Designing a T-Shaped Clamp Component and Section Analysis in Fusion for Scooter Handlebars

We're now at a really exciting place in our model. We're all the way at the top of our stem, and now we need a clamp that will connect our stem to our handlebar. Let's begin by activating the top level of our browser.

Then let's go to the Create menu and select New Component. This new component will be called Clamp, and its parent should be set as the top level of our browser. Then let's click OK.

Now we're in this new Clamp component, and we need to create a work plane. Let's go ahead and go to the Construct, and we'll do an Offset Plane. We want to select the center plane here, and click OK with no offset.

Verify that it is indeed that center plane that aligns with the red axis. Let's open up our clamp, and we will find our Construction folder, and there is our generic plane, and we'll give it a name. We'll call this Clamp Center.

There it is. Now with that, we'll create a sketch. Let's make sure nothing is selected.

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I'll click out into space, and under the Create area, I will go to Create Sketch and select my Clamp Center. Going to grab that line tool and zoom in to my wheel hub, click one time, and I'm going to hover with my cursor to the top left of my screen. Now I want to type in the dimension.

It's going to be 770,770 millimeters. Then I'll click Tab, and I want 106 for my degrees, and click Enter. So there it is.

I've got a line from my hub up 770 millimeters. Now let's select that line, right-click, and change it from Normal to Construction. Now I want my actual line.

I'll go back to my Line command, click where I left off, move my cursor up to the left, and look for those parallel constraints. They're two blue lines, and I want to type in this time 50 for 50 millimeters, and click Enter. So there's a line I will use for the beginning of my clamp.

With that, let's go ahead and click Finish Sketch. Let's open up our Sketches folder and give this a name. Right now it's just called Sketch 1. We'll call this Clamp Vertical Tube Sketch.

So there it has a name now, and let's click on nothing again, and go to the Create area, and this time I want to select a pipe. So Pipe, which path do I want? It's that 50 millimeter line that we just finished drawing, so I'll select that. And for my section size, I want to type in 34 millimeters, and I don't need a section thickness.

I can simply uncheck the box next to Hollow, and there's no longer a thickness to the walls. It's just a solid section. I want to double check that the operation is set to New Body, and now I'll click OK.

So there it is. I've got one component or one portion of my clamp, the vertical part. Now I need the horizontal part, because it's going to make a T shape overall.

So let's go ahead and go back to our sketching. Go back to the Create area and select Create Sketch. I again want to select the clamp center to sketch on, and again, I'll click the line command, click in the center of my hub, right in the middle of that wheel, and then move my cursor up and to the left.

This time, I want to type in 820 millimeters, hit TAB on my keyboard, and again, I want that 106 for my degrees, and click Enter. And that takes me right to the top of that tube that we just created. Now I can select that line, right-click, and it only needs to be a construction line, so we'll select Normal Construction.

Again, we'll go to the Create area and look for, this time, the center diameter circle. We'll select that, click right at the top of the line that we just created, and pull our cursor away, and we want to type in 34 for 34 millimeters, and Enter locks that in. Once that is complete, we will click Finish Sketch, and let's give that sketch a name.

We'll call it Clamp Horizontal Tube Sketch. We've got our Vertical Tube Sketch, now we have our Horizontal Tube. Now let's go ahead and go to our view cube in the top right and click on the house.

We're looking at our scooter at a bit of an angle now, and we'll notice that we have that sketch, that Horizontal Tube Sketch, ready to go. Let's click on the Create area and look for Extrude. We will select that Horizontal Tube Sketch right here, that circle, and we'll change our direction from one side to symmetric.

We'll pull out both sides. Let's go ahead and set that to a distance of 50 millimeters, and we'll notice that Fusion wants to cut by default, but let's go ahead and change this to New Body. So New Body, and with that, we'll click OK.

And do you see the T shape now? We have that Vertical Tube and the Horizontal Tube that create a T. If we open up our Bodies folder, we'll see that there are currently two separate bodies, Body 1 and Body 2. But let's go ahead and intentionally combine these. In the Modify area, we're looking for the Combine tool. Click Combine, and we'll click on that Horizontal Tube and the Vertical Tube.

And we'll notice in our Combine window, we have both selected, Operation is set to Join, and we'll click the OK button. That should give us just one body. And now we can give it a name here.

We'll call it Clamp, and Enter. So there it is, and it looks really good, but currently, it's a solid thing. It doesn't open up to accept anything inside of it.

We want to shell this out. So in the Modify panel, we'll see a command called Shell. We'll click that Shell, and it lets us select faces or bodies.

Let's go ahead and be super intentional about this and click on Faces. So first, we want to click the front face of our Horizontal Tube. We'll click that, and we'll give it an inside thickness of four.

And let's, before we do anything else, see the result. It creates a shell, but it doesn't go all the way through. Do you see that? It only goes through so far.

We have to keep selecting faces. Right here where it says Faces, Body, we'll click on that. And then this time, hold Control on our keyboard.

Control, and we can select the bottom face and open it up. And again, hold Control and grab the right face and open it up. Now we should have all three faces open.

If we orbit around, we can see right through this thing. It's all hollow inside now. That's what we're going for.

So let's review this window before we wrap it up. We'll say Faces, Body. We should have three selected, which are all three circular faces of our T shape.

And Tangent Chain is selected. That's fine. Our Basic Shell Type is a sharp shell.

That is good. We don't want rounded edges. And our Inside Thickness is set to four and the Direction is Inside.

We'll go ahead and click OK. And there is the main portion of our clamp. Now before going on, there's some cool tools in Fusion to understand how this clamp works.

So first, let's go ahead to our top level and we'll activate that top component. So everything is now active. Now let's go ahead and hit the Save button, save our progress.

And now in the Inspect area, we'll pull that down and we're looking for something called Section Analysis. We'll click that. And we'll click that center plane that we use so often.

Click it one time. And now we're seeing a section. We might have to orbit around and we can see the result.

We'll notice that clamp that we've made is hollow inside and it allows the stem to go up inside. In fact, if we look down, we'll start to see our holes, our rings and our various stem components that everything nests inside all the way down. Ideally, if it doesn't, that's okay, but we can inspect and start to see how everything is working in a section view.

All right, with that, we do not need to click OK because it would save this section analysis and we don't need it currently. We'll go ahead and click Cancel and zoom back to home and we'll be ready for our next step.