Join John Helfen for an in-depth discussion in this video Hollowing parts with the shell feature, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now ready to look at the Shell feature. The Shell feature allows you to hollow out a Part, higher Shape. To do that, we need to create some geometry we can work with, and on the screen, you can see I have a blank file. I'm going to right-click and select New Sketch. I'm going to select the XY plane to sketch on, and create a rectangle. I'm going to right-click and select Two-point Rectangle, then we'll hover over the center point of the sketch and drag out a rectangle. Now, the size doesn't really matter, so I'm going to leave the dimensions off and simply left-click to create the rectangle.
Next, we'll finish the sketch, right-click in the Graphics window, and select Extrude. We'll accept the value that's entered, and click the green checkmark. We now have a model we can start with, but let's go ahead and fillet this edge here at the top. I'm going to left-click on that and use the Heads-Up Display to select Create Fillet, and then I'm going to drag this so it's a little bit larger, and select the green checkmark. Now we have some geometry we can work with. To create a Shell, you need to go to the 3D Model tab and find the Modify panel.
You can see the Shell command here in the Ribbon Bar. Now, by selecting the Shell command, you can see in the Graphics window that a preview has been presented inside the model. Essentially, what Inventor has done is remove the inside of this model, so that there's a uniform .1-inch-wall thickness, all the way around. If we look at it from the front view, you can clearly see this. There's an even distance all the way around the model. Now, it's pretty unusual that you would hollow out a model and simply leave it.
Instead, in most cases, you're going to need to select a Face to remove from the model. If we hover over the top face on this model and left-click, you can see the results. Now, we only selected one face, but the entire top face, the fillet edge, and the front of the model were all selected at the same time, and that's because we have Automatic Face Chain turned on. I'm going to go ahead and select OK, and you can see the result of that model, and then we can edit that model by double-clicking the shell feature and make some minor changes.
Let's go ahead and select the Face selection mode, now hold Shift down on our keyboard, and select where the top of the model would be. That will remove the face from selection, and we can look at what would happen if we were to uncheck the Automatic Face Chain. Now, when we hover over the top, or the fillet, or the front, they can each be selected individually. The result is roughly the same, we can still continue adding these faces, but if you know that you're going to add them all at once, the Automatic Face Chaining is something that you probably want to leave on.
Now, just below that in the dialog box are some other additional options. We're not going to cover these in detail, because they're really beyond an essentials course, but what they do is allow you, in more complex models, to make compromises in the wall thickness. In certain complex shapes, you may find that the Shell feature can't actually create the uniform wall thickness, and if you have a failure in a more complex model, then I would start looking at some of these settings, because they may allow you to create the Shell when you previously weren't able to.
If we select OK, you can see the final result of our Shell. Now, you might be thinking, this is pretty simple. I could have done this without the Shell command. And that's completely true, in this shape. You could have created that shape with the fillet, sketched on the side, and extruded in to that model. Where the Shell becomes more powerful is when you look at a shape like this Bottle.ipt file. This can be found in the Exercise Files. It's actually a model we created earlier in the course. What we're going to do is take a look at how the Shell feature can be used on a more complex shape.
Let's go ahead and launch the Shell command here in the Modify panel, and let's select the top face of the bottle. That'll remove it. We'll select the checkmark, and the shell is created. If we look at this from the front, though, this doesn't look exactly like a shampoo bottle, because normally a shampoo bottle might be curved on the bottom. Let's go ahead and do that, and take a look at how it affects the shell. I'm going to select this bottom edge, select Fillet, and I'm going to look at it from the front view so that we can see what the curvature looks like, and that looks pretty good, so I'm going to go ahead and select the green checkmark, and now you can see we have a .3125 fillet here on the bottom.
Let's go ahead and change the visual style. If you don't have this button on the bottom of your navigation bar, you can select the little arrow down at the bottom right hand corner, and select Visual Style. I'm going to select Shaded With Hidden Edges, and the reason for that is, I'm going to zoom in on this corner, and you'll see that the outer edge of the bottle is curved, but the inside is not, and that's as expected, because when we created the fillet, the shell already existed. It simply took the one edge we selected and made the curvature.
Now, to fix this, we really want to have this inside edge curved as well. We could delete the shell, let the fillet move back up to the loft, and then recreate the shell. But because Inventor is a history-based modeling system, we can make this a little easier. If we left-click on this fillet and drag it up in the tree, and then release the mouse button when it's just below the loft, Inventor will recalculate the features, and now it has the loft, the fillet was created first, and then the shell was created.
So, without having to delete and recreate things, you can reorder them in the Browser to make changes a little more efficiently.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers