Join John Helfen for an in-depth discussion in this video Create revolves, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now ready to begin exploring the revolve feature. Similar to the extrude feature, you're going to see that the revolve feature has a lot of the similar interface components as I mentioned in the previous movie, and some of the same concepts. That's why we spend a little more time in the extrude dialogs, so that you can understand the settings, because everything you learned in that movie is going to be reflected here in the revolve in some fashion. Let's go ahead and start with a new part. I have one open on the screen. If you don't have one go ahead and open one. And we'll begin by creating a new sketch by right clicking the graphics window and selecting New Sketch.
We'll then select the x y plane to sketch on, and we can begin. I'm going to go ahead and right click and select Two Point Rectangle and I'm going to hover near the centerpoint and left click to start my rectangle and then I'm going to use the heads up display to enter some values. I'm going to enter 0.5 for the first dimension, and I'm going to hit one for the second. Hitting enter on the keyboard will create that geometry, and we can finish this sketch. Go ahead and double click on the screen with your middle mouse button, that'll zoom all the geometry into the center of the screen. We can now create our revolve.
We're going to right click and select Revolve, and because there's only one profile, just like in the extrude, Inventor automatically selects it and it moves us to the next step in the process. And that is the ability to select an axis to revolve around. Each feature might have different inputs that you need to select to create the feature, but the process is generally going to be the same. I'm going to go ahead and select the vertical edge on the left, and when I left click on it, you'll see that we create geometry and we get a cylinder standing on end.
Now if for some reason you made a mistake and you didn't want to select that line, and you wanted to select some different axis, you can always return to the axis selection mode by clicking on it in the heads up display, holding shift down on the keyboard and reselecting that same axis. What that does is deselects it, so that you're ready to select a different one. For example if we select this top, horizontal line, you'll see we also get a cylinder because we're creating a revolve of a rectangle, but in this case it's on its side, it's much larger, and it's skinny.
We're going to go ahead and one more time return to the axis selection mode, hold shift down, and deselect that top, horizontal line. And instead, return to the previous vertical line. With that selected, let's go ahead and click the green checkmark, that will create our geometry and we're ready to take our next step. Now, if we double click on this one more time to edit it. One thing I do want to call out is, just like extrude, because this was the very first feature, in this case it was a revolve instead of an extrude, we still run into the same thing that we ran into with extrude.
For example, because this is the base feature, the type of operation we can create is only New Solid. Join, Cut, and Intersect are not available until you've already created a base feature. I'm going to go ahead and cancel that. Let's go ahead and create another revolve. Let's go ahead and cut a ring around the outside of this that we might put an all ring or a c-clip in. To do that, we're going to go ahead and right click and select New Sketch. But because this is the second feature, we don't see the origin planes.
But, when we created the first feature, I know we used the center of the universe, so I know these origin planes are cut through the center of the part. If we expand the origin folder, you can hover over the y z plane, or the x y plane. Either of these would be perfectly acceptable because they cut through vertically through the cylinder. I'm going to go ahead and select the x y plane, and it's going to rotate us into a normal view to that sketch, and as you can see, some of the geometry from the cylinder is in the way.
Let's go ahead and right click and select Slice Graphics which is F7 on our keyboard, so that that geometry is cut away, and we can see the sketch more clearly. The next thing we're going to do is project some edges. I'm going to go ahead back to the Create Panel on the Sketch tab, and I'm going to select Project Cut Edges. If your view actually shows Project Geometry, simply select the bottom half of this button and you can see the project edges. By clicking on that, Inventor automatically projects all the outside edges to the sketch so that we can use them as reference.
The reason I did that, is we need to use this edge along the side to begin creating our groove that we're going to revolve through this. I'm going to right click and select Two Point Rectangle, and I'm going to use that vertical edge on the right and left click to start my rectangle. As I drag out, I get heads up display, and I'm going to enter 0.125 for the first value, hit tab, and hit 0.125 for the second value. Once I hit enter, the geometry's created and we just have one last dimension to create.
