Errors & Fixes
SOLIDWORKS shell failed — how to find and fix the cause
A shell offsets every face of the part inwards by the wall thickness. It fails when one of those offsets is impossible: a curved face tighter than the wall is thick, a face that would offset into its neighbour, or zero-thickness geometry where the wall exactly meets another face. The Check tool tells you the thickest shell your part can take before you even try.

Applies to: SOLIDWORKS 2020–2027 parts, including imported models.
Most likely causes
- Wall thickness larger than the smallest radius of curvature (most common)
- Zero-thickness geometry — a dimension equal to the shell thickness (common)
- A face that offsets into its neighbour or disappears (common)
- Free-form faces: splines and asymmetric fillets (occasional)
- Bad faces in imported geometry (imported parts)
Why thickness and curvature collide

Offsetting a convex curve inwards makes its radius smaller by the wall thickness. If the wall is thicker than the radius, the offset curve would have a negative radius — it folds over itself and the shell cannot be built. The SOLIDWORKS Tech Blog notes that when the thickness exceeds the minimum radius you may get only a warning: the shell completes, but check the inside faces, which may not be clean.
A quick diagnostic order
- Check → minimum radius of curvature. Is your wall thinner?
- Shell again and look at the highlighted faces.
- Any dimension in the part equal to the shell thickness, or twice it?
- Free-form surfaces? Split them with a split line and test with Offset Surface to find the exact face, as Javelin did on a golf club head.
- Imported model? Repair it first.
The Shell options — faces to remove, outward shell, multi-thickness — are covered in the Shell lesson. For plastic parts designed to be printed, the wall rules are in the 3D-printed enclosure project.
Fixes, in order
1. Read the minimum radius from Check
Tools → Evaluate → Check with Minimum radius of curvature reports the smallest radius in the part — the thickest shell that can work. PLM Group's example: 3.45 mm shells, 3.46 mm fails. Click the result to see where that face is.
2. Reduce the thickness — or the curvature
Set the wall below that radius, or open up the tight fillet or spline that limits it. Circular fillets usually allow a wall close to their radius; free-form faces are where the limit bites.
3. Look at the highlighted faces
When a shell fails, the faces that could not be offset are shown in a different colour. That tells you which feature to change.
4. Change dimensions that equal the thickness
The SOLIDWORKS Tech Blog's example: a 3 mm thick region cannot take a 1.5 mm shell. No option fixes zero-thickness — change the dimension or the shell thickness slightly. See zero-thickness geometry.
5. Use Multi-thickness for difficult faces
Add faces to the Multi-thickness box in the Shell PropertyManager to give them their own, thinner wall instead of shrinking the whole part.
6. Shell before features that should stay solid
Feature order matters: Javelin shows a shell after a merged extrude leaving an unwanted ledge. Shell first, then add bosses, ribs and outside details — or choose end conditions that stop at the shelled faces.
7. Use Shell to diagnose offsets
Offset Surface and Thicken have no failure diagnosis, but Shell does. Javelin's tip: run Shell outward to see which faces will not offset, then remove them from your selection.
8. Repair imported geometry first
On imported parts run Import Diagnostics before adding features, or Check for bad faces. See import errors.
Sources
- SOLIDWORKS Tech Blog — Surface and advanced modeling skills that you may not yet know (Part 1) (May 2020)
- PLM Group Support — Use of Check in SOLIDWORKS (May 2018)
- GoEngineer — Check Tool SOLIDWORKS Tutorial (Jul 2022)
- Javelin — Solving SOLIDWORKS surfacing challenges when designing a Golf Club head (Aug 2015)
- Javelin — Troubleshooting the Offset and Thicken Surface Commands (May 2012)
- Javelin — Creating a Multi-Thickness Shell in SOLIDWORKS (Nov 2023)
- Javelin — How Feature Ordering in SOLIDWORKS Affects Your Design (Jun 2026)
- Solid Solutions — Repair and Diagnostics Tools (training supplement PDF)
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
Why does Shell fail in SOLIDWORKS?
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Usually because the wall is thicker than the smallest radius of a curved face, or because a dimension equals the shell thickness and creates zero-thickness geometry.
How thick can my shell be?
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Run Check with Minimum radius of curvature: the shell must be thinner than the radius it reports.
Why does my shelled part have a ledge or extra material inside?
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The shell came after a feature that was merged into the body, so that feature was shelled too — or a later extrude ran into the hollow. Move the shell earlier in the tree or change the end condition.
Related
- SOLIDWORKS ShellHow to use Shell in SOLIDWORKS to hollow a part: faces to remove, wall thickness, shell outward, multi-thickness walls, and what to do when the shell fails.
- SOLIDWORKS zero-thickness geometry error — what it means and how to fix itWhat 'would result in zero-thickness geometry' means in SOLIDWORKS: edges shared by four faces, line and point contact, holes on edges — and how to fix it.
- 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 STEP and IGES import errors — how to fix themFix SOLIDWORKS STEP and IGES import errors: faulty faces and gaps, surfaces instead of solids, 3D Interconnect vs classic import, wrong IGES units.