Building a Scooter Handlebar Component Using Extrusion and Shell Techniques

I am so excited! Our scooter is now ready for its handlebar. To begin, let's make sure we activate our top level of our project browser. With that top level activated, let's go to Create and select New Component.

This component will be called Handlebar, and the parent is that top level. We'll click OK. We'll open up our handlebar to expose its inner folders, and now we will go to the Construct menu and create an offset plane.

We'll select that center plane with an offset distance of zero and click OK. In the Construction folder, that plane will be given a name. Let's call it Handlebar Center, and now we can create a sketch.

Let's make sure nothing is selected. We'll click out in space, go to the Create Sketch button, and pick Handlebar Center. Let's zoom up to our clamp.

Now we know that that handlebar will go right through the center open portion of our clamp. So let's go ahead and go to the Create menu, and we're going to find Project, Include, and Project. And like before, we'll click the very center circle of that clamp and click OK.

So there it is. We have that projected sketch. Now if you recall, the downside of the projected sketch is it will be locked to that other geometry, which is actually now in the clamp component.

And I don't really like referencing another component with a new component. It can be kind of confusing in the project browser if we have to make any changes. So kind of a little workaround we can do is go back to Create, Circle, Center Diameter Circle, and click that center purple dot.

Make sure that it goes right to a center point constraint, which looks like a blue circle. We'll click that one time, pull our cursor away, and we'll type in 50 millimeters, which is bigger than we need. But it sets a circle at the correct center point.

Now we'll go ahead and select our projected geometry. We'll select it and hit Delete on our keyboard. We're only left with this bigger circle.

Now we can double click the dimension and change it to 26 and click Enter. And it puts it at the correct size, at the correct center point, without having any projected geometry. With that, we can go ahead and click Finish Sketch.

We'll open our sketches and notice it's not locked because it has no projected geometry, just the geometry we drew, and yet it's in the correct place. Let's go ahead and give it a name and we'll call it Handlebar Profile. With that, we can orbit to a more 3D view and take a look at the result.

We have this profile right in the center of our clamp. Now let's go ahead and go to the Create area and look for Extrude. And we want to select our profile, which is this Handlebar Profile.

We'll select it and our direction is symmetric. And we want to type in our distance, which will be 180. And we want to ensure that the operation is New Body and then click OK.

So that gives us a Bodies folder and Body 1. We can call it Handlebar. Now we don't want a solid Handlebar, we want it hollow in the center. So let's go to Shell under the Modify area, click One Face, hold Control on my keyboard, and click the other face.

We've got both faces selected. We can give it an inside thickness of four and verify it is hollow on both ends. You know what? Four might be a little bit thick, so let's go ahead and change it to three.

So three millimeter thickness, that looks pretty good. And let's click OK. So there we are.

We've got our Handlebar, our Handlebar Profile for sketches, and our Handlebar Center is all that we need to create this Handlebar component. It looks really good. We can go ahead and minimize our Handlebar component, reactivate the top level, and smash that Save button.