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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.
We're now to the portion of the course where we can start really looking into the settings into some of our sketch features. We're going to start with the extrusion, and I'm going to break the extrusion functionality up into several movies because I want to talk into detail about some of the settings, and some of the uniqueness about the extrude. And the one thing that really helps people with Inventor, is once you learn how to create one feature like an extrude, we use very similar options, throughout things like revolve and loft and other features.
So that once you have the basic understanding on how to create one feature, that translates to other components as well. So I'm going to start with the extrusion command and focus a lot on the settings. Which hopefully will make the remaining features that we're going to cover a little bit easier. I'll start by creating a new part, selecting Standard.ipt as my template and clicking Create. As I mentioned previously, the very first feature in a part is going to be a sketched feature. It's called the base feature.
And it is a little unique because it's the very first feature. So I'm going to go ahead and create a new 2D sketch. I'm going to select a plane to sketch on. And we can begin creating our geometry that we want to extrude. I'm going to right-click in the graphics window, and select Two Point Rectangle from the marquee menu. I could also go to the draw panel and select Rectangle as well. But I prefer the heads up display. I'm going to start my rectangle at the center of the sketch, and I'm going to use the heads-up display to enter a value of two for its length.
I'm going to hit Tab on my keyboard and enter one as its height. I'm going to hit Enter on my keyboard to enter that, and the geometry is created. I'm now ready to finish this sketch and apply a modeling action. Here we're going to use the extrude. And again, you can see this sketch is unconsumed in the browser. And because this is a sketched feature, when I click extrude. What you'll find is Inventor automatically selects the one rectangle that was available that was available for extrusion.
And it brings up the heads-up display, now I'm going to move this around just so we can talk a little bit about some of the settings here. The other thing I want to call out is the fact that we have what is essentially the original extrusion dialog box, available. And sometimes we have students or new learners to Inventor, look at this just so they can see visually some of the options that are available a little more clearly. But, all of the features are available in both of these displays even though you are going to most likely lean towards the heads up display.
You can see that I have a profile option here and here. I have different output methods here and here. I have the different types of extrusion I can create in this line here. And I have the direction located on this drop down. Now you'll also notice, I'm going to collapse this, because I do like the heads up display. It's a little less in your face and it, it just stays out of the way a little more. So I leave this collapsed by default. Since we only had one profile, Inventor automatically selected it and set it to a distance.
To the left of that distance, we have what's called the termination type. Right now it defaults to a one inch distance, and we can change that distance if we want. And we can also select to a specific face or point, or between two faces. Generally, the first extrusion is going to be to a distance, so we'll leave that there. As I mentioned, we do have two different output types. We can output surfaces or solids. In this case, we're going to focus on the solids. And because this is the very first feature, we don't have the option to join, cut or intersect material.
We only have the option to create a new solid. And this is because it's the very first feature and it's what we're going to be building from from this point forward. The other option is the direction. We can simply select different direction options, to toggle back and forth the direction we're going to extrude. The symmetric option will maintain that set distance, but it will extrude a half inch in one direction and, and a half inch in the other direction. Finally we have asymmetric, which allows you to change the distance on each side of that extrusion.
I'll go ahead and set that back to it's original direction and click the green check mark to create the feature. If we zoom back to the home view you'll notice that we have the Extrusion 1, the original sketch that we used to create it, and we're ready to continue modeling. So what I'm going to do is I'm going to select this face on this model, and use the heads up display to create a new sketch. Next I'm going to go ahead and right-click in the graphics window, and select Two Point Rectangle, and create a rectangle in the inside starting at the top line.
Down to the bottom corner roughly so it looks like it's offset. Essentially what we are going to do is create a U channel. I'm going to right-click in my graphics window and select General Dimension, and I'm going to dimension the distance I want that rectangle offset from the original outside edge. In this case I'll enter 0.25. While still in the dimension command. I'll continue around adding additional dimensions. Rather than enter 0.25 for every single one I'm simply going to click on the original 0.25 dimension to enter its parameter so that I only have to change this one and update all three of these that I'm creating.
I'll select that original 0.25. And now if I want to change that, I can go back to here, change it to 0.125, and all the dimensions update. I'm going to go ahead and cancel out of the dimension command and undo that so I'm back to my 0.25. And I can finish my sketch. This time when I go to hit the extrude by right-clicking and selecting Extrude from the marquee menu, something different happens. Because this isn't our first feature, we now have been placed into the Profile section which allows us to select which shape we want to take action on.
For this part, I'm going to select the inner rectangle. And it extrudes it to a distance. It remembers the previous distance we used. And it's adding material. In the first feature, when we looked at this type of extrusion, we didn't have the option for Join, Cut, or Intersect yet, because it was the very first feature. So now that this is the second feature, we have the ability to decide the type of extrusion we're going to create. Join will obviously add material, Cut will remove material, and Intersect will create a solid at the intersection of the two shapes.
Here I'm going to select Cut. And you'll notice that since we extruded to 1.3125 previously, that that value is still entered there. And if we were to hit OK, or click the green check box, you'll notice that the solid looks as if that rectangle cut all the way through the part. And it has. But what's important here is we didn't really talk about the type of termination we're using on the extrusion. Let me show you what I mean. I set that to a distance, and I extruded it.
But because Inventor is a history based modeler, I can essentially go back in time, by double clicking Extrusion 1, and changing it from 1.3125 to say, 1.5. You can see the update previews. And when I click the green check mark the model updates, but this second extrusion, because it was set to a distance, essentially is pulled back into the model and doesn't cut all the way through, which is not my design intent. So let's go back and double-click on Extrusion 2 which brings us back into the creation dialog box where we can go back and adjust settings.
And the setting we need to look at here is rather than extruding to a distance, we want to go through all. And what that does is, it just means cut all the way through the part, regardless of how thick it is. And that comes in really handy because now, if I were to go back and make changes, I can ensure that this cut is going to run all the way through. Those are the basic settings for extrusions. Now we'll look at another type of termination.
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