Create the flywheel - SOLIDWORKS Tutorial

- [Instructor] Building a detailed assembly in SolidWorks, can sometimes seem like quite a daunting task, but like lots of things in life, it becomes much easier if you break it down into smaller, manageable chunks. And that's what we're going to do with our Sterling engine assembly. First, we're going to make some simple parts, and then later on, we're going to create an assembly and add those parts. And then we'll just continue that same kind of process, creating the next set of parts for the next section of the engine and then adding those. And so on until we have a complete model. The first part that we're going to make is the flywheel. And this is the part of the engine that actually spins round and gives an output. So I thought we'd start with the most useful part. There is an exercise file for this video. It's called 02_01_create the flywheel. And this is exactly the same as the part that we're going to create now. So you don't actually need this part. It's just an example of the finished part. So if you do get stuck, you can open this and hopefully see where you went wrong. We'll start off fairly slowly with this part, and then we'll increase the pace a little as we get through the course. So let's get started with our flywheel. Open up SolidWorks, and the part itself is quite simple. It's basically just a solid metal wheel with some cuts in the wheel to make spokes. First we're just going to make the overall shape using a revolved boss base feature. So start a new part. Unlike most features in SolidWorks, the revolved wast base starts with a sketch. Let's go over here to the design tree on the left, and select the front plane. And then from the menu that pops up, choose sketch. So now we're sketching on the front plane. And we can see we've got this sketch icon in the top right corner, which indicates we're editing the sketch. The revolve feature works by taking a close profile and revolving it around a center line or an access. So firstly, we're going to draw that center line. Go up to the line tool, which is on the sketch tab and click on the dropdown next to it. And then select a center line. Now go into the graphics area and we want to draw a horizontal center line out from the origin. And the origin is this fixed point in your model. So you can left click to start there, then draw out to the side and make sure you get this horizontal icon. And then left click to end the line segment. And then you can double left click to stop placing new line segments. Now let's also draw a vertical center line, starting from the origin again, go vertically up, make it nice and long, something like this. And then you can press escape to close the line tool. So now we should just have these two center lines, one vertical and one horizontal. Now we're going to draw our revolve profile. So select the line tool again, but this time don't choose the dropdown, just choose the main tool. So we're going to be drawing solid lines. We want to draw something like this. Don't worry about the exact spacing for now because we'll add the dimensions in a moment. So first left click on the vertical center line somewhere above the origin, draw a line out to the left, and then one up, and then into the right, and then another one up, left again, up again, and then back into the center line. And then press escape to close the line tool. So this is going to be half of our revolve profile, but to make the revolve profile, we need a closed profile. So we're going to mirror these lines over to the other side. To do this, from the sketch tab, choose mirror entities. And then in this entities to mirror box, just drag a box around all of those solid lines. So you can see all of those lines have now gone into that box. Then click on the mirror about box, and now choose that vertical center line. So you should be able to see this yellow preview. So we're going to mirror all of these lines over to this side. And if that looks good, press okay. So now we've got our closed profile and we're going to spin this around this center line. But firstly, down here we can see that our sketch is under-defined. And if we grab these lines and try to move them around, they're not fixed in space. It's really important in SolidWorks to try to always fully define your sketches. Otherwise it can cause you problems later on. So select the smart dimension tool from the sketch tab, and let's add some dimensions. Firstly, let's make the whole wheel eight millimeters wide. And when you add the first dimension, if it's miles out like mine is, it should automatically resize when you add the first dimension. So I've just typed in eight millimeters. And if you're working in inches, you can also just type 8mm and it should automatically convert that into inches for you. So press okay. And now the whole sketch is resized to that eight millimeters. And that only works with the first I mentioned that you add. So next let's add the overall diameter. So click this top line and then click the center line. And you can see if we keep the dimension up here, above that center line. It's 14, if we bring it down here, it actually doubles. So that's actually showing you the full diameter. Up here is the radius, down here is the full diameter. So let's set the diameter and let's make it 80 millimeters. And you might have to zoom out and then let's just add some more dimensions. So let's make this one 5.5, make sure you pick up the diameter again, say 5.5 millimeters. Let's make this one 20, and then let's make this one 70. And then finally let's just make this part four millimeters thick. So that should be all the dimensions that you need, but you can see on my sketch that it still says it's under-defined and these lines are blue, which indicates they're under-defined. So if we grab that, we can still move it around. So you could just add another eight millimeters between there, but we can also just select this top line, which is fully defined already because it's black in color, and then hold down control and then select that bottom line as well. And then we can add a colinear relation. And that just means that those two lines are now always on the same line. So now we've got a fully defined sketch. We've got a closed profile so we can revolve this profile around our center line. So from within your sketch, go to the features tab, and then choose revolved boss base here. We'll get some options here on the left, make sure you're in this first box, the axis of revolution. And then you might need to zoom in a bit, and just choose your horizontal center line. And you should get a yellow preview like this. If you don't get the preview, just make sure that you've got these solid lines all the way around the outside, and also make sure your two sensor lines aren't solid. So if they do look solid, you can go back into your sketch, select those lines and just click make for construction. If your preview looks good, press okay. And now we've added that revolve feature. And we can see the revolve feature is here in the design tree. We'll develop this part a bit further in the next video, but for now you can just press Control + S to save your part and let's call it something like flywheel. I'd recommend that you name your parts, something different to the example parts just to avoid SolidWorks getting confused with the file names. So press okay to save and well done. We've now taken the first step. From here on, it's just a case of building upon these foundations.