tips. If you right click on any sketch entity, you'll see that it shows all of the available or relevant sketch constraints and the marking menu. Now, if I go back and select multiple sketch entities while holding down the shift key and then right click again, you'll see that the entities that you selected will affect the constraints that are available in the marking menu. Now, in this video, I covered how to manually add constraints, but some constraints will automatically be applied while you sketch out entities. For example, if I hit the keyboard letter L for online and draw a line out you'll see that it will automatically add a horizontal constraint if I let it snap to the grid. So it's important that as you draw different sketch features out, you take notice of what sketch constraints are automatically applied and day number 17 will take a look at how adding dimensions can help us fully constrain our sketches and why fully constraining sketches is an important concept to understand. 8. Day #17 - Fusion 360: How & WHY to Contsrain Sketches: Hey there it's Kevin Kennedy and welcome to day number 17 of Learned Fusion 3 60 in 30 days . By the end of this tutorial, you'll have a solid understanding of how to use dimensions and constraints. Toe fully constrain your sketches. You'll learn a few dimension tricks, and I'll explain and demo why it's important to fully constrain your sketches. Let me start off by stating that Fusion 3 60 does not require sketches to be fully constrained. But it's a good practice to always fully constrain your sketches, which will cover in just a minute. But first, it's important to note that the way you define or constrain your sketches will differ per each design. This is why it's important that you come up with a strategy for how your sketch entities relates one another at the beginning of each model. Now this strategy is often referred to as the sketches design intent. Personally, I recommend sketching out your design on pencil and paper before you start sketching anything out. Infusion 3 60 Doing so will help you think about how the sketch should be constrained before you even get too caught up in the computer. Now for this demo, I went to draw this square washer plate, which is essentially a square with a hole cut out of the middle. While looking at this sketch, I can ask myself, What do I know about this object? Without knowing any of the dimensions? I see that all four sides appear to be equal. I see that the lines are perpendicular at the corners and the lines opposite of each other appear to be parallel. And it appears that the center of the circle is located directly in the middle of the washer plate. So let's start off by creating a new component from the assembled drop down list and all. Title it square washer and click OK, now let's create a sketch for this washer plate so we can walk through the steps of constraining in dimension ing it. We'll hit the keyboard shortcut letter are for rectangle, and I'll select the top plane now before we click on anything. If you look in this sketch palette, you'll see that we can switch from a two point rectangle to a three point rectangle or a center rectangle for this washer plate will want to use thesis. Enter rectangle because the center rectangle will already have a nice center point for us to reference for the circle cut out. This is why, as you continue to learn fusion 3 60 it's important that you understand what all of the sketch tools do. The more you know you'll become more efficient, and it will help you eliminate unnecessary steps. So I'll select the center rectangle icon, and I'm just going to click away from the origin out in space here and I'll drag out with my mouse and click at a random distance. And just so you can see the difference, I'm going to select a two point rectangle and draw that out right next to our center rectangle, and I'll hit the escape key to clear all commands. Now let's look at both of these rectangles, so you'll notice a few things here. As I mentioned in Day Number 16 you'll see that Fusion 3 60 will automatically apply some constraints when using these pre defined sketch entities. Now, using the two point rectangle tool, applied vertical slash horizontal constraints toe all four lines. Now here's a little tip for you. If a constraint is automatically applied and you can't seem to remember what it stands for , then simply click on the cliff or icon and you'll see in the lower right hand corner. It states the type of constraint you'll see this one says horizontal. And if I click on this one for the right line, it states that it's a vertical constraint. Now, looking at the centre rectangle be created, you'll see that it automatically created some different constraints. For us, it created some parallel constraints. A coincident constraint were the lines meet in the middle and a perpendicular constraint in the corner? Now that you see the difference here, I'm going to delete the two point rectangle by selecting over the entire object. And then I'll hit the delete key on my keyboard. As we go a bit further, you'll understand why we ended up going with the center rectangle. Now we'll once it fully constrained or define the center rectangle before we go ahead and turn it into a three dimensional object. That way we have 100% control of the sketch if we go to update the size of the sketch or change anything with the square washer plate. So in this current state, you'll notice that the lines of rectangle are blue, which means that they're not fully constrained, and we can still move them around. Now, if I click and drag on these lines, you'll see that I can move them up and down side to side. Or I can drag points and change the overall size of the rectangle. So our goal here is to figure out how to turn all of these lines from blue to black because black sketch entities signify that they're fully constrained and they can't be moved unless we update the dimension or the constraint that is driving the sketch again. Doing this will give us full control of the sketch. So if we update the size, we can keep the shape that we originally intended. Now the rule of thumb is toe. Always use constraints first, and then dimension your sketches second, and there are a few different reasons for this. First, the fewer amount of dimensions we have, the easier it will be toe update the size of our model. Should we need to second, the fewer dimensions we used, the fewer amount of problems will likely run into such as accidentally over defining our sketch, which means that the dimension cannot be altered because it's already driven