3D Modeling & CAD for Motorsport: Revolves
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Revolves
06.58
| 00:00 | - The tools we've used up to this point generally rely on datum planes and sketches to generate our features. |
| 00:06 | The revolves we'll be discussing in this module also require sketches on plane or planar surfaces but they also need datum axes too. |
| 00:15 | As the name implies, this is the method of revolving a profile about an axis to make a 3D solid. |
| 00:22 | Just like we saw with extrudes, revolves can also be used to remove material and create a revolved cut. |
| 00:29 | If you're familiar with the use of lathe machines then you can imagine that this would be a suitable manufacturing method for a CAD model that's created exclusively using revolve features. |
| 00:39 | With that said, the revolve tool can also be really useful for particular models where the use of a lathe isn't the intended manufacturing method, like o rings, suspension bushings or even springs. |
| 00:52 | Like the extrude tool, the revolve tool will require us to create the sketch profile prior to using it and we also need to understand where the axis used for the revolve will be before we make the sketch. |
| 01:04 | The position of this axis is generally going to be pre defined, however the actual sketch profile that we're revolving around this axis may take some thought. |
| 01:13 | Think about modelling a wheel spacer, just the base part without any of the holes for the wheel studs. |
| 01:20 | The revolve axis runs straight down the middle of the part and if there was a plane running through the axis, it would be symmetrical through this plane. |
| 01:28 | Imagine cutting that part down the plane. |
| 01:31 | The cut face of the part is what becomes our sketch profile, meaning that we only need to sketch one side. |
| 01:37 | It's important that our sketch profile forms a closed loop, while sketching we can make sure of this by having the show profile preference selected in the sketch palette here and the area inside the loop will be lightly shaded blue. |
| 01:51 | We also need to make sure the sketch doesn't cross the revolve axis or the feature won't generate. |
| 01:56 | OK so let's make a start at modelling the wheel space we've been looking at now, using the Y axis for the revolve. |
| 02:04 | The measurements will be coming from a physical sample that we have on hand. |
| 02:07 | We can sketch on the front or right plane, either will work fine. |
| 02:12 | Let's start by using a simple line drawing to make the profile and dimension it to fully define the sketch. |
| 02:20 | The base geometry of our spacer has an overall diameter of 136 mm and the distance between the mounting surfaces is 25 mm which is the distance our wheel would be spaced out. |
| 02:33 | Since we're only making a sketch of one side, our diameter measurements need to be halved to represent the radius. |
| 02:40 | There's a 73 mm diameter pocket underneath that's 22 mm deep. |
| 02:46 | We can make two vertical lines with the bases horizontal of the origin to represent these features of the spacer. |
| 02:53 | Then connect the bottom, which will be the face that mounts to the vehicle. |
| 02:57 | Next is the mounting face for the wheel which comes straight across horizontal from the top of the outer line until it meets the flange for the wheel centre bore. |
| 03:06 | The flange has an external diameter of 54 mm, extends up 10 mm and is 3 mm thick. |
| 03:14 | And it comes down to level with the top of the pocket feature. |
| 03:18 | Then we can connect the remaining points with a horizontal line to form our closed loop. |
| 03:23 | The corners of the sketch will become the edges of the resulting 3D body from the revolve operation. |
| 03:29 | As we know, sharp internal corners are stress concentrators and sharp external corners can be safety hazards from the user. |
| 03:37 | So let's quickly round the corners using the fillet tool. |
| 03:40 | The two outer corners of the mounting surfaces need to have a 1 mm radius and the others 0.5 mm to match our sample. |
| 03:49 | Finally a 3 mm equal distance chamfer which is just a short straight line to break the sharp corner at the bottom of the pocket. |
| 03:57 | It's important to make sure the show profile preference is selected here in the sketch palate as this allows us to check we've formed a closed loop and once that's done, we can finish our sketch. |
| 04:09 | Now it's time to select the revolve tool up here in the create toolbar. |
| 04:14 | Then we can select the profile and the axis as you can see here in the revolve tool pop up box. |
| 04:19 | For degrees of rotation we're going to want 360° to complete the part. |
| 04:25 | Only one side is needed for direction because it's a full 360° and in this case there are no existing bodies so we'll need to create a new body from the operation preference. |
| 04:37 | Click OK to execute and now we have our revolve feature, in this case, the basic structure of our wheel spacer which we'll add more features to in a coming module. |
| 04:47 | For this part, we could have used a series of circular extrudes to create the same model, as well as the fillet and chamfer modify tools that we'll be covering soon. |
| 04:57 | But rather than having only two features in our timeline, as you can see down here, we'd have at least six. |
| 05:04 | This isn't a major headache since it's such a simple part to model but you can imagine that for a part with significantly more elements there could be many more features in the timeline, equating to much more time spent modelling the part. |
| 05:18 | Now before we move on, you'll remember at the start of this module, we discussed that the revolve tool can also be used to remove material, not just add it. |
| 05:27 | So let's fire up a quick example of that now. |
| 05:31 | If we start by sketching a 100 x 100 mm square on the top plane, we can extrude this sketch upwards by 100 mm to make a cube for our base solid body. |
| 05:42 | Now let's sketch a circle of 50 mm diameter on the top face and then draw a line straight across the middle of this circle. |
| 05:49 | We can use the trim tool here to remove one side. |
| 05:53 | After finishing this sketch, next we use the revolve tool. |
| 05:57 | Here we can choose the half circle profile and for that axis we can actually just select the straight edge of the half circle. |
| 06:05 | Selecting the operation preference as cut, we'll cut half of a sphere into the top of our cube. |
| 06:11 | We can see that not only is the revolve tool handy for creating cuts in existing bodies, but it's also ideal for making spherical features from sketches of semi circles. |
| 06:23 | And that's really all there is to know about the revolve tool so let's summarise quickly. |
| 06:27 | This is a great tool for, but not limited to, parts intended to be made on a lathe. |
| 06:33 | This involves revolving a sketch profile about an axis and that means that we must first understand where that axis will lie and then create a sketch that forms a closed loop. |
| 06:43 | The tool gives us the ability to specify the angle of the revolve as well as the direction and operation and just like the extrude tool, we can also use it to remove material in a revolved cut. |
