Join John Helfen for an in-depth discussion in this video Create a base extrusion feature, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now ready to really begin digging in to part modeling. And some of this you've seen, but really what I want to do is focus on the Extrude command here. And I'm going to spend a little bit extra time on the Extrude command talking about some of the interface components and the concepts, because many of the features within Inventor follow these same types of concepts and use the same types of interface components. Once you understand the details of creating a basic extrusion, it'll ease the process as you continue through the part modeling because you'll become familiar with the general process in the first place.
We're going to start by creating a new part file. If you don't have one, go ahead and open a new part file. And let's create a sketch by right-clicking in the graphics screen, and selecting New Sketch. We can then go ahead and select the XY plane to sketch on. And we'll begin by creating a rectangular shape. We'll right-click in the graphics window and select Two Point Rectangle. We'll hover near the center point of the sketch and left-click to initiate the rectangle. And then we'll go ahead and enter 1.000 for the distance on the length, hit tab, and hit .75 on the other value.
Once you hit Enter on the keyboard, your geometry is created, and we're ready to continue. We can go ahead at this point and finish this sketch. Now what we've done is created our base initial sketch. You can see it here in the browser. We're now ready to apply a modeling action. In this case, we're going to focus on Extrude, so we'll right-click and select Extrude from the marking menu. You can also find it in the Create panel here in the ribbon bar, the Extrude button. But I'm going to stick to the heads up display because I feel that it's more efficient and I really want to encourage everybody to work this way.
Once you click the Extrude command, Inventor automatically selects the profile. Let's go ahead and drag the heads up display up and out of the way a little bit so that we can look at some of the settings. Over here on the left, you can also see that we have an Extrude dialog box that's automatically collapsed. As a new user, I do refer people to this dialogue box because it does have some labels in it, and you can see the icons and how they relate to those labels. And once you get an understanding of how this all works, the heads-up display contains all that information and more.
But it's nice to see how these icons relate to each other and relate to the text in the dialogue. Let's go through some of these settings. Again, because the first sketch we created only had one profile, the profile option is already solved. It selected the one profile we had. If we had multiple profiles, this would be selected, and it can be found here, in the heads up display. And you would have to pick the profiles you wanted to use. The next area we want to look at is the Output options. We have the option for Solid or Surface.
And that's available here in the heads up display as well. We're going to stay away from Surface right now, really, for the most part, the essential stuff you need to understand is around solid modeling. The next option is the type of operation you're going to create. Now, we're in a unique situation. We're creating what's called the base feature, the very first feature in the model. And because of that, these buttons here are grayed out. And the only one available is New Solid, at the bottom. These same options can be found in the heads up display as well, and if we click the dropdown, you can see the descriptions. Right now because this is the base feature and there isn't a sold model in this part already, we can't do a Join, Cut, or Intersect.
The only option we have is to create a new solid. And that's what we'll do. We'll leave that set. We'll come back to this in a minute because these options will be available to us on the second feature. Next, we have the extends. And this is actually a few different components from the heads up display. The first one is the Distance, and here you can see we have Distance To and Between. This can be found here just to the left of the Distance value on the heads up display. You can see that we list all the options here in the heads up display. We just gray out the ones that aren't available.
But, the ones that are available are the same as what you saw in the dialogue. We have Distance, To, and Between. We just have a little bit more description in the heads up display. The next option is the Distance. That's pretty self-explanatory. And then below that, we have the Direction. That can be found here in the heads up display as well. We have Direction 1, which we're in now. Direction 2 simply flips the direction of the extrusion. Symmetric will keep the distance at 1.000 inch, but will extrude equally a half inch on each side of the sketch we selected.
And finally, we have Asymmetric. Asymmetric allows you to select a different distance on each side of the sketch. We're going to go ahead and leave it at Direction 1. That works for us for right now. And we're going to go ahead and collapse the dialog box, because we're going to focus on the heads up display from here on out. And we'll select the green check mark to accept these settings and create our base feature. Now in the browser, that sketch has been consumed because it is controlling this extrusion feature. We can always go back and double-click this to edit that and make changes to its dimensions.
