Strategy: Identifying Relationships that Affect Shape Changes

As you build your part, consider the relationships you are creating as these relationships can freeze a shape change or introduce an unwanted shape change. Be particularly aware of the following relationships:

• parent/child relationships—If you move a parent, the child moves with it.

• dimension relations—If you define relations between your part’s dimensions and independent dimension as a design variable, the dependent dimension changes in accordance with the relation you established.

• alignment—If you align an aspect of your part with another aspect of your part and use a design variables in such a way that the aspect you used for alignment disappears, your part fails to regenerate.

• declared notebook relations—If you use a notebook when building your part or assembly, Creo Parametric defines relations between the aspects of the part or assembly you declare to the layout and the associated aspect of the notebook.

For example, if you declare the length of a part to the notebook, Creo Parametric defines a relation tying the part’s length dimension to the notebook’s length dimension. The layout dimension is the independent dimension.

Because Creo Parametric treats any part dimension you declare to a notebook as dependent, you cannot select the dimension as a Creo Simulate design variable without first undeclaring it.

• patterning and mirroring—Patterning and dependent mirroring link the movements of multiple geometric entities. If you use these techniques, you will not be able to move geometric entities individually. Further, you may introduce unexpected topology changes or Creo Simulate may eliminate a geometric entity altogether. Before using these techniques, consider how you may want the shape of your part to change during sensitivity or optimization studies.

Because it is fairly easy to set up unintentional relationships while building a part, you should perform the following checks before using Creo Simulate:

• Use the Info > Parent/Child command to review parent-child relationships and reassign dimensions when necessary.

• Before you enter Creo Simulate, select the Edit > References > Reroute Feat > Ref Info command to display the reference information window. Review the data in this file to determine each of the dimension references. When necessary, redefine the dimensioning scheme or redesign the feature.

• Select the feature in the Model Tree, right-click, and select Redefine or Edit References to cycle through each of the dimension references. When necessary, redefine the dimensioning scheme or redesign the feature.

• Test your design by animating the shape changes using Shape animate the model in the global sensitivity study prior to starting your design study. If you see any problems or Creo Parametric fails to regenerate the part, redesign the part in a way that prevents conflicts.

• Add cosmetic features, rounds, and chamfers later in the model's history, and avoid using these features as references for other features.