Creating Wheel Spokes with Sketch Reuse and Modeling Tools in Fusion

Now let's connect our hub and rim with some spokes. To do that, we want to recycle some of the work we've already done. Let's go ahead and find Sketches under our Wheel component, and we're looking for the hub and rim sketch.

Let's go ahead and unhide it by clicking the eye icon, and let's go ahead and right-click and say Edit Sketch. You will draw a big window around everything in the sketch, and then select right-click and Copy. We're copying all those elements.

Once we've copied them, we can click the Finish Sketch button. We can hide that hub and rim sketch again, and now we want to start the New Sketch command. So New Sketch, Create Sketch, and the construction plane we want is the tire profile plane again.

Now we can right-click and select Paste. No need to move this anywhere. We will simply click OK.

We'll zoom in nice and tight, and we'll add a few lines to the lines that we've already pasted. We'll go to the Line tool, and we'll go down to the bottom triangle first, the bottom left side right here. We will click, and we will go to the right.

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Two millimeters. We'll click, and then we'll type 2, Enter. Let's do the same thing for the top.

We'll find that corner of the triangle, Line command, click, move our cursor to the right, type 4 this time, and Enter. So that finds two points for us. I'm going to click the Line command again and click the top point, go down to the bottom point, and click again.

That gives us a nice tapered line right there. We'll hit Escape on our keyboard and delete these lines. We don't need them anymore.

Click Delete, click Delete, and we can also trim the lines we don't need. We'll go to the Modify, Trim, and we don't need the portion above the triangle right there or below the triangle right here. Click and trim those lines away.

And oops, I clicked the wrong side. I'll click Undo. And do Trim again right there.

Okay, that looks pretty good. Now we have just the line that we want. Now let's mirror it across.

To do that, we'll start the Line command again, and we'll connect the triangle tips together. Click, click, and we want to select that line we just drew and turn it into a construction line. So I'll select it one time, right-click, and select Normal Construction.

Now I can go to the, with nothing selected, go to that Mirror command. Objects, we'll select that tapered line. Mirror line, we will select that construction line.

And click OK. So that mirrors that line across. Now we can trim the lines we don't need.

We'll trim out the hub lines we don't need, those two. And we'll trim out the rim lines we don't need, those two. We just want this shape in the middle.

And oops, I misclicked again. I will Undo, Trim command, and get rid of the line on the right. We're just left with that portion in the middle.

Now we can also delete out the remaining lines from that first sketch that we no longer need. A few more lines. This one and the one on the right.

We're left with that sketch of just the inside portion. And we will click Finish Sketch. Now it's called Sketch 4. We'll click on that one time and give it a new name.

We'll call this Spoke Profile. Let's go back to our Home view and see the result. We have this profile that's kind of right here between the rim and the hub.

So there it is. Now let's turn it into some 3D geometry. So again, mine didn't take on the name.

So I'll click again and I'll call it Spoke Profile. There we go. Ah, it doesn't want to take.

We might have to rename it at the end of our project. Let's go ahead and go to the Create tab. And we're looking for the Extrude command.

We'll go to Extrude. And the direction this time, instead of one side, we'll change that to Symmetric. And the distance will be 2. Now by default, it wants to do Cut.

That's not what we want. We want to make this a new body. It's a new body.

Once that looks okay, we got Distance 2, Symmetric, New Body. We'll click OK. So there is our first spoke.

Let's see if we can rename things again. The spoke is called Body 4. We'll call this Spoke. And the sketch that created that spoke, we'll call that Spoke Profile.

Okay, looks like we're good now. We have that spoke. We want to select it and we want to rotate it a little bit.

We'll right-click and say Move Copy. Move Copy. Now we want to look directly at it.

We want to go to the front view. And in Fusion, this is called the Pivot. It's a little tool that lets us rotate, move, and scale.

We don't want to pivot from this point. We're going to come up to our Move Copy menu and click the Set Pivot button. I want to click right in the center of the center of our hub.

And to do that, we kind of hover over that hub circle, and that sets our pivot. Once we're happy with the pivot, we want to click this green checkbox in the Move Copy window, and that sets our pivot. Now we can rotate.

And we want to select the Z angle of 5 and then click OK. We've simply rotated it 5 degrees. Let's repeat that.

It was a lot of fun. We'll do it again. We will select the spoke, then right-click and select Move Copy.

We want to change our pivot again. We'll do the Set Pivot tool. Click right in the middle of that hub.

It's got to be perfectly centered. Click, and now click the green checkbox. This time, before we do any rotation, it's important to first check the Create Copy.

So Create Copy is checked. And now for Z angle, I can do minus 10. And we'll notice that creates a copy and rotates it back minus 10 degrees.

We get both sides of our spoke. And we'll click OK. Now that looks pretty good, but we'd like to make that all one item.

We can do that by going to the Modify rollout and selecting Combine. We'll click our first spoke, our second spoke, and click OK. So there it is.

Now we just have one spoke. Now we'd like to add something in the middle. Right now, it's just going to open inside.

So let's add some more geometry. We're going to start a new sketch. So again, I select nothing.

Nothing is selected. And I'm going to go up to the Create Sketch. Where do I want to place this sketch? I want to place it on the wheel middle.

So click Wheel Middle. It's going to zoom me over to that origin. That's OK.

I'm going to go back to my wheel. And let's try another tool here. In the Create window, you can pull that down.

And there's something called Project, Include, and then Project. Now we want to move our cursor around until we find the inside face of the spoke. There's one on the right, one on the left.

We want to click Ball. So I'll click one time here, one time there. I should get two blue lines.

If I misclick and get something else, not a problem. I can hold Shift on my keyboard and double-click again. Click again on that misclick, and it goes away.

All right. Now we've got those two lines. And we'll click OK.

Now we want to connect those lines. We're basically making a triangle. But the bottom of the triangle is rounded.

We're going to go to Create and look for Center Diameter Circle. Click right in the center of our hub. And then go and click a second time on the end of that line right there.

Now that created a whole profile, shaded in everything inside the circle. We don't want to do that. We want to finish by going to the Trim command and trimming out the outside.

And we're left with just a shaded portion inside that spoke. I'm going to orbit around so you can see the result that we're going for. It's a triangle with a rounded bottom.

1. And with that completed, we can click Finish Sketch. Let's try to give that a name.

And we'll call that Spoke Inside. OK. There we go.

Now we want to turn that into 3D geometry. We'll use our favorite tool, the Extrude command. We want to select that spoke inside as our profile.

And our direction, again, will be symmetric. We can grab one of these grip arrows and start pulling it out. What does Fusion want to do? It wants to cut.

We don't want that. We want to select New Body again. And the distance is 10 millimeters.

Once we have that, we'll click OK. So that creates a new body. We have our spoke.

And then inside the spoke is just a random body with a number. We'll rename it. And we'll call it Spoke Inside.

Now we'll click away so nothing is selected. And we can use our Combine tool again. Under Modify, we'll find Combine.

We'll start by clicking the spoke. And then click the spoke inside portion. And click OK.

And that creates one spoke with everything that we've modeled so far. Pretty cool, right? Now we need more than one spoke. So let's go ahead and create a pattern to create all of our spokes.

Under the Create tool, we want to find Pattern. And we're looking for Circular Pattern. Now the object type is Bodies.

And we want to select our one spoke. We'll have one selected. Now we want to select the axis.

Now we can pick anything really here. We can just pick the tire. That'll probably be fine.

We'll select the tire. And the quantity, it'll be set to maybe 3 by default. We'll change that to 6. And then click OK.

And now we see all of our spokes here. All of those bodies within our one wheel component.