Errors & Fixes
SOLIDWORKS zero-thickness geometry error — what it means and how to fix it
In a SOLIDWORKS solid every edge must border exactly two faces. When a feature would create an edge shared by more faces — two blocks touching along a line, a cut exactly tangent to a hole, bodies meeting at a single point — SOLIDWORKS refuses and shows this error. The fix is always the same idea: make the features overlap a little, leave a small gap, or keep them as separate bodies.

Applies to: SOLIDWORKS 2020–2027 parts; also failing section views in drawings.
Most likely causes
- Two features touching along a single edge or line (most common)
- A cut or hole tangent to, or exactly on, an existing edge (common)
- Hole Wizard holes placed exactly on an edge (common)
- Bodies meeting at a single vertex (occasional)
- Sweep cuts whose profiles touch at one tangent point (occasional)
- A shell whose thickness matches existing geometry (occasional)
The rule behind the message
SOLIDWORKS Help calls it non-manifold geometry: edges and vertices that do not join properly to the geometry next to them. In a valid solid every edge borders exactly two faces. Two blocks merged along a shared edge give that edge four faces — so the feature is refused, because the result would break calculations further down the tree.

| Situation | What to change |
|---|---|
| Boss touching a block along one line | Overlap the boss into the block, or leave a gap |
| Circular cut tangent to an edge or hole | Move the profile, delete the tangent relation |
| Two bodies touching at one corner | Overlap, a tiny joining extrude, or keep them separate |
| Hole Wizard hole exactly on an edge | Move the hole past or away from the edge |
| Sweep cut profiles touching at one point | Change the path or profile so they overlap or separate |
| Shell thickness equal to existing geometry | Change the thickness slightly — see shell errors |
When the gap or overlap is real design
If the two features genuinely only touch — two parts welded at a corner, say — they are separate bodies or separate parts, not one solid. Model them that way and join them in a weldment or an assembly.
Other red features in the tree? Work through rebuild errors from the top.
Fixes, in order
1. Make the features overlap
Extend one feature so the two share real volume instead of a line. Even a small overlap removes the shared edge.
2. Or leave a small gap
Break the tangent relation, offset the feature or move the profile so there is a small gap. TriMech suggests keeping any such gap or overlap at least an order of magnitude below your tightest tolerance, so it never affects the part.
3. Clear Merge result
If you do not need a single body, clear Merge result in the feature's PropertyManager. The rule only applies inside one body, so two bodies may touch along an edge. See multibody parts.
4. Edit the sketch of the failing feature
Remove the tangent or coincident relation that puts the profile exactly on the existing edge, move it slightly, rebuild, then confirm with Check that no bad edges remain.
5. Move Hole Wizard holes off the edge
Javelin's Hole Wizard case: a hole placed exactly on an edge — common with assembly holes through several parts and with patterns. Move it a little past the edge or further into the part, and review the design if it sits that close.
6. Fix point contact
For bodies that meet at a single vertex, TriMech suggests a tiny joining extrude, a midplane extrude or a revolve so the contact becomes a real volume.
7. Split faces back if needed
Merging can turn separate top faces into one. A Split Line with a sketch divides them again, for example to give them different appearances.
Sources
- SOLIDWORKS Help 2024 — Zero thickness geometry
- Hawk Ridge Systems Support — What is Zero Thickness Geometry?
- TriMech — Three Tips to Deal with Zero Thickness Geometry
- GoEngineer — SOLIDWORKS Zero-thickness Error: What Does It Mean? (Jul 2022)
- Javelin — SOLIDWORKS Hole Wizard Zero Thickness Geometry Rebuild Error (Apr 2020)
- EGS India (SOLIDWORKS reseller blog) — How to Fix Zero Thickness Geometry in SOLIDWORKS
- CATI — Modeling beyond the limitations (Oct 2012)
- SOLIDWORKS Tech Blog — Surface and advanced modeling skills that you may not yet know (Part 1) (May 2020)
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
What is zero-thickness geometry in SOLIDWORKS?
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Non-manifold geometry: an edge shared by more than two faces, or bodies touching at a line or point with no volume between them. SOLIDWORKS does not allow it inside one solid body.
How do I fix zero-thickness geometry?
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Make the features overlap slightly, leave a small gap, or clear Merge result so they stay separate bodies.
Why does my section view fail with zero-thickness geometry?
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A drawing section can fail with "The model could not be properly sectioned by the section line" when the model has zero-thickness conditions — Help names a cut tangent to a hole as a frequent cause.
Related
- 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.
- SOLIDWORKS fillet failed — causes and fixesFix failed fillets in SOLIDWORKS: fillet order, radius too large, tangent propagation, Keep features, FilletXpert, FeatureXpert and setback corners.
- SOLIDWORKS shell failed — how to find and fix the causeFix SOLIDWORKS shell failures: thickness above the minimum radius of curvature, zero-thickness geometry, faces that will not offset, and the Check tool.
- SOLIDWORKS multibody partsWhat multibody parts are in SOLIDWORKS, how Merge result and Feature Scope work, Save Bodies to make an assembly, and when an assembly is better.