Display/Delete Relations PropertyManager

To open the Display/Delete Relations PropertyManager:

Click Display/Delete Relations (Dimensions/Relations toolbar) or Tools > Relations > Display/Delete.

Relations

When you select a relation from the list, the sketch entities are highlighted in the graphics area, along with the icons representing that relation. If Sketch Relations (View > Hide/Show > Sketch Relations) is selected, all icons are displayed, but the icons for the highlighted relation appear in a different color.

Example of highlighted relations:

	Filter	Specifies which relations to display. Select one of the following: All in this sketch Dangling Over Defining/Not Solved External Defined In Context Locked Broken Selected Entities Displays the names of entities that you select in the sketch.
	Relations	Displays existing relations based on the selected Filter. When you select a relation from the list, the names of the related entities are displayed under Entities and the sketch entity is highlighted in the graphics area. The status of external references is displayed the same as in the FeatureManager design tree.
	Information	Displays the status of the selected sketch entity. If the relation was created within the context of an assembly, the status can be Broken or Locked.
	Suppressed	Suppresses the relation for the current configuration. The name of the relation turns gray and the Information status changes (from Satisfied to Driven, for example).
	Undo last relation change	Deletes or replaces the last action.
	Delete and Delete All	Deletes the selected relations or deletes all the relations.
	Repair All Dangling	Fixes the dangling relations. Available only for 2D sketches. Does not fix dangling relations that have external references. You must manually repair these dangling relations.

Entities

	Entities used in the selected relation	Entity Lists each selected sketch entity in Relations. Status Displays the status of the selected sketch entity, such as Fully Defined, and Under Defined. Defined In Displays the location where the entity is defined, such as Current Sketch, Same Model, or External Model. Information for external entities in assemblies: Entity Displays the entity name for sketch entities in the Same Model or External Model. Owner Displays the part to which the sketch entity belongs. Owner and Assembly Displays the name of the top-level assembly where the relation was created for sketch entities in an External Model.
	Replace	Replaces the selected entity with another entity. In the graphics area, select an entity for Entity to replace the one selected above, and click Replace. If the replacement is not appropriate, the status is Invalid.
	Find Replacement	Searches for a replacement for a dangling relations. A message appears if a replacement is not found. Available only for 2D sketches.
	Undo last relation change	Undoes the last Replace action.

Configurations

For models with multiple configurations, you can apply the selected relations to This configuration, All configurations, or Specify configurations. If you select Specify configurations, select configurations in the Configurations list. Click All to select all the configurations in the list. Click Reset to reset the selections to the original settings.

Options