Error Message - Dangling Geometry

Potential Error Messages

  • This sketch contains dimensions or relations to model geometry which no longer exists. Consider:
    • Deleting the dangling sketch entities (shown dashed and in dangling color).
    • Editing the model to restore the missing model geometry.

Potential Reasons for These Error Messages

Dimensions or relations reference something that no longer exists or is unresolved.

Dangling Dimension Example

Dangling dimension

Potential Solution:

Dimension repaired by dragging.
Dangling Relation Example

Dangling relation

Potential Solution:

Relation repaired with the Display/Delete Relations tool.

Potential Fixes

Begin by repairing the first feature with an error in the FeatureManager design tree, then work down through subsequent errors. Dangling dimensions and relations display in a different color (default: brown) than the resolved sketch entities.

To set the color for dangling dimensions, click Tools > Options > System Options > Colors. Select Dimensions, Dangling in Color scheme settings. Click Edit, select a color, then click OK.

Dimensions

Drag the dangling handle and reattach it to the correct sketch entity. If you attempt to reattach it to an invalid location, the pointer displays the symbol.

Relations

Drag the sketch entity to relocate a relation, use Auto Repair Sketch Relation or Dimension , or use the Display/Delete Relations tool.

  • Drag the sketch entity.
    1. Click the entity that displays the dangling handle to display the relations in the PropertyManager.

      The dangling relation highlights with the same color as the related sketch entity.

    2. Drag the dangling handle to the appropriate sketch entity to transfer the relation from the missing entity to the selected entity.
  • Auto Repair Sketch Relation or Dimension

    Right-click the dangling relation. In the context toolbar, click Auto Repair Sketch Relation or Dimension .

  • Display/Delete Relations tool.

    Some relations, like a coincident relation between points, can only be repaired with the Display/Delete Relations tool.

    1. Click Display/Delete Relations on the Dimensions/Relations toolbar, or click Tools > Relations > Display/Delete.
    2. In the PropertyManager, under Relations, select Dangling in Filter to display only dangling relations in Relations .
    3. Select a relation in Relations.
    4. Under Entities:
      1. Select the entity that shows Dangling for Status.
      2. Select the entity in the graphics area for Entity to replace the one selected above to form the correct relation.
      3. Click Replace, then click .
      In the PropertyManager, you can use Find Replacement to fix dangling relations in a sketch. SOLIDWORKS® searches for a replacement. A message appears if a replacement is not found.

      If you have multiple dangling relations, click Repair All Dangling to automatically fix all dangling relations.

      These options are available only for 2D sketches. Dangling relations that have external references cannot be repaired using Repair All Dangling and Find Replacement. You must manually repair these dangling relations.