Lesson 4 – Modeling the Wheel Using the Revolve Command
Section II – Modeling Simple Parts 4.3 Modeling the Wheel
Notice that SolidWorks guessed that the centerline is the axis of revolution. Click the
centerline twice and notice how the PropertyManager changes.
Click the check mark to accept.
Step 24: Next, we will create a spacer to separate the inside and outside bearings.
Select the Front plane.
Click the Sketch icon on the Sketch tab in the CommandManager.
Click Convert Entities to bring the inside diameter of the wheel to the new sketch plane.
The new circle will be the outside diameter of the spacer.
Sketch a circle. This will be the inside diameter of the spacer.
Dimension the last circle.
Extrude the spacer by clicking FeaturesExtruded Boss/Base.
In Direction 1, use the pull-down menu to select Midplane.
Type the thickness of the spacer in D1.
Click the check mark to accept.
To see the cross-section of the wheel, click on the ViewDisplaySection View command on
the Main Menu or in the View Heads-Up toolbar. In the dialog box select the top or right plane
to see the cross-section preview.
Click the check mark to
accept. You should have
Figure 4.3 on your screen.
To get back the complete part,
click on the Section View
command again.
Step 25: Notice that you get a
different result if you do not use
Convert Entities. To see the
difference,
Right-click the Extruded
Boss/Base feature in the
FeatureManager design tree.
Click Edit Sketch.
Delete the circle created with
Convert Entities.
Click the check mark to
accept.
Figure 4. 3 – Skateboard Wheel