Introduction to SolidWorks

Lesson 7 – Modeling the Truck
Section III – Modeling Complex Parts 7.3 Modeling the Truck

 Click Normal To again.

 Click Sketch on the Sketch menu and then Convert Entities.

 Use the command Convert Entities on the Sketch tab to add the edge of the second

cylinder to the new sketch.

 Click the check mark to accept.

 Click Extruded Boss/Base and select Blind. Type 0.75 inch for the length D1.

 Uncheck Merge result on the properties menu.

 Click the check mark.

 Notice that a new folder named Solid Bodies is now visible in the FeatureManager

design tree. Open the folder and verify that you have two bodies. You have a

SolidWorks Multibody model.

 Select the circular edge of the third cylinder and click InsertAnnotationsCosmetic

Thread. Select ANSI Inch standard and 3/8-16 UNC thread. The cosmetic thread can be

seen on the end face.

Step 45: Change the Appearance of the surface to simulate threads.

 Right-click the surface of the body with the Cosmetic Threads.

 Click the Appearances icon.

 Click Face. The PropertyMenu appears at the left side of the screen and the

Appearances/Scenes appear at the right side.

 Expand Appearances (color), and Miscellaneous.

 Click Pattern.

 Click the screw thread pattern.

 Click the Mapping tab to adjust the threads.

 Experiment with Rotation and Mapping Size.

Step 46: Mirror the axle across the Right plane.

 Click InsertMirror/PatternMirror.

 Select the Right Plane as the Mirror Face/Plane and the three extrusions as the

Features to Mirror. See Figure 7.1.

 Click the check mark to accept.

 Notice that there are only two bodies. The Mirror command merged two cylinders when

they were copied from the other side. The Mirror command does not work with

multibodies.

 To correct, right-click the Mirror feature and select Edit Feature.

 Delete the threaded portion of the shaft from the Features to Mirror.