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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 movie we learned how to create a sweep from scratch, from a blank file. In this video we're going to look at how to use the sweep within the context of a part file. On the screen you can see a basic oil pan shape that I created and we're going to just use this model as a way to create a sweep that follows along the lip of this oil pan. I've created a work plane here, Work Plane1, that runs right through the center of the part. And I'm going to use that plane as my sketch plane and what we're going to do is create a little lip that we can sweep all the way around this edge.
To begin, I'll select the work plane and use the heads-up display to create a sketch. We've rotated into the normal view for the sketch, and you can see we have geometry in our way. If you remember from some of the previous videos, we can right-click in the graphics window and select Slice Graphics to help make this more visible. F7 on your keyboard will also do the same. What this does is temporarily slices the graphics away so that I can see down to the sketch, and I can use my option for Project Cut Geometry from the toolbar to project the edges that touch this work plane.
And the reason for that is, I'm going to zoom in right up here. On the edge of the lip of this pan. And I'm going to use these reference lines as a way to start my profile. I'm going to right-click and select Two Point Rectangle. And I'm going to start my first corner of my rectangle at the intersection of these two lines. As I drag my cursor, you can see my heads-up display allows me to enter a value. I'm going to enter 0.75, hit Tab. And for the height of this lip, I'm going to go ahead and set it to 0.125.
By hitting Enter on the keyboard, I create that geometry and the dimensions that go along with it. If I finish this sketch, and we zoom back out, you can see that we've created this profile, let me zoom in a little bit. And it's sitting right on the edge of this lip. And we can use that to create a sweep that runs around this edge of the part. And what's really important here is if you haven't noticed, this is actually a 3D sweep. It actually changes, both in the x and y, and the z direction, along the entire path around the outside of this pan.
So if I go to the Sweep command in the Create panel, and bring the dialog box up. You can see that I have the ability to select a profile. If we zoom in. We have two different profiles to select, the one that was created when we projected the cut edges, and the one we drew manually. And we're going to select that as our profile. You'll notice that the Profile button turned white, which indicates Inventor has what it needs to continue from that standpoint. And it's moved us into the Path option and it's red which means that we still need to select a path, on which to sweep this profile around.
What I'm going to do is select this outer edge and you can see by selecting that I have the option to see a preview and if we look at it from the side, you can see that it's adding the geometry to the loop all the way around the entire shape. Now, in the previous video we were creating a base feature from scratch so we didn't have the ability to look at some of these features. So I want to circle back and call out these options. In the previous movie we only had the option for new solid. In this case, we have the ability to join material which is what we're doing now.
Cut material which will remove material, but in this case the way we drew the profile, cut doesn't make sense and neither does an intersect. But intersect would essentially sweep this along the path and leave whatever geometry was intersected with, the path that we created. We're going to go ahead and leave it at a join and when I hit OK, we create our sweep, and if I turn on my model edges by selecting Shaded with edges from the navigation bar. If you don't have this visual styles button you can click the triangle at the bottom corner and select Visual Styles to make sure it is enabled.
But you can now see a little more clearly that we have a lip that runs all the way around this edge. And it follows this 3D path as well. If you look over on this side, you can kind of see it a little more clearly where the lip actually follows that contour.
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