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This course introduces you to the interface and key processes of Inventor, the parametric design system from Autodesk. Author John Helfen covers sketching, part modeling, assemblies, and drawings. These tasks work in conjunction, allowing you to create parts and assemblies and document them in a way so that the manufacturing process proceeds faster and more efficiently.
At this point, we've nearly completed our Assembly. The last step in the process is to align the faceplate to the engine block properly. We're going to do that with the Insert constraint. If we right-click in the Graphics window, we can bring up the Constraint dialog box from the marking menu. Now up to this point we've used the Make constraint, and in the Type section of the dialog box we want to switch to an Insert constraint. Now an Insert constraint is essentially a shortcut to creating two Make constraints. Let me show you what I mean. We're going to make our first selection on the faceplate. We want to align this hole with the hole on the engine block.
What you'll notice is if I hover over this hole, two items are highlighting, the edge of the hole, and the access through the hole. I am going to go ahead and make this selection by left-clicking, and we'll rotate to find the corresponding hole on the engine block. The hole we selected on the faceplate should align with this hole on the engine block. By selecting that edge of that hole, you can see from the preview that the holes are now aligned. Not only are the holes are aligned, but the two faces are also touching. If I click OK to accept this, the dialog box closes, and we can test our function by left-clicking and dragging the faceplate.
You'll notice we're rotating around the axis of the hole, and if we rotate a little bit further up you can see that the faces are actually touching as well. So essentially we've created two Make constraints in one action by using the Insert constraint. The final stuff here is to add one more constraint to align one more hole on the faceplate to one more hole on the engine block. We're going to do that by right-clicking in the Graphics window and bringing up our Constraint dialog box from the marking menu. This time, rather than using the Insert constraint, we're going to use one more Make constraint.
We're going to select the access through the hole on the engine block and the access through the hole on the faceplate. By doing so, you can see that the preview is showing that the parts are properly aligned, and we can click OK to accept this and close our dialog box. We're going to click on the Home button to return to our default Isometric view, and now we can begin to test the motion of this part. If I left-click and drag on the crankshaft, you'll notice that the piston is moving up and down in the piston shaft. The problem is that you can't actually see that very well. One of the nice things about the Assembly environment is the ability to turn the visibility of parts off, but also to enable and disable parts, and they provide slightly different functionalities.
Turning off the Visibility simply removes the part from the Graphics window, but disabling the part offers something else. If we right-click on a part in the graphics window and uncheck Enabled, you'll see that the part has become clearer or ghosted, and in the browser the icon has changed to a green color to indicate that the part has been disabled. What this means is that I can't select the part in the Graphics window, but we can still see a ghosted image of it so that we can understand the context of the assembly. We're going to also do this with the piston shaft by right-clicking on the part and un-checking Enabled.
And we now have a pretty clear view of the parts inside the model, but we also have a view of the context in which those parts exist. If we left-click and drag on a crankshaft now you can actually see the motion of the piston in the piston shaft even inside the engine block. The beauty of this is we're actually able to test the function of our parts before we actually manufacture anything. This allows us to find design mistakes before we spend any time or money manufacturing any of these parts.
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