Discover how to create a 3D model of a scooter's rear wheel using various tools in the Fusion software. This tutorial provides a detailed step-by-step guide on how to construct the wheel, sketch the tire's profile, and give it a realistic rubber appearance.
Key Insights
- The tutorial commences with constructing the wheel of the scooter by selecting the offset plane that goes through the center of the scooter, expanding the wheel component, and renaming it to "Wheel Middle".
- Next, the tire's diameter is created using the Sketch Tool and given the name "Wheel Diameter." A sketch of the tire profile is then created on an offset plane named "Tire Profile Plane."
- Finally, the tire is made to resemble rubber by selecting the Appearance option from the Tire right-click menu and applying a hard rubber material from the Miscellaneous section.
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Our wheel one will be the rear wheel of the scooter. Let's start by creating that wheel's tire. So first, we will go up to the Construct menu and select Offset Plane.
I want to select the plane that goes right through the center of the scooter. I will click that plane. Offset Distance is zero, and then click OK.
Now, I will expand my window for the Wheel component and the Construction folder, and we'll have that plane one. Let's rename it, and we'll call it Wheel Middle. Enter should lock that in, and now we'll click off of it to make sure nothing is selected, and now we will create a sketch.
Create Sketch Tool. We want to create the sketch on the wheel middle, and we are looking for that center diameter circle. Select that tool and zoom in right around the back of the scooter in that hole we created right in the back of our scooter rail.
We'll click one time in the center, open up that circle, and type 200 for the diameter, and Enter. That looks pretty good. Now we can click Finish Sketch.
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Let's go back to our Home view. We'll notice that circle is centered right on our scooter, and it's centered right through that hole. We can select it and give it a name.
We're going to call this Wheel Diameter, and click Enter. Now we also need the profile of this wheel tire, so let's go ahead and draw that next. We're going to go to Construct, Offset Plane.
This time we will select the plane that's right in the front of our scooter and drag it back to that rear tire. We'll go to Front, and we can visually notice that it is centered right at minus 580, or we can simply type in minus 580, and Enter. Go back to our Home view, and give that plane a name.
We're going to call it Tire Profile Plane. Pretty straightforward. We'll click off of it to have everything unselected, and we will create a sketch again.
We will create the sketch by selecting the Tire Profile Plane. We'll zoom in a little bit to the origin. We'll grab our line command, click on the origin, and move our cursor straight up.
We'll type 15, and click Enter. So there it is. Now we want the circle tool, Center Diameter Circle.
Click on the top of our 15 millimeter line, and type in 30 for the diameter, and Enter. Now we need a couple of lines to wrap this up. We'll go back to our line command.
We'll zoom in even tighter, hover over the center of the circle, and move the cursor to the right. Notice that blue dashed line? It lets us know that we are still in alignment with the center of the circle. And as we get to the edge of the circle, it'll snap right to that edge perfectly.
We will click, and go up, and type in five for five millimeters. Let's repeat that for the left side. We'll start the line command, hover over the center, move straight to the left, click, go up five, and click Enter.
Now we need an additional line to connect these two dots. So line starting there, ending there. Now I want to use the trim command to remove everything we don't need.
We don't need this inside curve at the top, nor do we need it on this side. We also don't need this curve outside of our profile. When we're done, it should look something like this.
It's basically a D, a D shape, that's been rolled forward about 90 degrees. That looks pretty good, so we will click Finish Sketch. It's called Sketch 2 right now, so we'll select the word Sketch 2, and call it Tire Profile.
Now there are different ways to make the tire, but we're using all the different tools Fusion has to offer. So in this case, we will use the sweep command. Let's go back to our home view.
And under the Create menu, with nothing selected, we want to select Create and Sweep. Now the Sweep window has two inputs. The first is the profile.
So in our drawing, we can zoom in a little bit, hover over these profiles. We want to first select that tire profile sketch. We'll click to select the tire profile, and then we want a path.
We'll go down here to the Select button for Path, and we'll click that big circle, which is our wheel diameter circle, click that. And we'll notice it sweeps it all the way around and creates a new body for us. Now we can click OK.
So here we go, we see in our wheel component, we now have this Body 1. We can rename that to Tire, and click Enter. Now it doesn't look very tire-like right now because it's steel. We'd like a nice rubber tire.
So let's go ahead and update the appearance. Right here where it says Tire, we will select it and right-click on the word Tire. We will find the Appearance, select that.
And in the Appearance window, we can minimize Plastic if it's still open from before. And we're looking for Miscellaneous. Open that up and then scroll down.
There's one called Rubber. And then we want Rubber-Hard. It's the first rubber we have.
Drag and drop it onto the tire body, and let go. And there it is, we've got a nice rubber tire.