by other dimensions and or sketch constraints. So if we look back at our original sketch, notes will see that it appears that all four sides are equal. Therefore, using the equal sketch constraint, we can force all four lines of a rectangle toe always be equal. So holding down the shift key, I'm going to select the left line and the top line of the square, and I'm going to click on the equal constraint in the sketch palette. Now. The reason I only applied the equal constraint to the left and top line is because they already have parallel constraints. If I reactivate the equal constraint and select the other two lines, you'll see that it won't let us add the equal constraint toe all four lines because it would over constrain the geometry, making those constrains unnecessary. Now you'll notice that the lines of our rectangle still aren't fully constrained because they're still blue. So if you're ever wondering why they aren't fully constrained, you can simply click on any lines or points and drag them around. If I click and hold on the center point of the rectangle, you'll see that I can drag it around. Now we can use the coincident constraint to snap the center of the rectangle to the center origin. I'll activate the coincident constraint. Click on the center origin, and then I'll click on the middle of the rectangle and you'll notice the rectangle will snap to the center origin. Now you should also notice that the center construction lines and the center point of the rectangle are now black or fully constrained. So if I click and drag at the center point, I can no longer move this rectangle around. But we can still change the size of the rectangle by dragging the blue lines, which aren't fully defined yet. Now, one thing to know. I normally would have started the center rectangle sketch off the origin point. But for this demo, I wanted to show you what happens when you don't. With that said, I would always recommend starting your first sketch of each file at the centre origin unless you have a good reason not to. Now, let's go ahead and fully constrain the lines that are still blue. To do this will have to add a dimension toe one of the sides. So I'll hit Letter D on the keyboard for Dimension. And if I click on the top line, drag up with my mouse and type in 100 millimeters and click enter. You'll see that now Our sketch is 100% black or fully constrained, and I can't change the size or move any of these lines by dragging them around. Now the only way I can change the size is by changing this one dimension that we just added . Now let's go ahead and add our circle cut out in the middle. I'll activate the Centre Circle sketch tool with the keyboard shortcut. Letter C. I'll click on the center Origin Point, Type in 50 millimeters for the dimension, and I'll click with my mouse again to snap the circle into place. Now you'll see that our circle is also represented as fully constrained with black lines because the dimension we added and the fact that we drew it on the center point, which automatically added a coincident constraint. Now to delete a constraint that is automatically applied, all you have to do is click on it and hit the delete key. If I click on the middle of the circle, you'll see that there are four different coincident constraints, and if I hover over the glitz of each one, you'll be able to see what it relates to. I'll select the second constraint, and then I'll hit the delete key, and now you'll see that the circle is blue because I can move it around so I'll go ahead and reapply a coincident constraint by activating coincident in this sketch palette, I'll click on the center origin. Now let's go ahead and extrude are square washer up by hitting the keyboard shortcut letter E for extrude. I'll select the sketch and type in five millimeters for the thickness and click. OK, at this point, I want to show you a few dimension tips. I'll double click on the sketch in the timeline to reopen it, and if I hover over the dimensions, you'll notice that it gives the dimension number. So we have D one colon 100 millimeters, where the number one represents the dimension number. So if we hover over the circle dimension, you'll see that the dimension number is number two and these numbers are created based on the order in which you dimension entities. Now one cool thing about dimensions is that we can use functions and then dimension field to make them a bit more robust. So if I knew that, I always wanted this inner circle cut out to be half the size of my overall square, I could apply a function toe. Always be half of the squares dimension. To do this, I'll click on these circle dimension, and I'll type out D one to reference the first dimension or the dimensions of the outer rectangle. All type a Ford Slash to represent that I want to divide. And then I'll type out number two because I wanted to always be cut in half or half of the rectangle. Now, if I click enter, you'll see it, says FX for function and shows the diameter of 50 millimeters. Now, if I were to update the original dimension to 150 millimeters, you'll see that the circle dimension updates as well. So now it's automatically been changed to 75 millimeters. So once again, this is why it's super important to think through your designs before you start sketching anything out on the computer also point out that you have to use functions like this with caution. You don't necessarily want to reference dimensions all the time, especially in larger models or sketches, as it can get quite hard to remember what each function or dimension actually represents. Now, to summarize what we did here, we added constrains first, so we only had ads who dimensions to fully define and constrain our sketch, which allows us to easily go back and simply change one dimension if we decided our square washer needs to be smaller or larger. If we take a look at this other file, I've gone ahead and created the same washer. But I didn't follow these best practices, and you'll notice if I double clicked. Open up the sketch. The sketch is not fully constrained or defined Now. If I goto update the dimension, you'll see that it totally throws off the whole entire shape, and I'd have to also manually update the other dimensions here. Now it may not seem like that big of a deal, because this square washer is a fairly simple object. But as you can imagine, as you start to three D Model Mawr. Complex objects, especially ones that contain multiple sketches. It can really suck up a lot of time and cause a lot of problems if you don't plan ahead and fully constrain your sketches based on your original design intent. 