If we right click in the Graphics window, we can enter the General Dimension command. Select the top line in the rectangle, and then the top line on the model. Here we'll enter 0.125 as well. Hit enter on your keyboard, and we have everything we need to continue, so we're going to finish this sketch. By doing that, the geometry that was sliced away is returned and we're ready to create our revolve. You can see here we have a Sketch2 in the browser that's ready to have a modeling action applied to it. If you right click on the Graphics window and select Revolve, this time we're in the profile selection command.
Previously, there was only one profile to select from, so Inventor automatically selected it and placed this in the access tool. Now, we could select the rectangle that was created when we projected the sliced edges, or we can select the smaller rectangle that is what we're going to cut with, and that's the one we want to select. Now, when we go to the axis mode, we have a small problem. We don't have an axis that runs through the center of this. Well, kind of. Technically we do, because when we created the first revolve, I know that we created this in the center of the universe, or right in the middle of the sketch, therefore I know that this y axis runs right through the middle of the part.
But instead of selecting that right now, let's go ahead and cancel this and the reason is, I'm going to go back to this sketch and double click it, and I'm going to hit F7 on our keyboard to slice the graphics away, and I want to show you one other option. In the case where you have created a cylinder or something that you're going to revolve around, and you haven't centered it in the center of the universe, where the origin or axes, or origin plane would help you, you can draw your own axis in the sketch. If I right click and select Create New Line, I can select the midpoint at the bottom, which ironically is the center of the sketch, and draw a line up to the midpoint at the top.
That gives us a line that we can revolve around. Now I could either leave it as a line, or I could right click and select Centerline. Either one is appropriate, it really doesn't make much difference, but it will affect what profiles are available. For example, let's go ahead and leave it as a regular, standard line, and finish the sketch. If we enter the revolve command by right clicking and selecting Revolve, we can now select from several different profiles. We can select the large rectangle, we can select the rectangles that are also created on either half of the line down the middle, or we can select the smaller rectangle.
I'm going to go ahead and cancel that. Return to editing the sketch by double clicking on it, and then hit F7 to slice the graphics. The other option we have would be to right click on this and select Centerline. If we finish the sketch now, and we enter the Revolve command one more time, this time we're going to select the small rectangle. You can see here in the selection, I selected more that I needed to, so I'm going to hold shift down, and deselect that larger rectangle, and we now have the profile we wanted selected.
Next, we can move to the axis selection point. In here, you can see that we can hover over the model, and we have the option to select that centerpoint or that centerline. I'm going to go ahead and click on that and we move into creating the rest of the geometry. Now similar to the extrude dialog, we have a lot of the same settings. Instead of a distance here, you can see that we have Full entered. If you click the button to the left and select the down arrow, you'll see that we have several different options for extends.
We can use full, which is the default, that'll make a full 360° revolution. The other one you may use quite a bit is the angle option. What this will do is set the revolve to a specific angle. Here you can see it's revolving from the sketch we were on 90° over, and we could go ahead and use the heads up display and drag that further around our model to a specific angle that we wish. If you're going to go a full 360, I would recommend going back to the full option. The other thing you'll notice is right now we're going to add material.
You can't see the cut that's going to take place because it's just joining material, so we'll change the operation, and if you remember when we were looking at the first revolve we didnt' have Join, Cut, or Intersect. We only had New Solid, because the base feature always has to be a new solid. Now that this is the second revolve, we could choose to join material, which is what we're at now, we could cut material, or we could intersect which will create the ring where the two solids intersect with one another. I'm going to go ahead and return to the Cut option because this will create essentially a groove where we could place that all ring or c-clip.
I'm going to go ahead and select OK and you can see our cut is made, and in the browser we have Revolution1 and Revolution2. Because these are sketched features, we could always return to one of those sketches, in this case I double clicked on Sketch2. I'm going to hit F7 in the keyboard to slice the graphics, and here we could go back and choose to make this groove a little bit deeper, for example. If we double click on this 0.125, we can edit that and let's go ahead and make it 0.25. You'll see the geometry in the sketch updates and then when we finish this sketch you can see that the geometry in the model updates to reflect that change.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers