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We've now learned how to create geometry in Autodesk Inventor. And, for those people who are coming to Autodesk Inventor for the first time, or it's their very first CAD system, the geometry creation tools in Inventor are fantastic and you can continue moving forward creating your geometry. And, you'll be good to go. From those people coming from AutoCAD, another Autodesk product, you might be thinking, well I already have geometry. I have geometry, I've been creating for years in AutoCAD and I wouldn't want to lose that, why do I have to recreate it, and in this case you don't have to.
So, what I wanted to do is I added an importing AutoCAD geometry into the essentials course because of those people who are coming from AutoCAD and that's probably quite a few. So, let's begin by creating a new part file and we'll look at how we can reuse our AutoCAD data within Autodesk Inventor. I'll begin by clicking New on the tool bar, selecting standard.ipt as the template. And clicking Create. Now, to begin, we need to start as if we're going to create geometry in any other fashion and to do that we need to create a 2D sketch.
We'll go to the 3D Model tab under the Sketch panel and select Create 2D Sketch. The origin geometry is presented and we can select a plane that we want to add geometry to. We're now in the sketch and if we wanted to we could manually begin drawing geometry. But like I said, we want to import geometry from an AutoCAD file. So, rather than go to the Draw panel and start creating geometry, we're going to go to the Insert panel on the Sketch tab and select ACAD or AutoCAD. This will allow us to import the exercise file I created for this portion of the course.
It's called ImportingAutoCADGeometry.dwg. Once the dialogue is presented, you can see a few different sections that we'll be working with. The main section is here on the right, and this is an active preview window. What that means is, you can use your wheel on your mouse to pan by pressing and dragging, or zoom in and out by scrolling your wheel in and out. The other item that I wanted to call out here is the fact that you can toggle the background color and this is going to be helpful, especially in this case because the white background, in my opinion, makes it hard to see the geometry.
And there is a toggle here, I'm going to toggle with the dark background and for my vision it makes it much easier to see the geometry of You can always toggle back and forth at any point. The other item you'll notice is we have a list of layers in our browser. And I just checked the hidden line, which was unchecked from the last time I imported geometry, but it shows an important component of what this window does. Based on the layers that are set up in AutoCAD, they'll be listed here, and you can uncheck or check any layer you wish to remove it or add it to the geometry that's being imported.
I'm going to go ahead and uncheck it because I don't like the in, the hidden line geometry being imported by environment. The other item just below that browser is the selection options. By default, Inventor will select all the geometry, assuming you want to import all views. I don't want to do that in this case. I'm going to uncheck All, and I'm automatically placed in the selection mode. I'm going to pan and zoom in just a little bit. To look at this top-view. And that's the one that I feel provides the best definition for my Inventor model.
So, I'm going to go ahead and left-click and drag in this window. And you'll notice that the geometry is updated to be dotted, indicating that it's selected and ready for import. We can then move forward by clicking Next. On the next section in the dialogue, there's a couple settings that need to be set. First, by default, Inventor is set to detect the units from the AutoCAD file. I drew the file an inch, so I could define it because I know it. But you can also have Inventor automatically detect id. I'm going to leave that as it is. The other options we have are the ability to constrain end points and to apply geometric constraints.
I generally try to keep this on unless I run into some type of problem that prevents me from using it. But what it'll do is essentially make sure endpoints are connected so that Inventor can find close looped profiles, and it will automatically apply certain constraints. Things like tangents, for example. I'm going to go ahead and click Finish. And you can see that the geometry has been imported into my graphics window. You'll notice that also that it is not exactly in the center of my sketch and that's as expected.
What Inventor has done is taken the 0,0,0 point in AutoCAD and matched it to the 0,0,0 point in the origin of the sketch. And if you remember, when we were looking at the preview, the top view was again a little bit higher and the front view was down below closer to zero. So, to position this, I am going to go ahead and use the Move command. I'm going to first select all the geometry that I want to move and you don't have to do that first, you could do that in the dialogue as well. But, if I select it first and then click Move here on the modified panel, then you'll notice that my selection mode is already in a complete state.
It's no longer red, it has something selected. And I can simply go to the base point option and select the center of the circle. I'm now able to move this geometry around and I'm going to locate it at the center of the sketch. I'm going to do this by simply left clicking on the center of the sketch. And then I'm going to click Done. And I now have geometry positioned properly in this sketch for moving forward. At this point, it's as if you've created this geometry in Inventor. And you could continue on by adding dimensions, adding other constraints, and items like that.
Since we're not focused on that in this portion of the course, I'm going to go ahead and hit Finish Sketch, because I do want to call out another item when it comes to creating extrusions that'll come in quite handy for those who are importing from AutoCAD. And that's the ability to share a sketch. What you see here on the screen is the top view of my model. It shows the overall outline. It shows a slot that sliced into it. It shows a hole that's available and a boss that I'm going to add here. But they're all in a single sketch, and that's okay.
And that's why I wanted to call this out. I'm going to go ahead and right click in the graphics window and select Extrude, and select the profiles that I want to extrude. I'm going to set those to be 0.5 inches tall, which is the height of the base of that model, and I'm going to go ahead and select the green check mark to accept that value. Now, you'll notice, when I hit OK, the sketch is no longer visible. It's been consumed by extrusion one.
Here's sketch one. If I hover over it in the browser, you can see that highlight in the graphics window. So, what I'm going to do here is tell Inventor that I want to share this sketch with other geometry I'm going to create. Because this geometry had multiple loops, that's a perfect example of where Share Sketch comes in very handy. So, now that I've expanded extrusion one, I'll right-click on sketch one and select the Share Sketch option from the right-click menu. What this has done is told Inventor that I'm ready to use this geometry again to create a new solid model feature within this model.
If we rotate to the opposite side of the model, you can see that the geometry is visible again, and in the browser, something unique has happened. Sketch one is listed as consumed under extrusion one, but it's also listed outside of extrusion one as an unconsumed sketch. What that means is, Inventor can now use that to identify new closed loop profiles that can be used in a modeling operation. So, I'm going to right click in the Graphics window and select Extrude. And I can now hover over that and select those options again.
And because they're right up against Geometry, it automatically assumes we want to remove material. And that's not exactly the case. In some cases, that might be true. But in this case, I want to make this a joint operation. So I'll select the operation type and enter Join. Now, it remembered the 0.5 we had entered previously. So I need to update that to 1.5 to have that geometry extrude from the very base of that model, all the way to be 1.5 inches tall.
With that boss created, you can see extrusion two and extrusion one in the browser. And clicking the plus symbol will expand it. So that you can see that sketch one is now driving both extrusion one and extrusion two and is also available again to continue building from if we wish to. I'm not going to do that. I'm going to go ahead and collapse these and finish up by right clicking on the sketch in the browser and selecting the Visibility option to turn it off. We can now continue modeling by creating a hole. We could add some Fill Its or make any additional modifications we need to this part.
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