9. Day #18 - Fusion 360: Turning an .STL Mesh into a Solid Body: Hey there it's Kevin Kennedy and welcome to day number 18 of Learned Fusion 3 60 in 30 days . By the end of this tutorial, you'll be able to turn in STL or O B J Mesh file into a solid body. We'll take a look at a few different options while doing this, and we'll talk about the meaning behind some of this commonly used terminology and the world of three D printing. Before we get started with actually converting the mesh model, I want to cover some of the terminology to ensure we're on the same page. And so you actually understand why we're converting the model to start off will discuss a mesh file. Now, if you're familiar with three D printing and you used dot STL files or 30.0.0 B J files, then you work with mesh files all the time. Now a mesh file is a collection of vergis ease, edges and faces that define a three dimensional shape. Now I found this great image on Wikipedia that breaks down and mesh, all linked to the image in the video description, so you'll see that it shows that mesh files are created with Firdous ease edges and faces, which all create the polygon sides or surfaces of the object. So looking at the last image here, probably the most important thing to know about meshes is that their surface models now, to help you grasp the concept, we can compare it to a real life. Example. Origami. If we look at this object made out of paper, will see all the different shapes and surfaces that make up this model. Yet the object is still hollow on inside as it solely made up of the surface geometry. Now real quick. Let's take a look at the difference between the two most common types of meshes. Which R S T L and O. B J Files. Now an STL file is the native file format for stereo lithography, and it's often referred to as the acronym that represents standard triangle language or standard test elation language. Put simply, an STL file is a type of MASH file created with unstructured triangular surfaces. So again it's just making up the outer surface of the model, and it's not a completely solid object now, on the other hand, we have O. B. J files and really the only difference between an STL file and in O b J file is that the O . B J file. Display some extra data on the surface, so you see that STL files are always gray, whereas O. B J files can contain color and texture data, which are displayed on the outer surface. Now the color and texture map are most commonly captured by three D scanners, which is why most three D scanners air going toe output. Your O B J file. Now the last term that you'll need to understand here before we do a little demo and actually convert a file is the term be rep. Now be rep stands for boundary representation and could be seen as the opposite of Hermesh files, as it's a completely solid and watertight model. Now a beer up file is made up of Topol logical and geometric information. Alrighty. So now that you're familiar with some of the common terminology, let's take a look at how to use Fusion 3 60 to convert an STL file to a B rep solid body. The first thing that will want to do is make sure that the mesh workspace is enabled to do this, I'll select the preferences menu from the profile drop down list, and then I'll select preview and you'll see that we Cantat go the mesh workspace on and off by clicking the check box. Now, after clicking the check box, you'll have to hit the apply button and then the okay button. Now a lot of fusion 3 60 users get STL files from thingy verse dot com, and they want to modify them to fit their own needs, or they simply want to customize them with the name or logo. So I've gone ahead and downloaded this phone stand from thingy verse, and the first thing I'll have to do is import it into effusion. 3 60 And there are two main ways that we can do this. The first way would be to open up the data panel and click the blue upload button. Then, if I select the file, I can upload it and Aiken double click on the file toe. Open it once it's been successfully uploaded. Now the second way I could do this is to simply go to the insert menu, select insert mash from the drop down list, and then I'll go ahead and select the file and you'll see that before we work on the file. It allows us to change the orientation. Now I want the top of the phone stand to be the top of my orientation and the View cube, so I can either drag the sliders around or I can select the flip up direction in the insert mesh dialog box. And I can also hit center to move it to the center origin. And if your file is floating up in space for some reason you can hit. Move to ground to move the file to the XZ for the X Y plane, depending on how your orientation is set up, so I'll go ahead and click OK to confirm these orientation changes. Now, if I go to the workspaces menu, you'll see that it's still can't switch to the mesh workspace. And that's because the mesh work space does not allow design history to be captured. So we'll have to turn off the design history by right clicking on the file in a fusion 3 60 browser and I'll select Do not capture design history and I'll click the continue button to confirm now If I go back to the workspace selection menu, you'll see that I can change to the mesh workspace. I'm also going to go ahead and change my visual style. So it's a bit easier to see all the triangles, the makeup, the mesh under the display settings, all selective visual style and then all select, shaded with visible edges on Lee. And you'll see that if I zoom in, we can now see all of the vergis, ease edges and faces the makeup, the mesh model. Now what confuses a lot of users here is that we'll actually need to be in the model workspace in order to convert this model, so I'll select the model workspace. And now, to convert this mesh to a solid body, all we have to do is right. Click on the mesh and select mesh to be ready and you'll see in the dialogue box. We can have it create a new body or a new component, so I'll go ahead and select new components and then click OK, now I'll switch over to another example real quick, because if you imported a fairly complex model, then it's very likely you'll get a warning message at this point, stating that there are too many facets or number of faces for fusion 3 60 to convert the model. So, looking at this example here, it looks like it has a little over 1.5 million faces, and fusion 30 60 can really only compute approximately 50,000 facets. So before trying to convert, will first have to reduce the number of facets. To reduce the number of faces, you'll have to switch