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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.
To create the final hole, we'll begin the same way we did in the previous holes, by right-clicking and selecting Hole from the Marking menu. Rather than using the Linear Placement option that has defaulted in the dialog box, we're going to return to our Concentric option. It automatically jumps forward and asks us what Plane we want to place the hole on, and I'll select the top of this boss. Now you notice it has picked up the previous diameter so that when I'm asked to select the Concentric reference I can't select the top of this hole or the face of this boss. Typically we would just simply change the diameter to a smaller size so that it fits on that face, but in this case we're using a threaded hole.
So what I am going to do is move to the bottom of the dialog box where we can define what type of hole is being created. By default, it starts with a Simple Hole, you also have the option for Clearance Holes, Tapped Holes, or Tapered Tapped Holes. For this design we need to create a Tapped Hole. By selecting this option an entirely new section of the dialog box has been enabled. Below you can see Threads, these are the Threads listed in the engineering handbook so that you don't have to look this up. We know that the size of the hole that we're creating is going to be drilled with a number eight drill type.
By selecting that the Designation for the Threads automatically changes to 8-32 UNC which is appropriate for our design. We also have other options, but because the default is what we need, we'll leave it as it is. Now that we've set this option you'll notice that we have the ability to select that Concentric Reference. But because we had to move to this section, we do have to tell the dialog box we're ready to make that selection. You'll notice that the plane has already been selected, and because that's the case the icon has changed to a white.
Anything red in the dialog box indicates that there is input required still, so by clicking on the Concentric Reference icon I am telling the system I'm ready to make that selection. I can then hover over the cylindrical face or edge to walk that hole into position. Now we are almost ready to continue. The one remaining component that we haven't talked about was the type of termination. As I mentioned when we were starting this hole, this hole does not go all the way through the part. But if we rotate a bit you can see from the preview that in its current state it's expected to run all the way through the part.
The way we can fix this is through the Termination options. We've used Distance already, we know this isn't a Through All hole, and we're going to use the To option. What this allows me to do is select a specific face that I want that hole to terminate on. By selecting that face, you'll notice that this hole does not continue all the way through the part, and we can click OK to apply these settings. If we rotate back to a Home view and zoom in a bit you can actually see this hole has thread representations built-in to indicate that it is a threaded hole.
As we rotate around you can see that the hole extends through to the first face, but it does not continue through the entire part. At this point you've seen a few different ways to create holes and should have a solid foundation of how to create them and why the dialog box adds so much intelligence when creating holes.
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