This document provides instructions for creating a custom wheel design in SolidWorks. The design uses revolved features to create the wheel rim and lug nuts. Cut extrusions create the spokes by cutting away from the solid wheel rim. A circular pattern duplicates the cut features to create multiple spokes around the wheel. Dimensioning and fillets are added to complete the wheel profile.

1. 1
Custom Wheel - SolidWorks Tutorial
This is a simple wheel design to shown you how it's done. The main thing that you want to do is to get the main concepts
for each step: the revolves, cut extrude at a specified direction, circular patterns, and cut revolve. Then, explore and
create your own profiles to create your own wheels. If you are really proud of your work, I would love to see it. Just email
me at info@AboutSolidWorks.com.
To start out, open a new part document. I used mm for my units. Start a sketch on the Front plane and draw the following sketch. The
best way is to draw the basic shapes without the fillets and dimension it. Create about a 35mm vertical Line directly below the Origin
and going downward. Continue with a second line about 9mm at 135 degrees, down and to the right. The third line continues down
about 116mm, but at a sharper angle, just don’t let it lock in as vertical. Next, about a 62 mm line to the left and make it perpendicular
to the third line. Then make about a 69 mm horizontal line to the right. The next line goes up about 32mm and to the right at about 60
degrees. And another one up and to the left about 120mm. This line will be parallel to the similar line shown to the left of it in the
sketch (the third line). Now up about 13mm and to the left again, this one is at 135 degrees and is parallel to the second line. From
here, create a vertical line which ends a little higher than the first one started but below the Origin. Then, finally close the loop.
Create one more line, a horizontal Centerline through the Origin. Then, add the dimensions below.
Then, add your fillets. Break the sharp corners with a 6 radius fillet. I did this in five places. I also turned off the sketch relations so
that you could see the sketch better. (Pull down the "View" menu and uncheck Sketch Relations). Exit the sketch.

2. 2
With the sketch selected in the FeatureManager design tree, click the Revolved Boss/Base button from the Features
CommandManager tab, or pull down the "Insert" menu and pick Boss/Base - Revolve.
In the graphics area, pick the centerline of the sketch that goes through the origin. In the Revolve PropertyManager, make sure that the
Angle is set to 360 and click OK.
That's the first step to creating the wheel. Next, you are going to prepare for your cut that will reveal the spokes. To do this, create a
new sketch on the Front plane, and sketch the two centerlines as shown below. Make sure that the angled centerline in coincident to
the front edge line as shown by the black endpoint.

3. 3
Exit the sketch. Now you are going to create a new plane by copying the Right plane at the endpoint of your angled centerline. To do
this, in the FeatureManager design tree, click on Right Plane so that it is shown in the graphics area. Then, hold down the Ctrl key
and drag the plane in the graphics area to the right and let go of the mouse button. In the graphics area, pick the endpoint of the angled
centerline as shown below. Once the preview is correct, click OK in the Plane PropertyManager.
Start a sketch on the new plane that you just created. Pick the the outside circle and click Convert Entities from the "Sketch" toolbar
in the CommandManager, or pull down the "Tools" menu and pick Sketch Tools - Convert Entities. Then create a small circle at the
lower endpoint of the angled centerline from the previous sketch. Add two tangent angled lines, and then trim everything up as shown
below. Right click on the top arc and pick Select Midpoint from the menu. Hold down the Ctrl key and pick the centerpoint of the
small arc. In the Properties PropertyManager, pick the Vertical relation and click OK. Finally, add the two dimensions shown and
exit the sketch.
With the sketch selected in the FeatureManager design tree, click the Extruded Cut button from the Features CommandManager tab,
or pull down the "Insert" menu and pick Cut - Extrude.

4. 4
In the Extrude PropertyManager, set the End Condition to Through All. Click in the Direction of Extrusion box. Then, pick the
angled centerline from the graphics area, and then click OK.
Start a sketch on the Front plane and draw the sketch below. Make sure that the left most vertical line is Coincident to the Origin and
the rightmost vertical line is Collinear to the right edge of the part, as shown below. Exit the sketch.
With the sketch selected in the FeatureManager design tree, click the Revolved Cut button from the Features CommandManager tab,
or pull down the "Insert" menu and pick Cut - Revolve.
In the Cut-Revolve PropertyManager, click in the Axis of Revolution box. Then, pick the bottom horizontal line in the sketch. Make
sure the Angle is set to 360 and then click OK.
Now, in the next step, you will create a circular pattern to create the rest of the spoke and lug nut holes. All you have to do is click the
Circular Pattern button from the Features CommandManager tab, or pull down the "Insert" menu and pick Pattern - Circular.

5. 5
In the CirPattern PropertyManager, click in the Features to Pattern box and then, in the flyout design tree, pick the Extrude and the
Cut-Revolve. In the graphics area, pick the centerline of the part. Make sure that the Angle is set to 360 and set the Number of
Instances to '5'. Click OK.
This is where you can play with the number of spokes by changing the Number of Instances. Equal spacing is easier to do than
trying to calculate the angles manually.
Lastly, start a sketch on the Front plane and draw the following sketch. Make sure that the right side is Collinear to Plane1 and the
top line of the sketch is Collinear to the bottom edge of the part.

6. 6
Then, add your fillets. Start with the largest fillets first and work your way down. I also turned off the sketch relations so that you
could see the sketch better. (Pull down the "View" menu and uncheck Sketch Relations). Exit the sketch.
With the sketch selected in the FeatureManager design tree, click the Revolved Boss/Base button from the Features
CommandManager tab, or pull down the "Insert" menu and pick Boss/Base - Revolve.
In the graphics area, pick the horizontal centerline of the sketch that goes through the origin. In the Revolve PropertyManager, make
sure that the Angle is set to 360 and click OK.
That's it!