to the mesh workspace, and then you can select reduce from the modified drop down list, and then we'll have to select the mesh faces or the entire body. So when some scenarios, you may only want to select a certain area of the faces and then others will want to go ahead and select the entire body from the Fusion 3 60 browser, the next option you'll see, is the reduced type. Now, adaptive means that fusion will adapt the surface triangles. How it best fits. The shape and uniform will force them to all the uniform in shape and size. So for this complex object, I'll leave it at adaptive, so it doesn't totally skew the overall shape. Now We want to reduce the amount of faces, so we'll have to select face count for the reduced target. And then, for the number of faces like we talked about a minute ago will have to have this number under 50,000. And it's a good idea to a much lower as the more faces your file has, the more data fusion 3 60 has to process, so your file will be much slower the more faces you have. So I'm just going to type out 30,000 and click OK, and this may take a while to process because 30,000 is still a lot of faces. Once it's done processing, you'll see that if we switch back to the model workspace, weaken right click on the mesh and select mesh to be read, and this time it will convert it for us, although it will give us a warning again because there are a lot of faces which may slow down the file. So I always recommend reducing the face count as much as you can without destroying the overall shape. Now let's switch back to the phone stand demo and look at a few more things that we can do after we convert the file, I'll go ahead and rename the component by double clicking on it in the browser and I'll type out phone stand and I'll make sure that the mesh body is hidden and then our new component is visible and activated. Now. Fusion 3 60 did a pretty good job of processing this file and turning it into a solid body . But you'll see here that we still have a lot of triangular surface faces that make up our solid body, and sometimes things can get in the way of us altering the design to our specific needs. So one thing that we can do is reduce the number of faces by merging them together. If I wanted to work on this flat surface here, these triangles will get in the way. So let's go ahead and get rid of some of them now. I could zoom in and select all of these one by one, but an easier way would be to use the paint selection tool, which is going to allow me to click with my mouse and drag over all these faces to select them much faster now, before using the paint selection. I want to set the selection priority to select face priority, which will help ensure that we don't select the entire component. And if I go back up to the menu and look at thes selection filters, you'll see that we can see that activating these select face priority churned all these other options. Off and on, Lee left, the body face is turned on, which will again help us select only the faces. Now, with the paint selection activated, I can click and drag across a number of faces. And if I miss any faces, I'll just hold down the shift key and select them. Then I'll switch to the patchwork space and I'll select emerge from the modified drop down list, and you'll see that I can continue to select emerge faces to really clean up this solid body model so it doesn't have so many faces on it Now. Having less faces will really allow us to focus on the tools in the model workspace, and it won't restrict us a smudge as we try to modify our new solid body. Now there's one more thing I want to show you here in order to summarize what I covered in this video. If I turn on these section analysis in order to look in the side of the object, you'll see that RB reptile is completely solid. And if I toggle the STL mesh file back on and turned the component or solid model off, you'll see that it's a thin surface model created with hundreds of mesh triangles. So again, this is another great example of the difference between a mesh and a B rep or solid body. 10. Day #19 - Fusion 360: Hinged Box for 3D Printing (Part 1 of 2): Hey there it's Kevin Kennedy and welcome to day number 19 of Learned Vision 3 60 in 30 days . By the end of this tutorial, you'll be able to three D model a hinged box for three D printing. We'll take a look at how to set up user parameters, how to apply in as built joint and how to prepare the part for three D printing before we get started with the box. Let's make sure that our preferences are set up the same way I'll click on my user profile and then preferences, and I'm going to make sure that my default modeling orientation is set to Z Dash up because that's how most three printer slicing software's air set up. If you do have to change any settings here than, be sure to select the apply button and then the okay button. Now, if I go down to my display settings, you'll see that I'm in the photo booth environment and that my visual style is set to shaded with visual edges on Lee. You'll also want to make sure that your layout grid and snap to grid are selected under the grid and snaps menu and last but not least, you'll want to double check that your in the model workspace. Now let's start creating the bottom lid of our box by first creating a new component. I'll select new component from the assembled drop down menu. Now in the new Component Dialog box, I'll make sure that empty component is selected, and then I'll type in bottom box for the name and I'll click. OK, now we can begin to draw the box shape. I'll call the Rectangle Sketch Tool with the keyboard shortcut letter are, and I'll click on the bottom plane. Then I'll click on the center origin and drag out with my mouse. I'll type out 70 millimeters, hit the tab key toe, lock the dimension in place, and then I'll type out 70 millimeters for the other side. I'll hit the tab key once again, and then you'll notice that we can't do anything other than click on any side of the origin point. So I'll just click in one of the directions and real quick I'll point out like we talked about in day number 17. We always want to make sure that our sketches are fully constrained and mentioned as signified by all of the sketch lines turning black. Also, before we move on, let's find the sketch in the Fusion 3 60 browser, and we'll click on the word sketch in Rename It Box. Now, before we get started with the box shape, will want to set up some user parameters. I'll go to the modified drop down menu, and then I'll select change parameters from the bottom of the list. Now, I know a lot of