SolidWorks 2011 Parts Bible - Matt Lombard [259]
5. Extrude the second rectangle to about two-thirds of the depth of the first rectangle.
Note
Notice that the Merge option was not changed from the default setting (On) for the second extrude, but because the first extrude was hidden, the second extrude did not merge with it. Be careful of subsequent edits to either of the features if the first body is shown, because this may cause the bodies to merge unexpectedly. In this tutorial, the bodies are later merged intentionally. Ideally, what you should do is deselect the Merge option of the second extrude.
6. Shell out the second extrusion by removing two adjacent sides, as shown in Figure 19.25. One of the sides is the top and the other is the shared side with the hidden body. The body that should be hidden at this point is shown as transparent in the image for reference only. The body was made transparent to make it easier to select the face of the second body.
Figure 19.25
Shelling two sides of a block
7. Show the first body either from the Solid Bodies folder at the top of the tree or from the RMB menu of the first solid feature in the tree.
8. Shell the bottom side of the first body, so that the cavities in the two bodies are on opposite sides.
9. Combine the two bodies using the Combine tool you can find by choosing Insert⇒Features⇒Combine. This feature is also available via the RMB menu in the solid body folder. Select the Add option and select the two bodies. Click OK to finish the feature. Figure 19.26 shows the finished part.
Figure 19.26
The finished part
Splitting and patterning bodies
This tutorial guides you through the steps to delete a pattern of features from an imported body, separate one of the features, and then pattern it with a different number of features. This introduces some simple surface functions in preparation for Chapter 20. Follow these steps:
1. Open the Parasolid file from the DVD called Chapter 19 – Bonita Tutorial.x_t.
2. Using the Selection Filter set to filter Face selection (the default hotkey for this is X), select all the faces of the leg. You can use window selection techniques to avoid clicking each face.
3. Click the Delete Face button on the Surfaces toolbar, or access the command by choosing Insert⇒Face⇒Delete from the menus. Make sure that the Delete and Patch option is selected. The selected faces and the Delete Face PropertyManager should look like Figure 19.27. Click OK to accept the feature.
Figure 19.27
The Delete Face PropertyManager
4. Repeat the process for a second leg, leaving the third leg to be separated from the rest of the part and patterned.
5. After the two legs have been removed, click the outer main spherical surface, and then choose Insert⇒Surface⇒Offset from the menus. Set the offset distance to zero. Notice that a Surface Bodies folder is now added to the tree, near the top.
Tip
A zero distance offset surface is frequently used to copy faces.
6. Hide the solid body. You can do this from the Solid Bodies folder, from the FeatureManager, or from the graphics window.
7. Hiding the solid leaves the offset surface, and there should be three holes in it. Select one of the edges of the hole indicated in Figure 19.28 and press the Delete key. The Choose Option dialog box appears. Select the Delete Hole option rather than the Delete Feature option. The Delete Hole operation becomes a history-based feature in the model tree. Before moving on to the next step, remember that you may need to turn off the Selection Filter for faces.
Figure 19.28
Using the Delete Hole option
Note
Delete Hole is really a surface feature called Untrim. Untrim is discussed more in Chapter 20, but you can use it to restore original boundaries to a surface.
8. Once you delete the hole from