Working in SOLIDWORKS, and having trouble with your sketches? Maybe they are showing up in red and yellow, with messages indicating errors and warnings? Below is a quick guide to help you troubleshoot the problems, and more importantly, fix them.
- Understand the Error & Use Sketch Color Cues
Black: Fully defined. This is what we want, fully defined sketches. This means that the sketch is defined by relations and or dimensions. It is important to do this with intention, as it has a large impact your design intent.
Blue: Underdefined. This means your sketch still has the ability to move and be repositioned. If you are not sure why something is still showing as underdefined, try selecting a blue entity and try dragging it. This usually provides an indication of what type of dimensions or relations need to be added to fully define it.
đź”´ Red: Conflicting or overdefined. Any dimensions and/or relations showing up in red, means that you have relations or dimensions that conflict with each other, or are accomplishing the same thing. You will want to remove the incorrect ones, and once fixed, the sketch will show up in either blue or black.
🟡 Yellow: Dangling (broken reference or constraint). This means that whatever your sketch entity was referencing, is now missing. It might have been related to a feature that was deleted, and changed significantly. The broken relation or constraint can be either reattached manually, replaced, or repaired.
- How to Fix Red and Yellow Sketch Entities: Use These Key Tools
Dangling dimensions/relations: These occur when the geometry or entities they were originally attached to are deleted or modified, causing the handles to lose their reference.
SketchXpert
Where: Tools > Sketch Tools > SketchXpert (If your status bar
Use this to identify and resolve overdefined/conflicting relations. It allows SOLIDWORKS to assess the problems and provide different solutions to choose from.
Display/Delete Relations
Where: Tools > Relations > Display/Delete Relations
Shows all constraints in one list for easy deletion or editing. You can specify to show dangling relations. You can use the Replace tool at the bottom of the Display/Delete Relations PropertyManager.
Reattach Relation/Dimension Handles
Drag and drop: Click the dimension or relation that is dangling, and a small red square, called a handle will appear. Drag the dimension handle to the new attachment point.
Fixing Common Problems
- Overdefined Sketch
Cause: Too many dimensions or redundant constraints.
Fix:
- Use SketchXpert to auto-resolve (see above for more information).
- Delete any duplicate dimensions or constraints (like multiple horizontal/vertical constraints).
- Avoid dimensioning both ends of a fixed-length line when it’s already constrained by geometry.
- Underdefined Sketch
Cause: Missing constraints or dimensions. Generally, all sketches should be fully defined. Fully defined sketches will be shown in black, while underdefined sketches will be shown in blue.
Fix:
- Add missing dimensions manually.
- Use Add Relations to define geometry (e.g., horizontal, perpendicular).
- Lock reference points (e.g., fix one point to origin).
- Check for disconnected or floating segments.
- Geometry errors causing Feature to fail or fail to rebuild
Cause: Gaps, overlaps, or bad contours can cause features to fail to be created or rebuilt. Assess the warning that is associated with the error, as this can help pinpoint the problem and possibly offer routes to a solution.
Fix:
Use Check Sketch for Feature:
Tools > Sketch Tools > Check Sketch for Feature to assess the sketch for errors for the type of feature you are using it for.
Zoom in to ensure endpoints are properly merged. (Use the Zoom to Fit tool on the heads-up toolbar to look for extraneous entities
- Tips to Prevent Sketch Errors
- Always fully define sketches before adding features.
- Start from the origin when possible.
- Use construction geometry to help with layout without affecting solid features.
- Avoid mixing too many automatic and manual constraints.
- Multiple problems in the FeatureTree? Start at the top and work your way down. This helps
- When All Else Fails
Suppress dimensions/relations temporarily to isolate problems.
Recreate the sketch cleanly if you get stuck or are spinning your wheels. Sometimes it is quicker to just restart a sketch!
Save your part before experimenting—errors can cascade, and this way you can always go back to a good spot.