you are just getting Infusion 3 60 this may even be your first Riel CAD program. So let's go ahead and take a minute to discuss what parameters are. If we look at the parameters box, you'll see that we can add a name, a unit and expression a value. And we can also add some comments or notes. At its core. Parameters are mathematical variables that weaken set up and they're defined by value. We can then call those variables by their names and order to find sketch elements, feature sizes and geometry across different components. When we set up parameters, we can define them by a single numerical value, an equation, or we can also reference other parameters So in some use cases, we may set our parameters up so we can change one single parameter in which all the other aspects of the model are fully updated simultaneously. Now, using parameters like this will give you a tremendous amount of control over the model. So to set up, some user parameters will click on the plus sign, and a dialog box will pop up. Well, then first, enter a name. So the first parameter I'm going to set up is the wall thickness for a three D print. Now, as you're typing out names, you'll notice that we can't use spaces or hyphens. So it's good practice to type out the names in Camel case, where each new word is capitalized for the units, we will leave that set two millimeters, and then we'll type in 1.3 for the wall thickness. As I found that that works well with most consumer level F D M three D printers for the comment. We can leave this blank if we want as it's not required, or you can type something out that may help a colleague understand the parameter. So I'm a type something out like F D M three d printer thickness and then I'll click. OK, now we're going to add two more user parameters. We'll click on the plus symbol again and add box height and we'll enter 70 millimeters and click OK, and for the last user parameter, we're going to set up the gap of our hinge. I'll click the plus sign once again and I'll type out gap and then 0.5 for the value and click. OK, now again, These are just some user parameters that we've set up to start out with. But we can always go back to this menu at any time to change these parameters. Or we can always add additional parameters and let's go ahead and click OK to close the parameter dialog box. Let's extrude this sketch to make a cube. I'll hit the keyboard shortcut letter E for extrude and then click on this sketch. Now, if we look at our extrude dialog box, you'll see that weaken type in the distance of our extrude. And we can also type in our user parameters in this field so I can delete all of this text and then start to type out box height and you'll see that after I type out the first letter , it recommends the box height user parameter for us so we can just go ahead and click on that and we'll click. OK, and if we look at our model from the home position, you'll see that the user parameter worked as expected, and we have a nice 70 millimeter cube, as that was the value we set for the box height. Parameter at this point will need to make the Cube hollow by using the shell tool. I'll select show from the modified drop down list and with the shell tool. If we just select one face, it will essentially cut away that face and create the thickness we apply. But we want our cubed to be completely closed because we'll use the split feature later on . So in order to keep the object completely closed, we'll have to select all six faces of this cube, and we'll need a type in our user parameter wall thickness for the inside thickness, and we'll click OK now because our shape is completely closed. It's hard to tell if this actually works. So the check that the shell worked properly will go up to the Inspect menu and then select section analysis. We'll click on any side of the Cube and then dragged the arrow in a bit. We can see that are Shell did, in fact, work as we wanted, so I'll just hit the cancel button in a dialog box. Now we'll need to create a plane in order to splitter box in half. We could use a mid plane from the Construct Drop Down menu, but I want to show you another thing that we can do with user parameters. So I'll select Offset Plane, and then I'll select the top of the Cube for the distance. I'll type out the minus symbol because I want this to go in the direction of my cube, then all type out the box height parameter, and we'll divide it in half, using the Ford Slash and then the number two and you'll see that that put our construction plane directly in half or the middle of the cube. And if we go toe, update the box height later on. Our construction plane will always be split directly in the middle because we used half of the box height user parameter, so I'll go ahead and click. OK to confirm these results. I now want to split this Cuban half, so I'll select split body from the modified drop down menu. I'll first have to select the body to split, so I'll select the Cube and then I'll select the construction plane for the splitting tool and then click. OK, now, if we take a look in the body folder of the Fusion 3 60 browser will see that we have a top body in the bottom body. And let's go ahead and rename these real quick and we're done using this construction plane . So I click on it and simply select the keyboard shortcut letter V toe. Hide it now, before we go any further. Also make sure to save this I'll click the Save icon and type out hinged box and click Save . Now we'll need to create the hinge of the box. All right, click on the face of the bottom body and click create sketch. Then, if I zoom in here, we're going to want to create our hinge in the middle of the two bodies. I'm going to first hit the keyboard. Letter L for line, and I'm going to draw a line 2.95 millimeters from the center over to the right. Then I'll hit the keyboard shortcut letter C for center circle, and I'm just going to click on the end of the line and draw out three circles as well. Dimension them in just a bit. Now we'll hit the keyboard letter D for dimension, and I'll click on the innermost circle. I'll type the parameter wall thickness. Then I'll hit the letter d again and I'll select the inner circle and then the second circle. And I'm going to type out Gap as this is going to create the gap between our pin and the hinge. And finally, all hit letter D once again. And I'll select the second circle and then the third circle, and I'll make this one the parameter wall thickness. And then I'll hit the escape key to clear the dimension command. I'll hit letter L for line again, and I'm going to draw a line from the