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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 on creating work planes, work axis, and work points, we used a part very similar to this. The one difference is that we had an angled cut that started at this intersection and ran across the face of this part. We're going to work through creating that cut in order to talk a little bit about projecting geometry. Within a sketch, projecting geometry can be incredibly helpful. As a matter of fact, Inventor Bug does it by default, right out of the box. I'm going to start by creating a 2D sketch by clicking Create 2D sketch from the toolbar, and I'm going to select this top face.
Inventor rotates us into a normal view. And you can see that it's projected some edges automatically, as I mentioned. It's projected all the edges that are touching this sketch plain by default. You can turn this option off, but I find it very useful, and I find that most people leave it on. What you'll notice is that it did not project these edges that are on an angle. And that's what we're going to do here. In order to create this angled slice, we could go back to our top view, right click and select Create Line, and we could begin drawing the shape we want to cut.
We could start at the intersection point; we could draw a line over here. We could draw a line down to the bottom pulling it and connect it back to its start point. Now, what you'll find is if we zoom in here, that's not very accurate. You can see that this line doesn't match up with this line exactly, and we could go through adding constraints to make these colinear. I could, for example, dimension this line, but in order to place this dimension, I need to actually go and measure the distance between these two lines. But there's a much easier way to do it with projected geometry.
I'm going to right-click and Undo several times to back out and get back to prior to creating those lines. This time, instead of going into the Line tool, I'm going to use the Projected Geometry functionality. Which is found in the Sketch tab under the Draw panel. And what it allows me to do is select individual pieces of geometry that I can project to this sketch and use to create my shape. I could select individual lines or if I cancel out of that and Undo, I can also select Project Geometry and select the entire face.
What that's done is just taken all the edges around that face and projected them, so that if I look at it from a top view, they line up perfectly with the lines and geometry below. Now, if I right-click and select the Line command, I can be very accurate about the fact that I know that this line is directly from the line below it. And when I left-click to place that geometry, I know that the end point is exactly on that line. The next thing I can do is right click and select General Dimension.
To define the exact angle at which that line resides. I'm going to select 40 on my keyboard and click the green checkbox, and you can see now that the line is purple indicating that it's fully constrained, and I can always come back to this and change this angle. If I finish this sketch, we rotate back to an isometric. And I can now right-click in the graphics window, select Extrude, and I have the ability to extrude this feature. I'm going to change the termination to through all, and instead of joining the material, I'll cut material.
And you can now see if we select the green checkbar, that we have an extrusion in the browser, the sketch we created is consumed, and we can always go back and edit that by double clicking it. I can, for example, change this to 30, hit enter, or click the green checkbox, and when I finish that sketch, the model will be updated to reflect that change. That explains how to project a geometry by default. The other option I want to look at is projecting cut edges. This is another one you'll use from time to time that can come in quite handy.
In order to show this, I need to create a new work plane. And I'm going to make on that is parallel to this plane. And it runs through the midpoint of this line. What I've essentially done is generated a work plane that cuts right through the middle of this part. And we're going to go ahead and begin by selecting that work plane and creating a new sketch on it. What you'll see is that I'm rotated into the view so that I'm looking normal on the sketch, but I have all this geometry in my way. If you look here, you can see all this geometry out in front of the work plane is blocking the view that I need to create this sketch.
What I can do is I can right click in the graphics window and find Slice Graphics. It's also F7 on your keyboard. And, when I toggle this, you'll see that all the geometry is removed and remember, F7 on your keyboard is the toggle for this. So, if I press F7 on my keyboard, the material comes back. It's simply a toggle, so that you can quickly slice away graphics and see what you're working on. The other thing that's important here, and what I really want to show, is how to project these cut edges. Because this sketch was created, and it didn't touch any other edges, like these outer edges; nothing was projected to the sketch.
But again, projecting those cut edges would be very helpful in controlling some of the geometry I'm going to create. So I'm going to use the drop down menu under Project Geometry, and I'm going to select Cut Edges. And when I do that, you can see Inventor automatically runs around the edge of the part and finds the lines that intersect this work plane and projects them to the sketch. And the reason I do that is I can now create a new line. And I can use these reference edges to, for example, draw a line from the midpoint of this line that's perpendicular to the line on the top.
You can see by doing that, I'm using those very specific points that I selected, the midpoint here and the perpendicularity, which was automatically added by Inventor when I got this line to a perpendicular point. And I now have those two points controlling this entire sketch. If I finish the sketch, you can see that my geometry comes back, and I do have a sketch that's ready to be used in a 3D modeling action. If I right click and select Extrude, I can select these profiles through the part.
And I have the ability to now make, for example, a slot in this part. Rather than extrude in one direction, I'm going to extrude in a symmetric fashion. And instead of joining material, I'm going to cut material. Now I can use my Heads-up display to adjust the length of this extrusion. And you can see I've created a slot directly on the midplane of what used to be this long line here. And it's not important that you understand how I did this. We'll cover this when we get into creating features.
You can see here that I can create work geometry that cuts through a part and then use Project Geometry to get very specific reference lines that I can use to create more advanced features.
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