Join John Helfen for an in-depth discussion in this video Projecting geometry, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] 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 modeling. You're really going to 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 use 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 going to create here, so that we can look at projecting. I'm going to start by creating a sketch.
I'm going to 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 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 want to 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 the 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 want to 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 going to check it, I'm going to leave it off, but I want to expalin 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 going to 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 going to 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 this 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 autoproject 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 going to create a coincident constraint. This comes in quite handy because rather than manually going and projecting this edge, Inventor's going to 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 can simply right click and create a line that connects the end point of the line we first created and the endpoint 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 going to 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 in 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 out 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 material so we can change this to a termination of Through All and we'll change the operation to a Cut. Now you don't need to understand that necessarily, we'll cover that when we get into part modeling.
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 checkmark, 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 this 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 the sketch, the model's updated to reflect that change. The next option I want to 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 going to use the defautl work plane tool in the ribbon bar under the Work Features panel and I'm going to create a work plane that's parallel to this plane through the midpoint of this line.
Now that we have that, we can go ahead and create a sketch on this plane. I'm going to 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 them, or if we use the drop down, there is an option for projecting cut edges. If we select that, Inventor will automatically run around the edge of the part, and will 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 going to create. For example, I can now right click, select Create Line, and I can use the midpoint 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 in the midpoint of the first reference line and it's perpendicualr to this angled referenced 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 the sketch.
And we can now right click and select extrude and use the two profiles we created to, for example, create a slot. So rather than joining material, I'm going to change this to a cut operation and rather that moving in one direction, I'm going to 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 we created and we've projected slice edges to help facilitate the creation of this piece of geometry.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers