Trim, extend, and split tools

- [Voiceover] Now that we've learned how to create geometry, it's time to explore how to modify that geometry. You've seen some of the modifications in previous movies. For example, when we were working with constraint, you saw me left click and drag on geometry to see how it reacted based on the rules that were applied, whether there be dimensional constraints or geometric constraints. As you click and drag, you get to change the overall shape based on those rules. Now we're gonna look at how we can actually use some additional modification tools, such as trim, extend, and split, to make modifications to sketch geometry.

We're gonna start with a part file. If you don't have one, go ahead and start a new part file, and right click on the graphics window, and select New Sketch. I'm gonna select the XY plane to sketch on, and pan down into the left to give us room to work. At this point, I'm gonna go ahead and right click, and select Create Line, and create a basic shape we can work with. We're gonna simply draw a horizontal line. The dimensions aren't important, so we're not gonna enter them, but what is important is that we have geometry here that we can use to practice the trim, extend, and split tools.

Go ahead and create this piece of geometry. When you're finished, right click and select OK. We're now ready to explore those tools. Let's say for example, we had a design change and for some reason we needed to remove this whole top section of this geometry. We could simply select all the geometry and hit delete and redraw it, but we could also use the trim, extend, and split tools to help us. Those tools can be found on the sketch tab under the modify menu here in the center. Let's go ahead and start with the extend in this case.

The reason I'm using this one is because now if we hover over this horizontal line, we can see that Inventor automatically tries to extend it to the next piece of geometry. If we were to hover over the vertical line here, the same is true, but it extends in a different direction. One of the unique features of the extend tool is that if we hover over the line on the right, it will also extend, even if it doesn't have geometry to hit. What it's doing is evaluating what this line would be if it was extended all the way to that point. We'll go ahead and hover over the horizontal line, and left click.

That will extend that geometry all the way to the left until it hits the vertical line. Next we need to trim away some geometry. Now, we could go to the modify panel again, and select trim up here, but, while we're still in the extend command, because these commands are often used together, if you right click on the graphics window, you'll see Extend, Trim, and Split, are toggles that you can switch between without having to return to the menu. I'm going to go ahead and select Trim, and now if I hover over geometry, the dotted line indicates geometry that's gonna be removed.

If we clicked right here, it would remove the line we just extended, and we'd be where we started. What we're gonna do is go ahead and trim this line on the left, the top half of it. Now the other things that's a little unique around the trim tool, similar to something that's unique with the extend tool, is you can select geometry that really doesn't have a way to trim, and it will remove it. This comes in really handy, because you don't have to exit this command and try to delete geometry, you can use the trim as a trim or a delete, depending on the sketch geometry you have.

Now that we've seen the Trim and Extend tools, let's right click and select OK, and get out of the command, and let's create a couple other pieces of geometry. Let's draw a rectangle that overlaps the first rectangle, and let's draw a circle by right clicking and selecting Center Point Circle, that intersects the top rectangle. The reason I wanted to do this is to show where the split tool can come in very handy, and also explain a little something that Inventor does when it's creating extrudes, or evaluating a sketch for profiles.

Before we get into the split command, let's go ahead and finish this sketch, and let's right click in the graphics window, and select extrude. Now the way we drew this geometry, we essentially drew the first rectangle, then we drew the second rectangle, and then the circle. None of those were started on or ended on any of the previous geometry, so we really have the circle here, the rectangle here, and the rectangle at the bottom. The difference is, as you can actually see in the background, the highlighting shows other profiles that you could also create.

We have the light blue area on the bottom. We have the dark blue rectangle in the center, a light blue area above that. A dark blue where the circle and the rectangle overlap, and then the light blue again on the remaining section of the circle. Let's go ahead and hit cancel, and let's edit that sketch one more time. We'll double click on it in the browser to return to editing. Now that we're back in the sketch, let's look at the split tool. I'm gonna select the Split tool from the modify panel, and as we hover over geometry, what's going to happen is, from where the cursor's located, Inventor is gonna run in each direction around the circle until it hits something that can split that line.

It doesn't matter if you pick the top half or bottom half, it's gonna run in either direction until it hits something. I'm gonna go ahead and select the bottom half, and you can see it's done that, it's hit intersection points here and here. We're gonna do the same thing with this vertical line on the left, and the same one with the vertical line on the right. You can see now that we have intersection points at these locations where you see the yellow dots. Go ahead and right click and select OK to get out of the command, and let's finish that sketch now. This time, when we right click and select Extrude, instead of getting the circle, we get the top half of the circle, and you can see, each of those areas that were overlapping are now individual profiles that can be selected.

In the end, if you select them all, you get the same general shape that you had before. However, you can always hold Shift down and remove specific sections as needed. You can always, with Shift held down, add those sections back as well. Hopefully you can see how Inventor uses the split command and intersection points to create this geometry, and where that would be beneficial for you during your design process.