edge of the bottom base to the outermost circle, and I'll make sure that they line snaps in where its tangent to the circle and I'll go ahead and do the same thing on the top. Then I'll click Letter D for Dimension again, and I want to add a 45 degree angle for this line as 45 degrees is kind of our maximum threshold for getting a nice angled surface and three D printing. So I'm just going to select both lines here and then type in 45 degrees. And once again, I'll repeat the same step for the top, and you'll notice that our sketch is completely black, so it's fully constrained. I'll go ahead and hit, Stop sketch, and then I'll rename the sketch in the Fusion 3 60 browser by clicking on it. And then I'll type out the word hinge. Now to complete the hinge and actually three d print the box, you'll have to click the link to Part two in the video description 11. Day #19 - Fusion 360: Hinged Box for 3D Printing (Part 2 of 2): Hey there, it's Kevin Kennedy. And welcome back to part two of day number 19 of Learned fusion 3 60 in 30 days. If you haven't watched Part, one can be sure to click the link below in the video description and watch that first in the first video, We created Our Box and created the sketch for Hinge. Let's go ahead and turn the henge sketch into a three dimensional object. I'm going to zoom in and look at the sketch from a slight angle, and I'm going to hold down the shift key and select the bottom and then the outermost circle and then right click on the selection and click on press Poll. Then I'm going to change the extent to to object. That way, if I ever update the size of the box, the hinge will automatically update for us. Also select extend faces under chain faces and then I'll select new body as the operation so we can hide this hinge. As we build the other parts, I'll click OK and then rename this bottom hinge in the Fusion 3 60 browser. Then I'll hide the bottom hinge by clicking on the light bulb in the browser, and I'll re show the hinge sketch this time while holding down the shift key, I'll select all three circles and the top hinge All right, click again and select press Poll. And then we'll change the extent to to object again. We'll also select extend faces for chain faces and then make sure that new body is set as the operation. After clicking okay or rename this to top hinge in the browser and then click the light bulb. I kind to hide the body now, making sure that my sketch is still on all select on Lee the inner Circle and I'll hit letter E for extrude, and I'll extrude this to the edge of the box. I'll change the extent to to object. Once again, we'll also have to select extend faces for chain faces and then make sure that new body is set as the operation. After clicking, Okay, I'll rename this body to pin, and for now I'll go ahead and hide the pin. So up to this point we have the form of our box and we have part of the hinge done, but we need to break up the parts of the hinge so they actually interlock properly. I'll go ahead and hide everything except the bottom box and then right click on the top surface of the bottom box. Here. Annul, select, create sketch I'm going to hit letter are on my keyboard for rectangle, and I'm going to draw a rectangle starting at the center origin. I'll make it 5.5 millimeters long so it's as long as our hinge and then for the with all type out wall thickness. To call that parameter at this point will want to draw a few more rectangles for the gaps, so this hinge will actually twist and work properly. All hit letter are on my keyboard to draw a rectangle right next to this one. I'll make it 5.5 millimeters long hit the tab key to lock the dimension in place and for the with all used the gap parameter. Now I'll want to mere these rectangles in just a second, so I'll first need to draw a line down the middle with letter L for lying and before I draw the line off select construction in the line dialog box. Then I'll click in the middle here where you see the triangle or the midpoint constraint and I'll just drag out to a random distance, click with my mouse and then hit the escape key. Now, before we mere I'll have to create one mortgage app rectangle, and I want these hinges to be divided up in approximately thirds. So I'm going to hit L for line again and I'll draw another construction line down 11.5 millimeters. We'll hit the tab key to lock the dimension in place and then hit the escape key. I'll draw another rectangle with Letter R, and I'll click on the endpoint of line and make this 5.5 millimeters long at the tab key and used the Gap user parameter for the with. Now it's important to note that I'm hitting the tab key after typing out these dimensions in order to lock them in place. And before I click with my mouse to set the rectangle, I want to make sure that the construction is turned off. Next, I'll select the mere sketch tool from the sketch drop down, list our click and drag over all of the rectangles to select them. I'll select the construction line as the mere line and click OK, and before we go on, I'll double check that. All of my lines are black, signifying that they're fully constrained at this point. All hit letter E for extrude, and then I'll select all of the Gap rectangles or all of the rectangles here except the outer, too. Then, in the Fusion 3 60 browser, I will turn on all of the bodies except for the pin, because we need that to be a solid all the way across in the extrude dialog box. I'll change the direction to two sides all select all for the extent of both sides and will make sure that the operation is set to cut and the last thing I'll check here is the objects to cut. So I'll toggle this open and I want to make sure that the bottom hinge and the top hinge are selected and I'll click. OK, now, if you look in the Fusion 3 60 browser, you'll see that we have all kinds of different bodies because we cut our hinge into multiple bodies, so we'll have to delete a few of these in order to get our hinge toe work I'm going to turn off the first and third parts of the top hinge. By going through these bodies and seeing which ones they are, you'll notice when I hover, they have transparency, and when I select them, they turn blue. I'll also go ahead and turn off the middle body of the bottom hinge. Then, ah, hold down the command key on my Mac or the control key. If you're using windows and I'll select the bodies that we just turned off and all right, click and select. Remove because remove will take the features off the browser, but it will keep them in the time line down here at the bottom. So if I were to go back through