Troubleshoot Shape Change Problems
When you review or animate your model, you may find that the design variables change the model's shape in ways you did not anticipate. If you encounter this situation and cannot determine why the shape is changing unexpectedly, look for conflicts or problems with the following:
• Relations—Problems with relations are a common source of unexpected shape changes. If you use relations to make dimensions move relative to one another, review the relations or look at the Pro/Program file. Try to locate errors in the relations or conflicts between relations. For more information on Pro/Program, see the Part Modeling area of the Creo Parametric Help Center.
• Creo Parametric parameters in multiple relations—Creo Parametric parameters that appear in multiple relations can cause unexpected shape changes. Review all the relations associated with the Creo Parametric parameter to make sure you understand their implications. Try to locate relations that you may have forgotten about.
• Parent/child relationships—Child dimensions can move in unexpected ways or freeze depending on the changes in the parent dimension. Thus, in moving a parent feature, you may see a child change shape or position. If you suspect this problem, review the parent/child relationships for your part and redimension the part if necessary.
• Dimensions based on datum planes or center lines—You can use datum planes or center lines to position features in your part. Positioning dimensions of this sort may freeze feature movement. Among other things, this can result in size changes that translate feature position rather than maintain feature centering.
If you suspect this problem, consider adding a design variable to move the positioning dimensions as well as the sizing dimensions. As an alternative, you may want to redimension your part or redefine the relations.
• Sketcher assumptions — When you dimension a part, Creo Parametric's sketcher makes certain assumptions about undimensioned areas of your part. These assumptions can result in unwanted part movement.
For example, if you are designing an L-bracket and dimension the width of only one leg, the sketcher assumes an identical width for both legs. Should you create a design variable for this dimension, Creo Simulate will move the width of both legs instead of just the leg with the design variable.
If you suspect that the problem is the result of sketcher assumptions, add extra dimensions to counteract the sketcher assumptions.