SolidWorks 2011 Parts Bible - Matt Lombard [167]
In This Chapter
Using Rollback to look at the results of the design tree
Reordering features in the design tree
Reordering all features as a folder
Selecting items using the Flyout FeatureManager
Summarizing best practice suggestions for modeling parts
Applying evaluation techniques to plastic parts and complex shapes
Diagnosing errors
Editing and evaluation techniques tutorial
When you use CAD programs, you typically create a part once but edit it many times. Design for change is at the core of most of the modeling work that you will do in SolidWorks, and deletion is not an editing option.
The initial stages of modeling are the most crucial. This is when you set up parametric relations between the features and sketches that form the foundation for an assembly or complex part. For this reason, editing often quickly turns into repair. Granted, some changes are simply unavoidable, but a thorough knowledge of editing — and repairing — can help you to understand the how, what, and why of modeling best practice.
This chapter starts with some very basic concepts of editing, which you may have picked up if you have been reading this book from the beginning. It also contains a summary of part modeling best practice techniques and a set of model evaluation tools that can help you evaluate the manufacturability and aesthetic properties of parts. I have included these evaluation tools in a chapter on editing because the create-evaluate-edit-evaluate cycle is one of the most familiar in modeling and design practice.
Using Rollback
Rolling back a model simply means looking at the results of the design tree up to a certain point in the model history. In SolidWorks, you can actually change history — that is, you can change the order in which operations are completed. The order in which you create features is recorded, and if you change this order, you get a different geometric result.
You can use several methods to put the model in this rolled-back state:
• Dragging the Rollback bar with the cursor.
• Right mouse button (RMB) clicking and selecting one of the Rollback options.
• Editing a feature other than the last one in the design tree. (SolidWorks rolls back the model automatically.)
• Choose Tools⇒Options⇒FeatureManager⇒Arrow key navigation to control the Rollback bar with the arrow keys.
• Saving the model while editing a feature or sketch, and then exiting the model. When the part is opened again, it is rolled back to the location of the sketch that was being edited.
• Pressing Esc during a long model rebuild. This method is supposed to roll you back to the last feature that was rebuilt when you pressed Esc; however, in practice, I have rarely seen it do this, and it usually rebuilds the entire model anyway.
Using the Rollback bar
The Rollback bar, which typically appears at the bottom of the FeatureManager in SolidWorks part documents, enables you to put the part into almost any state in the model history. This is not the same as the Undo command, but is the equivalent of going back in time to change your actions, and then replaying everything that you did after that point. Figure 12.1 shows the Rollback bar in use. Notice how the cursor changes into a hand icon when you move it over the bar.
FIGURE 12.1
Using the Rollback bar
Understanding consumed features
When you use a sketch for a feature such as a Sketch Driven Pattern, the sketch is left in the design tree, in the place where it was created. However, most other features, such as extrudes, consume the sketch, meaning that the sketch disappears from its normal order in the FeatureManager and appears indented under the feature that was created from it. Consumed sketches are sometimes also referred to as absorbed sketches.
Examining the parent-child relationship
In genealogical family tree diagrams, the parent-child relationship is represented with the parent at the top, and the children branched below the parent. In SolidWorks, parent-child relationships are tracked differently. Figure 12.2 shows the difference