these steps, I could see that in the history, whereas the delete key will get rid of all traces of the object. And if we go ahead and take a look at the hinge, you'll notice that we deleted the opposite parts. So each part of the hinge actually has space to revolve around that center pin. So at this point will want to create a component for the top of the box so we can then rotate the box around and order to three D. Print this all right, click on the top body and I'll click. Create components from bodies. Now you'll notice that this place that component within the bottom component that we started off with, which we don't want. So a click and drag the top body component to the top of the browser tree and you'll see that it is now nested as the same level as the bottom box component. I'll go ahead and rename it by double clicking on it and typing out top box. And if I toggle these component folders back toe open, you'll see that some of our top bodies are still in the bottom component. So we can just hold down the command key on Mac or the control key on Windows and select all of the bodies with top. And I'll also turn on the pin and select that as well, and I'll click and drag all of them to the top box component. Now, if we toggle each component on and off, you'll see that we have the bodies correctly nested under the components. At this point, the last thing will need to do is at a joint so we can rotate the lit around. That way we can three d print the box with both lids touching the build plate surface. I'll go up to the assembled menu at all. Select as built joint, which allows us to position components relative to one another, and it also lets us add emotion. I'll select both components, and you may see your box rapidly shake here because the motion was set too rigid. So we'll want to change that to revel oot. And then I'll zoom in on the pen and I'll select the center of the pin or these circle here . And if I go ahead and zoom out and play this motion again, you'll see that our box is revolving around the pin just like we wanted. So I go ahead and click. OK, now I can double click on this Revolution arrow and you'll see that I can open and close the lid of the box by dragging the slider around. Now you could print the box with the lid in any direction, but to be most efficient and to come out with the best print quality will want to type out 180 degrees for the rotation. So doing this will put both lids of the box flat to the build surface, and I'll go ahead and click enter on the keyboard. The last thing I'll show you here is how to shrink this box size down so you can three d print the hinge without having to wait for the entire box to print. And this is a good idea when coming up with new objects. So we contest functionality without wasting time and filament. I'll double click on the original box sketch in the browser, and I can change the length of the box to 10 millimeters, then hit Stop sketch and we can change the height by editing our user parameters. So, if you remember, will have to go up to the modified menu and then select change parameters and all changed the box height value to 20 millimeters and click. OK, now, if I zoom in, you'll see that our hinge size actually didn't change one bit, which is what we wanted. So again we've shrunk our box size, so this will print much faster and so we can test out the hinge and then, if the hinge does print correctly. We can always go back and change the parameters to make this box any size that we want. Lastly, to three d print this box. I can right click on the top level Assembly and click Save as STL and in the Savers STL Dialog box. I will make sure that the refinement is set too high. And then I can either output to a specific slicing software, or I can always uninsulated this click. OK, name the STL file and save it to my local hard drive. 12. Day #20 - Fusion 360: One-Part Mold: Hey there it's Kevin Kennedy and welcome to day number 20 of Learned Fusion 3 60 30 days. By the end of this tutorial, you'll be able to three D model a simple one part mould for three D printing. We'll take a look at how to use the combined feature to subtract one body from another. Also, stay tuned for day number 21 where we'll take a look at how to create a more complex, two or three part mould to get started. I'm just going to three D model, a simple key chain, and will make a one part mould from it that you can three D prints, which can come in handy if you want to make resin replicas for faster and smoother reproductions. Now be sure to check out the links in the video description with my favorite mold release and resins. If you're going to work with three D printed bolts, I'll select new component from the assembled drop down list and rename it key chain before clicking OK, then I'll select box from the create drop down menu. I'm going to select the top plane and then click on the top plane of the view cube toe. Look directly at the top. Then I'll click on the center origin and drag out with my mouse. Well, type in 50 millimeters for the length. Hit the tab key to lock the dimension in place and then 35 millimeters for the with also followed by the Tad Key. And then I will click with my mouse to set the box Now because we use the box feature. It saved us that extra step of having to hit extrude, and we can simply enter the height of three millimeters and click. OK, now I'm going to round the edges over using the keyboard shortcut letter F for fill it. I'll select all four sides, and then I will type out seven millimeters for the distance and click OK at this point, Let's go ahead and add a whole for the key ring. We'll hit the keyboard shortcut letter l for line, and I'm going to click on the top of the key chain. And then for this first point of the line, I'll select the mid point at the top where you'll see that triangle or midpoint constraint pop up. Then I'll type out five millimeters. Hit the tab. Key toe Lock the dimension in place and click with my mouse to place the line. Now that we have the endpoint for where we Want the whole to go, I hit the keyboard shortcut letter H for Whole and I'll click on the top plane of the key chain to get the whole to snap tour lines and Point will have to click reference in the whole dialog box and then select the end point of the line and you'll notice that it immediately snaps into place. We can also change the whole settings in the whole dialog box. Ah, select simple, simple and flat because we just need our whole to go through for the key ring. I'll change the depth of the whole 23 millimeters or the thickness of our key chain, and