And have the model update. Now that we have a model, let's repeat that process so we can see the changes in the Extrude command. Now that we have a solid created, let's go ahead and select the face on the side of the model, and use the heads up display to create a new sketch. The button on the far right is the Create New Sketch button. Once we have that, let's go ahead and right-click and select Two Point Rectangle. And let's go ahead and hover near the top horizontal line and left-click to initiate the rectangle. And go ahead and left-click down near the bottom corner.
The dimensions don't specifically matter here. I'm not even going to add them. If you want to practice and add dimensions feel free. But, they don't really affect what we're trying to show here. So, I'm going to leave them off. The one thing I will do, just so that we can show another option in the dialogue box, is I'm going to go to the Sketch tab, under the Create panel and select Project Geometry. And I'm going to project this entire face. The only purpose for this right now is just to show you an example of selecting multiple profiles. Otherwise I would not have projected that.
But we now have the rectangle in green and the rectangle in yellow. So that when we finish this sketch, and we return to the Extrude dialogue box by right-clicking and selecting Extrude, you'll notice that Inventor doesn't select the profile for us. Because we projected the entire face to the sketch, we now have two profiles that we can select from. We could select the outer rectangle, or the inner rectangle. And we're going to go ahead and select the inner rectangle. By default, Inventor sets it to 1 inch distance, that's the distance we used on the previous block for extrusion.
And, it joins material. It went ahead and selected the Join operation. And we can change that. I'm going to go ahead and move this up just a little bit so we can see it a little more clearly. And, if we look at the Join operation and we select the dropdown, you can see now we have Join, Cut, and Intersect available to us, along with New Solid. If we were to select New Solid, we would essentially get two separate solids in this file, and it's really beyond this course. I'm going to leave that alone. But, let's look at, right now we have Join, if we select Cut, a couple things happen.
Inventor automatically flips the direction to the opposite of the joint, and it changes the preview to a red color and removes the material. The distance is set to 1, and we're going to leave that. Now, I'm going to leave this on purpose, and I know it's going to cause a problem, but not right at first. And I want to explain this to you because it does come in handy, and it's going to let you understand how this concept works. But, I'm going to go ahead and select the green checkmark and leave that at 1 inch. And on the screen, you can now see we have essentially a U-channel.
In the browser, we have Extrusion1, which is controlled by Sketch1. And we have Extrustion2, controlled by Sketch2. Now what's important here is that while this looks correct, and it is, Inventor is a history-based parametric modeling system. That sounds really fancy, and it sounds like a lot of information, but, let me show you what that means. At any point in time we can go back in time and make edits to this model. If you start at the top, this is further back in time, and it progresses as you move down the browser.
If I were to left-click on this outer face, and look at the heads up display, I have the option to edit the extrude. I could also go to Extrusion1, right-click, and select Edit Feature. But we'll use that method in a minute. Let's go ahead and select the side face and edit this feature with the button on the far left. What that does is essentially returns the model back in time to when this was first created. You can see in the browser that the Extrusion2 is grayed out. And, if we update this to 1.5 and select the green checkmark, the model updates.
Now here's the problem. Believe it or not, Inventor has done exactly what we told it to do. We just told it to do the wrong thing, and that's what I wanted to show you here. Because we can go back in time and make changes, you need to consider that when you're creating your extrude features. Or any feature for that matter. If we return to the browser and right-click on Extrusion2, we can choose to edit this feature. Now you'll see it's still at 1 inch, that's exactly what we told it to do, but because we can go back in time and make changes, we need to consider that as we're creating new features.
I'm going to go ahead and change this. Instead of bumping this up to 1.5 or 100 inches so that it's really, really long, instead we're going to use the dropdown arrow to the left and change from a distance to Through All. What this means is no matter how large the previous feature had become, or how small, this cut is always going to remain all the way through the part. For example, if we click the green check mark, we get an update, and it works the way we expect. But this time, if we click on the side face, and edit this base feature, and update it to 2 inches, when we click the green check mark, you can see that the cut continues to run completely through the model.
And that's what we expect. If we right-click and select the Measure command, you can select the edge on the model, and, sure enough, it is 2 inches, even though this cut goes all the way through. At any point, we can right-click on the Extrusion1, edit its feature, and return it back to the 1 value and you can see that it updates. So you can build this intelligence into the model by selecting different settings in the Extrude dialogue box. And the same is true for additional features we're going to look at in this section of the course.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers