SolidWorks 2011 Parts Bible - Matt Lombard [185]
25. If you right-click Extrude1 and select Parent/Child again, the Shell feature is no longer listed as a child.
26. Delete Extrude1, and when the dialog box appears, press Alt+F to select Also Delete Absorbed Features.
27. Edit the Shell feature and select the large end of the loft. Exit the Shell feature. The results up to this step are shown in Figure 12.42.
Figure 12.42
The results up to Step 27
28. Drag a window in the design tree to select the four fillet features. Then right-click and select Add to New Folder. Rename the new folder Fillet Folder.
29. Click the Section View tool, and create a section view using the Front plane.
30. Reorder the Fillet folder to after the Shell feature.
31. At this point, you should notice that something does not look right. This is because creating the fillets after the Shell causes the outside fillets to break through some of the inside corners. The fillets should have failed, but have not, as shown in Figure 12.43.
32. Choose Tools⇒Options⇒Performance, and select Verification on rebuild. Then click OK to exit the Performance menu and press Ctrl+Q. The fillets should now fail.
33. Click Undo to return the feature order to the way it was.
34. Save the part.
Figure 12.43
Fillets that should have failed
Summary
Working effectively with feature history, even in complex models, is a requirement for working with parts that others have created. When I get a part from someone else, the first thing that I usually do is look at the FeatureManager and roll it back if possible to get an idea of how the part was modeled. Looking at sketches, relations, feature order, symmetry, redundancy, sketch reuse, and so on are important steps in being able to repair or edit any part. Using modeling best practice techniques helps ensure that when edits have to be done, they are easy to accomplish, even if they are done by someone who did not build the part.
Evaluation techniques are really the heart of editing, as you should not make too many changes without a basic evaluation of the strengths and weaknesses of the current model. SolidWorks provides a wide array of evaluation tools. Time spent learning how to use the tools and interpret the results is time well spent.
Chapter 13: Using Hole Wizard and Library Features
In This Chapter
Working with the Hole Wizard
Exploring library features
Creating library features
Examining Dissection feature
Working with library features tutorial
The SolidWorks Hole Wizard is an automated tool that helps you place standard-sized holes in parts
Library features are user-defined, and you might use them in a similar way to how you use the Hole Wizard. They can be automated to some extent, and can make use of configurations. This chapter contains the information you need to decide how to implement and use the Hole Wizard and library features in your work.
Using the Hole Wizard
The Hole Wizard enables you to place holes for many types of screws with normal, loose, or close fits. You can create Hole Wizard holes as assembly features in an assembly or as features in individual parts that are built in the context of an assembly using the Series Hole functionality. This tool is called a wizard because it guides you through the process step by step. A summary of the workflow of creating a Hole Wizard hole is as follows:
1. Pre-select the face to put the holes on, although this is not required. Versions after SolidWorks 2010 no longer require pre-selection to avoid 3D placement sketches; the Hole Wizard uses 2D sketches by default.
2. Select the type of hole; for example, counterbored, countersunk, drilled hole, tapped hole, pipe tap, or legacy.
3. Set the standard to be used, such as ANSI (American National Standards Institute) inch, ANSI metric, or ISO (International Organization for