then I'll change the with 25 millimeters and click OK, if you're following along and making your own key chain, you can customize it at this point by either adding some text or an SPG logo. I'm going to head up to the insert menu and select Answer SPG, and I'll select the face of the key chain. Then in the SPG Dialog box or click on the open folder and I'm going to select the product design online logo. You'll see that the logo is way too big and way off the key. Shane. So I'm just going to use these sliders to resize and reposition the logo. Until I'm happy with it. I want to add some thickness to the logo, so I'm going to right click and select Press Poll. I'll make this first section one millimeter thick. Then I'll repeat the steps to the other two parts of the logo, making sure that all of the operations are set to join. So we have just one body for the key chain. So now that we have a fairly simple key chain that we can create a one part bowled out of I'll just toggle opened the key chain component. Go ahead and rename the body to key chain by double clicking on it and typing out key chain now to create our mold will need to create another box, and then we'll use the key chain. Or if you would like to replicate something else, then you'll have to make sure that you have a body in order for the combined command toe work. So if you've imported an STL file from thingy verse, then you'll need to convert that from a mesh to be read. And if you need help with that conversion, you can watch my other video, which all linked to in the video description, all now select box once again from the Create Drop down menu and I'll click on the X Y plane. I'll select with my mouse in the upper left hand corner. And then I just want this to be big enough to encompass the key chain or whatever model you're using. Here. I'll type in 60 millimeters for the length and hit 45 millimeters for the with and I'll click with my mouse. And the box dialog box will make sure that the operation is set to new body and then I'll go ahead and look at this box from the front view. I want to make sure that the height goes over top the entire key chain, and I'm just going to type out eight millimeters, which should be plenty, and then I'll click OK, then, before doing anything else or rename the body that we just created by double clicking on it in the Fusion 3 60 browser and I'll type out mold for the name. I'll go ahead and click the Save icon at the top and type out one part key chain mold, as it's always a good idea to save your model before you go any further at this point, are key. Chain and mold for the box are taking up the same space so that help us see what we're doing here. I'll first activate the top level component by right clicking on it and selecting. Activate. Then, all right, click on the mold body and I'll find opacity control. And I'll change this to 50% and you'll see that changing the opacity control will help us better see what we're doing. As we go ahead and cut the key chain away from the mold box, I'll select the combined tool from the modified drop down list. First, you'll need to select the target body, which is going to be the object that you want to cut away from or add to. So we need to select our mold body, then for the tool body will need to select the key chain or whatever body that you're cutting away in order to make a one part mould. And if you're having trouble selecting the body in the graphics window, remember that you can always select the body in the Fusion 3 60 browser on the left hand side. Well, then, have to change the operation to cut because we want the tool body or, in this case, the key chain to cut out the material of our box. Now I can select new component if I want the mold to be added to a new component, and I can select keep tools which will keep the body or bodies that you had selected for the tool bodies. Should you need a reference them or use them again in this file. Now, after clicking OK, we'll have to turn off the original bodies by selecting the light bulb in the browser, and then I will also go ahead and turn the opacity back to 100%. So it's easier to take a look at the mold now that we have our one part mould, we can look at the draft analysis to see how well the object is expected to pop out of the mold. I'll select a draft analysis from the Inspect drop down list. Then I'll select the mold, and we have to also select an access or face for the direction that the item will pop out of the mold. So I'll go ahead and select the top face here of the whole knockout. It's also important to note that before you click OK, you can also set the tolerances in the bottom section of the dialogue box. I'm just gonna leave these to the defaults and click OK. Then you'll see that the draft analysis will color code everything. And we have the red edges here where the object may have trouble coming out of the mold. So what we can do to fix this is go up to the modified drop down menu and then select draft . Now, using this draft tool, we can apply a new draft angle to the model. So to do this, I'll select the top of the mold as the plane and then the inside faces here that are red. And then I can simply drag the slider around until we get the minimum degree turns the analysis to Green. I can click OK, and I can repeat these steps for the key chain knockout by right clicking and selecting repeat draft. And again I'll select the top as the plane and the side faces and then make this five degrees and click. OK, now it's kind of hard to see the draft angle here. So if I look at the section analysis from the side, you'll see that we did end up creating this nice draft angle, which will ensure that our object or replica will be able to pop out of mold without being damaged. And one other thing will point out. When you turn on the draft analysis, you will see it adds the analysis folder to the browser, where you can toggle it on and off once again. If you are going to three d print simple one part moulds to cast resin parts in order to make replicas faster than three D printing the object again and again, Then please support my channel by clicking my links below to my favorite resin and mold making products. I'll also point out that some parts of your model may pop out fine if the analysis is showing that they're red. It really depends on the materials that you're working with, how thick the object is and whether or not you spray on or apply a mold release. If you don't have any mold release handy than you can, try using the spray Pam from your kitchen, or you can pick some up from your local grocery store.