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Already up and running? This course is the next step in building your Autodesk Inventor skillset. Author John Helfen takes you through the interface and key processes of this parametric design system, including sketching, part modeling, assemblies, and drawings. Each process works in conjunction with the rest, allowing you to create parts and assemblies and document them in a way that they can be manufactured. Learn how to set up your project file; create and modify geometry; create extrusions, sweeps, and lofts; build parts with placed features and patterns of features; and create iParts and iFeatures. John also covers assembly visualization techniques, drawing views, and balloons and parts lists.
The course was created and produced by John Helfen. We're honored to host this training in our library.
In the previous video, we covered how to create a base extrusion, and we looked at the through-all and distance termination types, along with some of the other settings. In this video, I want to focus on an additional termination type. I'm going to go ahead and create a new 2D sketch by selecting this interface of the model, and using the Heads-up display to create a new sketch. We rotate into viewing the sketch, but you'll notice the graphics are in the way. If you right-click the graphics window, there is an option to select Slice Graphics, which is F7 on your keyboard.
What that'll do is temporarily slice the graphics away so you can clearly see the sketch you're working with. I can then right-click and select Center Point Circle. And I'll locate this in the center of this part near the top, and I'll set the diameter of the circle to .25. Hitting enter on my keyboard will create that shape and I can then right-click and select General Dimension to finish adding dimensions to this. I'll dimension it at .75 from the edge, and I'll dimension it to .25 from the top of the part.
I can finish the sketch, and you can see that the sliced geometry is returned, and my sketch is ready to be extruded. If I right-click in the graphics window and select Extrude, I am placed in the profile option, because I now have two different profiles that I can take action on. I'm going to select this cylinder. And you'll notice that by default, it extrudes to a distance of one inch. Now, I could rotate to a front view and use the Heads-up display arrow to drag this out so that it's far enough where, I know it's inside this part.
If I hit the green check mark, again, it looks as if this model is accomplishing what I need it to. This cylinder is extruding from this face all the way to the other side of the part. The problem is, is that if we were to return to Extrusion1 and double-click on its Sketch, and change this from 2 to maybe 2.5. And then hit Finish Sketch to update the model. What you'll notice is this cylinder no longer reaches the other half of this part. And that's why I wanted to talk about another type of termination.
When you're doing these designs, it's up to you as the designer to build in your design intent or the intelligence into the model, so that as the model changes, you're not having to update every single feature in the model. The way we can fix this one is by double-clicking on Extrusion3 in the browser to bring up the original dialogue box again and make changes as if we're recreating this from the very start. So rather than setting it to a distance of 1.625, we can select the termination drop down and select to neck, face or body.
And what that will do, is ensure that no matter how this part changes, this cylinder will extrude from this face to this other face, by clicking the green check mark, you'll see that the model is updated. And, if we go back and change this over all sketch on Extrusion1 back to two inches, you'll see that the model updates appropriately, and the cylinder doesn't poke through the outside of the part. More importantly is this face on the inside of the channels is actually defined by Extrusion2.
And if we were to go back and double-click on the Sketch2, for Extrusion2, we can get back into this original sketch, and we can make the modification to the dimensions. I'll enter .125, and hit enter on my keyboard, and you can see now that these faces are further away from each other than they were previously. But, if we finish this sketch, you'll see that the model updates accordingly and because we selected to the next face, this cylinder is automatically updated because this face moved back and that's where the original sketch was created.
But even though this one moves back as well, the termination type of two necks automatically updated the model to maintain our design intent, which was for this cylinder run between both edges or between both face.
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