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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.
The next feature we're going to look at is the Hole feature. Inventor has two different types of features. Sketch features, like the Extrude and Revolve, and Placed features, like the Fillet and Chamfer. The Hole feature actually falls in the middle because you can use either method to create holes. This part requires four holes to be added. The first one is a flat bottom hole, the next two run completely through the part, and the final one is a threaded hole. While creating the holes I'll use both the Placed method and the Sketched method so that you can see how each work. They both create identical geometry so it's up to you as the designer to determine which you prefer.
The first hole we're going to create is on the back of the part, and it's concentric to one of the earlier extrudes we created. To create the hole we're going to use the marking menu by right-clicking in the graphics area and selecting the Hole command. Within the Hole dialog box there is a bunch of different options that let you build intelligence into the hole. In a lot of cases if you were simply going to create a through hole you could draw a circle and extrude simply cutting material away, but you'll lose some of the intelligence. This becomes more important as we get to things like threaded holes, but even on this first hole we have an option that simply extruding wouldn't allow us to do.
We can choose the type of endpoint, perhaps we're going to use a drill, perhaps we're going to have a flat bottom hole. The Hole dialog actually allows you to determine which you're going to use and build that into the Hole geometry. Within the dialog box there is a Placement option, within that dropdown list you have a few different options, From Sketch, Linear, Concentric, and On Point. In this case, we're going to create a concentric hole. By selecting the Concentric option some of the dialog changes because the type of input required for this hole also changes.
Inventor tries to walk you through the dialog box as you go. After we've picked Concentric it automatically highlighted the Plane option because it wants to know what plane you want to place the hole on. If we hover over the face on the model and left-click you can see a preview of the hole is created, but at this point it's not concentric. In the dialog box you'll notice that Inventor already moved us to the Concentric Reference. It's now asking what face or what circle we'd like our hole to be concentric to. By selecting the circular edge on that face the system aligns the center points, and you can see that this hole is now perfectly aligned to go through this part.
The hole however is not required to go all the way through. Within the dialog box we have different types of termination. This hole isn't a Through All hole, it actually has a distance. Within the Termination dropdown you can choose Distance, Through All, or to a specific face. Here we're going to select a specific distance, and by doing so we're enabling other features within the dialog. By selecting a specific distance the Drill Point options have become enabled. We're going to go ahead and select the Flat drill point and then we can turn our attention to the depth and to the diameter.
This hole is required to be 0.417 in diameter and only go to a distance of 0.663. As we update the dialog box, you'll notice the preview on the screen is also being updated. If we orbit you can see that preview, the red indicates that we're cutting material away. At this point the hole looks correct, and we are ready to accept these entries. We can either hit OK in the dialog box or click the OK button in the heads-up display to accept this entry and create our first hole. You can see that the hole has been placed in the browser at the bottom of the tree.
The next hole we'll be creating is on the top of the part and is a Through All hole. Again, from the marking menu we can right-click and select Hole. I'm going to go ahead and create this hole as a concentric hole. So from the Placement menu I'm going to select Concentric option, and Inventor automatically jumps and asks what plane I'd like to place my hole on. I'm going to go ahead and select a face on the top of the part. It now wants to know what edge or what cylindrical face to become concentric to. I'm going to go ahead and select the cylindrical face around the top of the boss, and I'm going to set the diameter to 0.375.
By doing so the preview shows that the whole fits within the face that it's been placed on, but you'll also notice that it remembers the previous settings we had, including a flat bottom drill point and a termination to a specific distance. As I mentioned this was a Through All hole, so rather than terminating a specific distance I'm going to select the Through All option. By doing so you can see the preview update and the hole extends completely through the part, because this appears the way we wanted to we can simply click OK in the dialog box to accept that entry, and if we orbit, you'll notice that the hole goes completely through the part, intersecting the previous hole that we created.
This is exactly what we want, so we're ready to continue to our next hole. As I mentioned earlier in the movie there are two different ways to place holes, using the Placed method which we've used on the first two holes and through a sketch which we have not done. Since the last hole was a Through All hole and the next hole we're creating as a Through All hole, I'll use this opportunity to use the Sketch method for this hole. To begin we start just like we were creating an extrusion. We'll right-click and select New Sketch, pick the face we want to sketch on, and the edges from that face are projected to the sketch.
Because it's a cylindrical face, and we know we want it centered we have a perfect center point to start from. All we need to do now is finish this sketch and launch the Hole command. From the Marking menu select Hole, and you'll notice that our Placement option in the dialog box has changed. Because there was an unconsumed sketch at the bottom of the tree the system automatically defaulted to use that sketch. If we wanted to we could change that option, say for example, back to Concentric, but in this case we do want to leverage that sketch. The system automatically asks what center points we want to use, and we can simply click the center point of the projected circle to create our hole.
Last, we need to set the diameter for this. It remembers the previous diameter, but in this case we wanted to check 0.268 as our size for this hole. It's set to be a Through All hole so we're ready, and we can click OK to accept these settings. If we rotate around a bit you can see that this part goes all the way through, punching a hole in the bottom of our flat bottom hole that we initially created. This is exactly what we expected and what we need for this design, so we can return to our Home view and prepare for our final hole.
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