From the course: Inventor 2016 Essential Training

Projecting geometry - Inventor Tutorial

From the course: Inventor 2016 Essential Training

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Projecting geometry

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- We're now ready to look at how we can project edges. And project edges is one of those features that kind of falls in between sketching and part modelling. You're really gonna be projecting sketch geometry, but most often, you'll be projecting that geometry from part edges. So on the screen you have a part very similar to what we used when creating work planes, work axis and work points. The difference is, we previously had a slice that ran across the front of this face. And that's what we're gonna create here, so that we can look at projecting. I'm gonna start by creating a sketch. I'm gonna right click, select New Sketch, and I'll select this top face. By doing that, a new sketch is created. However, we haven't projected any of these edges that sit on that sketch plane. You can see here, if we rotate on an an angle, these edges all sit flush on this work plane, or this sketch. There is an option in Inventor which I've mentioned previously in the course, and I wanna mention again. It used to be a default in Inventor, and I still find it useful, but I leave it off for training purposes just so that I can explain this to people. If we go to the application menu in the upper left and left click, we have Options down at the bottom. These are the Application Options. Now if you look, you should be on the General tab most likely. But, what we wanna do is left click on the Sketch tab. And within the Sketch application options, there's this option right here, Autoproject edges for sketch creation and edit. If this is checked, and I'm not gonna check it, I'm gonna leave it off, but I want to explain what it does. If this is checked, when we were creating this sketch on this face, these lines around the top face of this would all be projected to this sketch as yellow reference lines. It's up to you to determine whether that setting is right for you in your world. But, you don't have to turn it on to accomplish the same steps. I'm gonna go ahead and use the Project Geometry option to manually project those edges. The project geometry command can be found on the Sketch tab under the Create panel here on the ribbon bar. I'm gonna left click on the Project Geometry command and hover over the face we just selected. By left clicking, you'll see that each of those edges is now projected into the sketch, and if we look at it from a home view, you can see that they are all flush and parallel with the sketch we just created. If we return to a top view, and we wanted to start creating the geometry that creates the slice, we can do that right now. We can right click and select line, and we can use the intersection point at the corner of those lines to begin our line. Now what we can do is we can look at a couple of different things that we have available to us. We could simply draw a line out here and drag it down, and connect back over, and have geometry that we could extrude. But Inventor also has an auto project capability. If we hover over this line, you'll see that it turns black and we snap to it, and the heads up display shows that we're gonna create a coincident constraint. This comes in quite handy because, rather than manually going and projecting this edge, Inventor's gonna automatically project it for us. If we right click and select OK to get out of the command, and then return to the home view, you can see that Inventor has automatically grabbed this edge from down here, and moved it up or projected it as reference into the sketch that we currently have. This allows you to use the project capability, but not have all edges projected every single time. By doing that, if we return to the top view, we can either project this bottom edge, or we could simply right click and Create a Line that connects the end point of the line we first created, and the end point of the projected line. And now if we look at this from an isometric view, you can see we have a profile here of this angle, that we can use to cut a slice through this model. I'm gonna go ahead and right click and select General Dimension, and I can add a dimension here as well. This allows me to control the angle of this line, let's say for example we set it to 40. When you hit enter, the model is updated and if we look at it from the top view, it doesn't run all the way off the part, so that's fine. I'll go ahead and finish this sketch. We can now right click and select Extrude, and that profile we created is able to be used to slice this model. Obviously, right now, it's trying to add materials, so we can change this to a termination of Through all. And we'll change the operation to a Cut. But you don't need to understand that necessarily, we'll cover that when we get into part modelling. But the point is, we now have the ability to project part edges, in order to help facilitate creating geometry that we can use to modify this part. By clicking the green check mark, you can see that we have the sliced edge cut now, and in the browser, Extrusion4 is the sketch we just created. It was consumed when we extruded that slice. But we can always return to that in the browser by clicking the plus symbol next to the feature to expand it, and the plus symbol next to the sketch, to see that we have projected loops. But, you can double click on the sketch to edit it, and then you could double click on any other dimensions you've created, let's say maybe we change this to 30 and hit enter. That'll update the geometry in the sketch, and when we finish this sketch, the model's updated to reflect that change. The next option I wanna talk about is projecting sliced edges or cut edges. This can come in really handy, and it's something that I use quite frequently. So I wanted to make sure you understood how to use it as well. In order to show this, I need to create a new work plane, and I'm gonna use the default work plane tool in the ribbon bar under the work features panel. And I'm gonna create a work plane that's parallel to this plane through the mid point of this line. Now that we have that, we can go ahead and create a sketch on this plane. I'm gonna select it and use the heads up display to create a new sketch. Now what you see here is we have a work plane and we have a sketch created, but we have a lot of geometry in the way. If I rotate this a little bit, you can see all this geometry that's in the way of the sketch plane. One of the ways we can fix that is to use what's called slice graphics. If we right click in the graphics window with nothing selected, there's an option for slice graphics. It's F7 on your keyboard. If you go ahead and select that, what you'll see is the texture changes a little bit, and now all of a sudden we can see into the model a little bit more clearly. If I rotate that model again, you can see all the geometry has been temporarily removed, so that we have a clear view of what we're working on. Remember, F7 on the keyboard is the toggle for this, so clicking F7 on the keyboard simply toggles that geometry on and off. With the geometry off, let's go ahead and project some geometry. We could go to the manual project and select each of these edges and project em'. Or, if we use the dropdown, there is an option for Projecting Cut Edges. If we select that, and then we'll automatically run around the edge of the part, and we'll find any edge that intersects with this plane and project it to the sketch. We can now use that geometry in order to control some of the other information we're gonna create. For example I can right click, select Create Line, and I can use the mid-point of that projected reference geometry to start my line. I could then use the geometry on the slanted face to find my perpendicular point, and I now have a line that's fully constrained based on the reference geometry we created. It's locked to the mid point of the first reference line, and it's perpendicular to this angled reference line. With that in place, we can right click and select OK. And we can finish this sketch. Now what we have, is you can see, the geometry has been turned back on, because that slice was simply a temporary solution to see this sketch. And we can now right click and select Extrude, and use the two pool files we created to, for example, create a slot. So rather than joining material, I'm gonna change this to a cut operation, and rather than moving it one direction, I'm gonna do some metric, and finally, I'll use the heads up display to shrink this down. And now, we have a slot that has been created using that work plane that we created, and we've projected slice edges to help facilitate the creation of this piece of geometry.

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