Errors & Fixes
SOLIDWORKS fillet failed — causes and fixes
Fillets fail more often than any other feature, and the error message names the fillet without saying why. The usual reasons are order — which fillet comes first — a radius too big for the faces around it, and too many edges in one feature. The first warning sign is in the preview: if the preview disappears while you pick edges or change the radius, the fillet will almost certainly fail.

Applies to: SOLIDWORKS 2020–2027 parts.
Most likely causes
- Fillets created in an order that cannot be solved (most common)
- Too many edges selected in one fillet feature (common)
- Radius larger than the neighbouring faces allow (common)
- Several fillets meeting at one corner (vertex) (common)
- Tangent propagation picking up more edges than intended (occasional)
- Bad edges from Boolean operations or imported geometry (occasional)
Order of fillets: the rules from Help

| Rule | Why |
|---|---|
| Larger fillets before smaller ones | Especially where several fillets meet at a vertex |
| Draft before fillets | On cast and moulded parts with many filleted edges |
| Cosmetic fillets last | They slow every rebuild after them |
| Same radius in one feature | Faster rebuilds, one value to edit |
Javelin adds that fillets generally belong at the end of the tree, because they remove edges that later features may need to reference. If you must fillet earlier, dimension later sketches to planes rather than to filleted edges.
Corners where fillets meet

Three fillets meeting at one vertex are the classic failure. In order of effort:
- Create the largest of the three first.
- Use a Setback fillet on the vertex.
- Try FilletXpert — or FeatureXpert once it has failed. Hawk Ridge notes the latter often fixes corner errors by adding fillets.
- Build the corner yourself with surfaces: delete faces, trim, fill.
The fillet types themselves — constant, variable, face and full round — are explained in the Fillet lesson. For the red feature in your tree, start with rebuild errors; if the message mentions zero-thickness, see zero-thickness geometry.
Fixes, in order
1. Put larger fillets first
SOLIDWORKS Help recommends adding larger fillets before smaller ones, especially where several meet at a vertex. TriMech shows models where only one order works — swapping two fillets in the tree can be the whole fix.
2. Fillet fewer edges per feature
Selecting many edges in one fillet can fail because not all of them can be built together. Split the fillet into two or three features. Group edges with the same radius into one feature only once it works.
3. Reduce the radius or change the overflow type
If the fillet is too big for the geometry around it, reduce the radius. The Overflow type options — Keep Edge or Keep Surface — apply only when the fillet is too large for the geometry around it and change how it resolves there — worth trying before giving up.
4. Check tangent propagation and Keep features
With Tangent propagation on, one edge can pull in a whole chain of tangent edges — in one Engineers Rule example, 12 of them. Clear it if you only want the edge you picked. Keep features decides whether small bosses or holes crossed by the fillet survive.
5. Let FilletXpert find an order
FilletXpert builds constant-radius fillets and reorders them until it finds an order that solves, if one exists. It is not available in parts with more than one configuration.
6. Run FeatureXpert from What's Wrong
When a fillet or draft fails, the What's Wrong dialog can offer FeatureXpert, which usually splits the feature into several. Turn it on under Tools → Options → System Options → General if the button is missing.
7. Use setback for corners
Where three fillets meet at a corner, Setback Parameters let you pick the corner vertex and set a distance along each edge for a smoother blend. Variable size and face fillets cover cases a constant fillet cannot.
8. Rebuild the corner with surfaces
When nothing works, Hawk Ridge's method is to delete the problem faces, trim the remaining edges and close the corner with a filled surface.
Sources
- SOLIDWORKS Help 2024 (nexthelp) — Fillet Overview
- TriMech — Introducing FilletXpert in SOLIDWORKS
- Engineers Rule — An Advanced Breakdown of the SOLIDWORKS Fillet Feature Tool (Oct 2016)
- SOLIDWORKS Help 2024 (nexthelp) — Example: Tangent Propagation
- Hawk Ridge Systems — SOLIDWORKS: Exploring Fillets (Oct 2018)
- TriMech — SOLIDWORKS modelling errors, part two (Jan 2023)
- Hawk Ridge Systems — How to Blend Corners in SOLIDWORKS (Aug 2019)
- Javelin — Adding Setback Distances to your SOLIDWORKS Multiple Radius Fillet (May 2013)
- 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 my fillet fail in SOLIDWORKS?
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Most often because of fillet order, too many edges in one feature or a radius too big for the faces around it. Try larger fillets first, fewer edges per fillet and a smaller radius.
What is the difference between FilletXpert and FeatureXpert?
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FilletXpert is a way of creating constant-radius fillets that finds a working order for you. FeatureXpert appears after a fillet or draft has already failed and tries to repair it, usually by splitting it.
Should fillets be the last features in a part?
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Generally yes. Fillets remove edges later features might need, and Help recommends leaving cosmetic fillets for last because they slow rebuilds. On cast or moulded parts add draft before the fillets.
Related
- SOLIDWORKS FilletHow to use Fillet in SOLIDWORKS: constant, variable, face and full round fillets, profiles, tangent propagation, FilletXpert and why fillets fail.
- 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 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 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.