Errors & Fixes
SOLIDWORKS drawing errors — dangling dimensions, empty and outdated views
Drawings are linked to the model, so most drawing errors come from a change made somewhere else: an edge that a dimension was attached to has gone, the model file was moved, or the views are not set to update. SOLIDWORKS 2024 made the most common repair easier with Reattach for dangling dimensions; the other fixes work in any recent release.

Applies to: SOLIDWORKS 2019–2027 drawings; Reattach from SOLIDWORKS 2024.
Most likely causes
- Model edge or face a dimension used was changed or removed (most common)
- Model moved or renamed outside SOLIDWORKS — views go blank (common)
- Automatic View Update switched off for the drawing (common)
- Annotations hidden rather than deleted (occasional)
- Broken-out section profile not closed, or depth edge not usable (occasional)
- Detached drawing showing old geometry (occasional)
Which problem do you have?
| What you see | Go to |
|---|---|
| Dimension in a different colour, attached to nothing | Reattach dangling dimensions |
| Views show the old model | Automatic View Update, Ctrl + Q |
| Views are empty | Point the drawing at the moved model |
| Dimensions you added are gone | Hidden annotations |
| Broken-out section will not build | Profile and depth |

Keep dimensions from dangling
- Dimension to edges that survive changes — outer edges and hole centres rather than fillet tangent edges that move when a radius changes.
- Make model changes before detailing, especially fillets and chamfers.
- Move and rename files with SOLIDWORKS tools (File Explorer's SOLIDWORKS right-click menu or Pack and Go), not plain Windows, so drawings keep their links — see missing references.
Dimension and annotation basics are in the drawings course, starting with dimensions and annotations. Sheet metal flat pattern views that show the folded part are covered in flatten errors.
Fixes, in order
1. Reattach dangling dimensions (2024 and later)
Right-click the dangling dimension → Reattach. The unattached points are marked red; pick the new edge or vertex for the first point, then the second. It also works on healthy dimensions you want to move to another reference, but not on imported, DimXpert, chain, symmetric linear diameter or path length dimensions.
2. Drag the endpoint in older releases
Before 2024, drag the dimension's endpoint handle onto the new model geometry. If that is fiddly, delete the dimension and add it again.
3. Turn on Automatic View Update
Right-click the drawing name at the top of the FeatureManager tree and select Automatic View Update. Since SOLIDWORKS 2019 it is saved in the drawing, so one file can behave differently from another. A view can be excluded on purpose with Exclude from Automatic Update.
4. Rebuild — and force it when needed
Ctrl + B rebuilds what changed; Ctrl + Q rebuilds everything, including detail and section views built from sketched lines. Hawk Ridge treats Ctrl + Q as a diagnostic step rather than routine.
5. Point blank views at the moved model
Empty views usually mean the model was moved. Close the drawing without saving, File → Open, select it, click References, double-click the model and browse to its new location, then open.
6. Show hidden annotations
View → Hide/Show → Annotations shows hidden items faintly so you can pick and show them again.
7. Fix broken-out section problems
The profile must be a closed spline — or sketch a closed rectangle or circle first and select it before the command. For depth, use a straight edge parallel to the cut plane or a circle (the plane goes through its centre). If a silhouette edge cannot be picked, CADimensions uses the 3D Drawing View to pick it.
8. Load the model into a detached drawing
A detached drawing opens without the model and shows the geometry as it was saved. Right-click a view → Load Model to update it.
Sources
- Engineers Rule — Final Five Favorite Features of SOLIDWORKS 2024 (Dec 2023)
- GoEngineer — What's New SOLIDWORKS 2024 Drawings: Chain Dimensioning, Highlighting, & More (Nov 2023)
- Javelin — SOLIDWORKS 2024 Drawings and MBD (Feb 2024)
- Javelin — Automatic View Update option saved as a Document Property in SOLIDWORKS 2019 (Dec 2018)
- Javelin — SOLIDWORKS Rebuild Commands (Jul 2017)
- Hawk Ridge Systems Support — Check for Feature Errors in SOLIDWORKS with Force Rebuild
- Javelin — How to fix Empty SOLIDWORKS Drawing Views (Mar 2021)
- Javelin — How to locate hidden or newly-imported annotations in SOLIDWORKS Drawings (Feb 2024)
- CATI — SOLIDWORKS DRAWINGS: Hiding and Showing Annotations and Dimensions (Aug 2017)
- TriMech — Broken-Out Section View in SOLIDWORKS
- CADimensions — Use 3D Drawing Views to Ease Section Depth Selections
- CATI — SOLIDWORKS: Detached Drawings (Jul 2014)
- engineering.com — How to Create Detached Drawings in SOLIDWORKS
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
What is a dangling dimension in a SOLIDWORKS drawing?
+
A dimension whose model reference — an edge, vertex or face — no longer exists after a model change. Reattach it to new geometry or delete and re-create it.
Why don't my drawing views update when I change the model?
+
Automatic View Update may be off for that drawing, or a view may be excluded from it. Turn it on from the drawing's right-click menu and rebuild with Ctrl + B or Ctrl + Q.
Why are my drawing views empty?
+
The drawing cannot find its model — usually because the model was moved or renamed in Windows. Re-point it with References in the Open dialog and move files with SOLIDWORKS tools from now on.
Related
- Dimensions in SOLIDWORKS drawingsHow to dimension SOLIDWORKS drawings: import Model Items, add reference dimensions, ordinate and chain dimensions, hole callouts and auto arrange.
- SOLIDWORKS missing references — unable to locate fileSOLIDWORKS "unable to locate file" when opening an assembly or drawing? How the search order works, how to repair references, and how to rename files safely.
- Broken-out sections and break viewsHow to use broken-out sections in SOLIDWORKS drawings to reveal hidden features, set the depth, and shorten long parts with a break view and break gap.
- SOLIDWORKS rebuild errors and warnings — how to fix themFix SOLIDWORKS rebuild errors: red and yellow feature icons, the What's Wrong dialog, dangling references, zero-thickness geometry and failed fillets.