About References
You can add valid references to create, dimension and constrain geometry in these ways:
• Use the References dialog box.
• After activating a sketch tool, press ALT, select one or more background entities, and right-click and choose Add references from the shortcut menu.
To automatically add selected geometric entities as references before activating a sketch tool, set the sketcher_auto_create_references configuration option to yes or click the Automatic reference creation from selected background geometry check box in the Sketcher area of the Creo Parametric Options dialog box.
You are prompted to create references in the following situations:
• When you create a new feature, the References dialog box opens. Select a perpendicular surface, edge, intent edge vertex, datum reference or composite curve relative to which the section will be dimensioned and constrained.
• When you redefine a feature that has missing references.
• When you do not have enough references to place a section.
When working with a section, if the sketch reference becomes invalid or is removed, you can update or remove the failed or missing reference. Additionally, you can replace the failed or missing reference with an alternative reference. You can delete, update, or replace a failed reference, even if the reference belongs to an external model. Use the Undo or Redo commands when resolving failed or missing references.
When you delete, update, or replace a reference using the References dialog box, the sketch is not updated automatically and you can choose to update the sketch.
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The sketch is updated automatically if you replace a reference using the Replace command in the References dialog box or in the shortcut menu.
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The Solve option in the Reference dialog box is available only if there are no failed or missing references.