Combine sketch tools and adjust with Design History

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In the previous part one video, we set up this loft with three cross sections and a guide path. Okay, so now we have three cross sections of different diameter and they're all connected to the guide curve. The guide curve can't go between the centers of the circle, it has to go through the actual arc. And now we go to tools, loft, select inside each circle.

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and then you might have to zoom up a little, but select that guide curve. And it should just snap into place. If it doesn't snap into place, it probably means that your guide curve doesn't touch your cross sections. The next part of the handlebar is pretty easy. We'll just grab the end face and we'll drag this out, say six inches. And now we're going to make this hollow. So we'll go to tools again.

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shell, select the flat end, the two flat ends, and...

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Drag the arrow to create a thickness, say 0.1, and done. So now we have a curved section of hollowed out tube that's been expanded in the middle, and we need to add a couple more features. One is we need to add a riser on here to connect it to the rest of the fork on the motorcycle, and we have to mirror

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the entire thing so we have a left and a right. In order to do this, the standoff has to intersect the handlebar, but it has to do it at an angle. We're gonna start with some construction geometry. I'll make a sketch on this plane. I'm just gonna draw a line from the center of the circle down a certain distance. Let's make this six inches. Well, we need another horizontal line here.

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Let's select the two lines.

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and add an angle dimension. And now that's complete. All we needed here was construction geometry. Notice also that this isn't right where you need it. It's in the middle and we're going to need this off to the side. The way we're going to handle this is this way. I'll create another construction plane. Again, using perpendicular to curve at point.

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So we'll make it at the end of this line that we created out here. And say done on that. Now we're going to create a new sketch on this angled plane.

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The software brings us normal to the plane, which is going to help us in this situation. In this sketch, we're going to sketch in a circle, make sure it has an inch and a quarter diameter, and I'm going to want to add a rectangle from the center of the circle to the origin.

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and select the rectangle, make that construction.

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The main point of this rectangle is just to get a six inch dimension.

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and make this horizontal and place this circle in the middle of the handlebar. Now we can exit the sketch and take a look at this in 3D. From here I want to extrude this circle and I'm going to drag it up to the handlebar. Notice that it snaps right to it and it's mitered

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It hasn't gone through it on the inside. This is just the way we want it to be. But we might also want to hollow out this part. Now there are a couple of ways to do that. Some of which ignore a little bit of manufacturing process, but we can deal with that separately.

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So let's take a look at the history tree and see what we have going on. This shell feature, I'm going to grab this shell and drag it down after the latest extrude. And when I do that, it should shell out this extrusion, but it doesn't. If we look over here, we notice that if I change from all items to bodies, we have two bodies.

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and that these two features have become separate bodies. That's not at all what we want. So we go into the extrude and instead of the combine type being new body, we want that to be a union. And once that's complete, we have to tell it what we want to combine it with. So will the combined

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solid body and we say done and now we see that this little piece is hollowed out as well. Although it's not hollowed out on both ends. So now we have to edit the shell, select another target face which is the end face of this riser. Click done and now we have a completely shelled out half.

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of a motorcycle handlebar that can't necessarily be manufactured this way easily. Let's do something else that makes it even more difficult to manufacture, but it's an interesting design aspect. We can go in here, grab this edge, drag it out with the arrow to make a fillet.

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And then once we collapse the extrude and the shell feature, we notice that the fillet shows up after the shell. If we push the fillet before the shell.

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Now we can see that the shell has also shelled out around the fillet, which is a very cool thing. It's not necessarily how you'd make these parts, but here we're just showing how to make the geometry. The final step is to mirror the handlebar. So mirror is under the transform menu. Come down to mirror and it wants you to select the items to mirror and then select the mirroring plane.

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So the items to mirror are this body and the mirroring plane. We'll just see if we can select this face.

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And now we've got both sides of the handlebar. Click on done. But if we look at this now, we've got two separate bodies, which is again, not really what we want. So we'll use the tools.

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Union.

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Select both bodies from the list. And you'll need to use Shift-Select for the second one. And click Done. Now we've got a single body of a shelled out lofted handlebar that has the flexibility of history-based design. Thanks for watching.