SolidWorks 2010 Bible

Chapter 16: Modeling in Context

FIGURE 16.22

Selecting a configuration

Tutorial: Working with a Layout

In this tutorial, you will use regular assembly sketches to lay out and build a tooling die.

1. Open the assembly from the CD-ROM named Chapter 16 tutorial layout
   start.sldasm. Notice that three layout sketches and some of the parts have been
   added already. The existing parts are virtual components, saved inside the assembly.


2. Click Add New Part on the Assembly tab of the Command Manager. The cursor
   appears with a green check mark, and in the lower left corner, the Task Bar prompts you
   to select a plane on which to place the Front plane of the part. A sketch will automatically
   be opened on that plane. Click the Front plane of the assembly.


3. Click the Corner Rectangle sketch tool from the Sketch toolbar. Create a rectangle
   from the two corners indicated in Figure 16.23. It may be helpful to bring the model into
   a Front view before drawing these rectangles.


4. Extrude the rectangle using the Up To Vertex end condition for both Direction 1
   and Direction 2. Select sketch endpoints in the Plane Depth Layout sketch for both
   directions so that the new plate matches the other existing plates.

Be careful not to click on model faces, edges, or vertices when creating these depth refer-
ences. Make sure that all your references stay in the sketch.

5. Click the Exit Edit Part icon in the ConfirmationCorner, the upper-right corner of the
   SolidWorks graphics window. Right-click on the new part in the FeatureManager and
   select Rename Part. Rename it Plate4. You can also use the Windows standard method of
   slow double-clicking to rename parts. The ^Chapter 16 tutorial layout start part of the name
   is automatically added. Assign a material from the Appearances tab for the new plate.