About Replacing a Reference
You can replace a failed or missing reference of an active sketch with an alternative reference using the Replace command in the References dialog box or on the shortcut menu. In Assembly mode, you can select a new reference from a different model in the assembly, or from an external model. When you replace a reference, all dimensions and constraints associated with the replaced reference are recreated. The original dimension and constraint IDs are retained.
Keep in mind these points when replacing sketch references:
• The original and new geometric entities that define references do not need to be the same type. The following geometric entities can be used interchangeably to define references:
◦ Linear edges, linear curves, datum planes, datum axes, planar surfaces for distance and angle dimensions, and for parallel and perpendicular constraints
◦ Any geometry entity for a point on constraint
◦ Edges, curves, planes, axes, surface silhouettes for tangency constraints
◦ Edges, curves, surface silhouettes for Use Edge constraints, and so on
• When the original and new reference are not the same geometric type and are not interchangeable, the original dimensions and constraints are not recreated. New dimensions and constraints are created to position the sketch. This is similar to deleting a reference and adding a new reference in place of the deleted reference.
• When the original and the new reference are the same geometric type, the original dimensions and constraints may not be able to be created. For example, where the original reference is a vertical datum plane that defines a horizontal distance dimension and the new reference is a horizontal datum plane.