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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SOLIDWORKS drawing errors — dangling dimensions, empty and outdated views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.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Engineering drawing with one dimension highlighted as dangling and an empty view frame

Applies to: SOLIDWORKS 2019–2027 drawings; Reattach from SOLIDWORKS 2024.

Most likely causes

  1. Model edge or face a dimension used was changed or removed (most common)
  2. Model moved or renamed outside SOLIDWORKS — views go blank (common)
  3. Automatic View Update switched off for the drawing (common)
  4. Annotations hidden rather than deleted (occasional)
  5. Broken-out section profile not closed, or depth edge not usable (occasional)
  6. 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
Dangling dimension being reattached to a new edge with red marked attachment points
Reattach picks new references one point at a time.

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. 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. 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. 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. 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. 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. 6. Show hidden annotations

    View → Hide/Show → Annotations shows hidden items faintly so you can pick and show them again.

  7. 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. 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

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?

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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?

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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?

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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.