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FIGURE 12.2

Different interpretations of the structure of parent-child relationships

You can display the parent-child relations between SolidWorks features, as shown in Figure 12.2, by right-clicking on any feature and selecting Parent/Child. This helps you determine relationships before you make any edits or deletions because you can see which features will be removed or go dangling (lose their references).

When SolidWorks puts the child feature at the top, it is, in effect, turning the relationship upside down. In the SolidWorks FeatureManager, the earlier point in history is at the top of the tree, but the children are listed before the parents. The SolidWorks method stresses the importance of solid features over other types of sketch or curve features.

For example, you create an extrude from a sketch, and, therefore, the sketch exists before the extrude in the FeatureManager. However, when you create the extrude, SolidWorks places the sketch underneath the extrude. This restructuring can become more apparent when a sketch (for example, Sketch1) is created early in the part history, and then not used to create a feature (for example, Extrude5) until much later. If you roll down the FeatureManager feature by feature, you arrive at a point at the end of the design tree where Extrude5 appears and Sketch1 suddenly moves from its location at the top of the tree to under Extrude5 at the bottom of the tree.

This scenario may cause a situation where many sketches and other features that are created between Sketch1 and Extrude5 are dependent on Sketch1, but where Sketch1 suddenly appears after all these other features. This can be difficult to understand but is key to effectively editing parts, especially parts that someone else created.

The main point here is that SolidWorks displays many relationships upside down. You need to understand how to navigate and manage these history-bound relationships.

One way to get around difficulties in understanding the chronological order of features when compared against the relationship order of features is to roll back a model tree item by item. This can help you sort through the issues. Also remember that from SolidWorks's point of view, the solid feature is the most important item in the tree and is what the rest of the items in the tree support. SolidWorks has made the solid features easily visible and accessible in the tree.

Rolling back features with multiple parents

Take an example such as a loft with guide curves. If you create the guide curves first, and then you create the loft profiles by referencing the guide curves, the loft automatically reorders these sketches when they display under the loft feature such that the profiles are listed in the order in which they were selected, followed by the guide curves in the order in which they were selected. This is shown in Figure 12.3. This restructuring can be confusing if you want to go back and edit any of the relationships between the sketches. You can find this example on the DVD with the filename Chapter 12 Loftwgc.sldprt.

FIGURE 12.3

Multiple parents and sketch reordering

Note

In this example, the two guide curves were created as part of a single sketch, and the SelectionManager was used to select them as individual open curves. This is why the Guide Curves sketch is represented with the contour symbol rather than a regular sketch symbol.

Viewing consumed features in their original order

If you want to view consumed sketches in their original order — for example, the sketches in the loft feature in Figure 12.3 — you must first expand the feature by clicking the plus (+) symbol next to it so that you can see the consumed sketches, and then roll back between the feature and the first sketch. At this point, a warning message appears, stating that the sketches will be temporarily unabsorbed during editing. You can then move the Rollback bar again to show the sketches.

This maneuver can become complicated when you have two sketches absorbed by a