Join John Helfen for an in-depth discussion in this video Import AutoCAD data, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now gonna look at another way we can create geometry. Up to this point in the course, anytime we needed sketch geometry, we simply drew it ourselves. But many of you may be coming to Inventor from AutoCAD and may be thinking to yourself, "Well, I don't want to recreate the geometry. "I've been creating it for years in AutoCAD." So we're gonna look at how we can import that geometry and use shared sketches to create Inventor models from AutoCAD data. To do that you need to start with a part file which I have on the screen, and you need to start a new sketch as if you were gonna draw the geometry yourself.
So, we'll right-click and select New Sketch and we'll select a plane to sketch on. Now that we're in the sketch environment we could go about our geometry creation by using the tools in the Create Panel to draw our geometry. But as I mentioned, we're gonna import AutoCAD geometry. And to do that, we can go to the Sketch tab under the Insert panel and select ACAD or AutoCAD. Doing that will bring up a dialog box where you can browse to find the drawing. In this case, I have a drawing I've created, Importing AutoCAD Geometry.dwg that we're gonna use for this portion of the course.
I'm gonna go ahead and select that geometry and click Open. After a moment, the dialog box is presented and we can see the geometry that was in our AutoCAD file. In the import preview window, this is a live window. What that means is, if we press and hold our middle mouse button we can actually pan the geometry around or we can scroll by using our wheel on our mouse to move the geometry closer or further away. The other thing you might see is just above this window there's a toggle to switch between a white background and a black background.
Depending on your preference, either is perfectly okay. I'm gonna go ahead and set mine to black. I think it makes it a little bit easier to see the geometry. Now, on the left-hand side of the dialog box, you can see the selective import list. What this really means is it's a list of the layers that are in AutoCAD. Now, the last time I imported geometry, I had the hidden layer turned off so it remained that way. You'll probably see these both selected. What's important here is to know that you can select or deselect layers that you do or don't want in your geometry.
In this case, I don't like importing the hidden geometry because I don't think it's gonna help us. What I really wanna do is find the view that best defines the part I'm gonna create in Inventor, and that's this top view. But by default, Inventor automatically is set to select everything in the drawing. So I'm gonna uncheck this All option, and I'm gonna select just the top view. If I go to this window and left-click and drag, I can draw a loop around the geometry I want and you can see it's highlighted blue.
I'm gonna go ahead and click Next and now we have a few options that we can set to configure the geometry so that it works appropriately in Inventor. There's gonna be a couple options here that we wanna pay attention to. First, is the units. I know that I created this drawing and I know created it in inch so I could specify the units but I went ahead and let Inventor detect the units and it did correctly. So I'm gonna leave that as it is. Now, the first time you come into this dialog box these two options are gonna be unchecked.
The first one is Constrain End Points. What this does is it takes all of the AutoCAD geometry that's being imported and takes any end point that is overlapped with another end point or, for example, at a corner of a box, and it's gonna apply coincident constraints to those end points so that Inventor can evaluate those closed loops as profile for modeling actions. And you'll see what that means in a moment. So, I'm gonna go ahead and check that. The other one is Apply geometric constraints. I'm gonna check this as well, and what it does is automatically apply certain constraints in Inventor.
For example, tangency. This will prevent us from manually having to add some of those constraints once the geometry has been imported into Inventor. With those settings checked, I'm gonna click Finish and after a moment, you can see the AutoCAD geometry has been imported. But it's not positioned at the center of our sketch. However, it is positioned appropriately based on the AutoCAD file. What Inventor does is it takes the zero, zero, zero point in AutoCAD and maps that to the zero, zero, zero point in the sketch. And that's fine, that works for us.
But I still need to move this geometry because when I create geometry I like to lock stuff to the center point of the sketch so that it scales properly. To do that, we're gonna return to the sketch tab under the Modify panel and select Move. We default to the selection option which allows us to simply left-click and drag a window across the geometry we want to import. We can select the Move option and pick the base point for the move which in this case is gonna be the center of the circle, and then we can move our cursor down to the center point and left-click to lock that geometry in place.
I'm gonna go ahead and click Done and double-click my middle mouse button to zoom in on all the geometry. We've now imported geometry from AutoCAD, and at this point it's as if we created it in Inventor. The nice thing is we're ready to create 3-D geometry from the 2-D AutoCAD file. I'm gonna finish the sketch and double-click on my middle mouse button to zoom out. And then I'm gonna right-click and I'm gonna select Extrude. Now, what you'll see here is Inventor is just like any other geometry, allowing us to select from the closed loops that have been created.
And I'm gonna go ahead and select all of them and I'm gonna set my distance to .5 and I'm gonna select OK. We now have the base feature of this model created from the AutoCAD geometry, but you'll notice the sketch we imported, Sketch 1, has now been consumed by this extrusion because it's driving the overall shape of this extrusion. And I don't want that. I still wanna use this sketch. And that's where shared sketches come in handy. Shared sketches are quite frequently used when importing AutoCAD geometry because, as you can see, I can create multiple features from that single view in AutoCAD.
To do this, we're gonna right-click on this Sketch 1 on the browser and select the Share Sketch option. What this does is tells Inventor that this sketch is special. Not only is it used for Extrusion 1, but it contains information for other geometry as well. I'm gonna go ahead and collapse Extrusion 1, and if we rotate to the other side of the model you can see that that sketch is visible again. What we'll do is right-click and select Extrude one more time. And this time, we're just gonna select the ring that makes the boss and the circle that makes the whole.
And by default because this is touching a 3-D model, it assumes you want to remove geometry, and that's not the case right now. And that's easily resolved by going to the operation drop down and changing from a cut to a join. You can now see we're creating geometry and it remembers the last distance we used. So what I'm gonna do is I'm gonna use the heads up display, and I'm gonna drag this out to 1.5 inches. Once we're there you can see we now have another extrusion. I'm gonna click the green check mark and in the browser, we have Extrusion 1 which is the base; and we have Extrusion 2 which is the boss.
If you expand the plus symbol next to each of those you can see they're both driven by Sketch 1, which also still remains open and out in the browser. Let's go ahead and right-click one more time and select Extrude. And this time I'm gonna hover over and select what is the profile that makes the whole. And when I do that, Inventor automatically remembers the distance that we used previously. And because it was on a piece of geometry, it automatically chooses the cut operation. I'm gonna make one minor change.
Rather than extruding to a distance of 1.5, I'm gonna change this to through all, and that's just so that if this model were to change in height, that whole would remain all the way through the part. We now have our part created, and we now have a third extrusion which is also controlled by Sketch 1. And Sketch 1 is visible in the browser still. And now that we've finished using it, we can simply right-click on it and select Visibility to remove it or hide it from the graphics window. The nice thing about this is we now have three different features that are controlled from the first sketch.
So at any point during the design process, you can go back and double-click on Sketch 1 to edit it, perhaps make a change to the model. Let's make this slot a little bit deeper, and we can finish that sketch, and you'll see that the geometry is updated. We can also add dimensions and things like that or even make adjustments to it, create additional geometry or trim some geometry away. But the point is, is you don't have to create all geometry from scratch if you have a library of AutoCAD data.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers