Errors & Fixes
SOLIDWORKS sweep and loft errors — failures and twists fixed
Sweeps and lofts fail for a handful of reasons, and almost all of them are in the sketches rather than the feature. A sweep needs a closed profile that the path pierces, and nothing may intersect itself. A loft twists when profiles are picked at different points or their sketches have different numbers of segments. Watch the preview: if it disappears, the feature will not build.

Applies to: SOLIDWORKS 2020–2027 swept and lofted bosses, cuts and surfaces.
Most likely causes
- The path does not pierce the plane of the profile (most common)
- Profile, path or result intersects itself (common)
- Guide curves not related to the profile, or over-related (common)
- Loft profiles picked at different points, misplaced connectors (common)
- Loft profiles with different numbers of segments (common)
- Open profile used for a solid sweep (occasional)
Sweep checklist

| Requirement | Applies to |
|---|---|
| Closed profile | Boss and cut sweeps (surface sweeps may be open) |
| Path pierces the profile plane | All sweeps |
| No self-intersection in profile, path or result | All sweeps |
| Guide curves coincident with or pierced to the profile | Sweeps with guide curves |
| Tool body: convex, not merged, continuous tangent path | Solid-body sweep cuts |
GoEngineer's notes on solid-body sweep cuts: the path must be tangent along its length and start on or inside the tool body's profile, and an extruded tool body is more reliable than a revolved one.
Loft checklist

- Each profile is a planar sketch or a face; only the first and last may be a point.
- All profiles have the same number of segments, split where needed.
- Pick profiles at matching points in the graphics area.
- Check the connector lines in the preview before you click OK.
- Guide curves end coincident with the profiles; set start and end constraints for the shape at each end.
If connectors vanish after a dimension change, GoEngineer suggests looking for sketch errors, dangling relations or unsolvable sketches — see sketch errors. When a loft cannot hold a constant section, a sweep with a twist is often the better feature.
Both features are taught step by step in the Sweep and Loft lessons; the compression spring and helical gear projects use them in practice.
Fixes, in order
1. Add a Pierce relation between profile and path
The path must cross the profile's plane. In the profile sketch, select the sketch point at the profile's centre and the path itself and add a Pierce relation. Hawk Ridge calls this the condition that causes the most confusion.
2. Close the profile for a solid sweep
A swept boss or cut needs a closed profile; only a swept surface may use an open one. Run Check Sketch for Feature if you are not sure.
3. Remove self-intersection
Neither profile, path nor result may cross itself. Check the path for loops and the profile for crossing lines, and watch the preview as you change sizes. Sweep cuts whose profiles touch at one tangent point fail for a related reason: SOLIDWORKS cannot tell whether material exists there.
4. Relate guide curves with Pierce, not Coincident
Solid Solutions traced failing guide-curve sweeps to the profile sketch: coincident relations to model edges or curve endpoints stop the profile from following. Use Pierce relations to the guide curves and the path, and no other relations to the outside.
5. Pick the right orientation option
For paths with sharp corners, GoEngineer suggests Keep Normal Constant or Follow Path with all faces. If a 3D path twists the profile, Hawk Ridge converts the path to a 2D sketch and uses the 3D sketch as a guide curve.
6. Pick loft profiles at matching points
Select each loft profile in the graphics area near the same corner or vertex — not from the FeatureManager tree. That keeps the connectors lined up and the loft untwisted.
7. Edit or reset connectors
Drag the green connectors to matching vertices, or right-click → Reset Connectors. Normal Undo does not undo connector edits; use Undo connector edit.
8. Give profiles the same number of segments
When one profile has four lines and the next a circle, split the entities so both have matching points: Split Entities, Segment or Fit Spline under Tools → Sketch Tools.
Sources
- Hawk Ridge Systems — Basics of the Sweep Feature in SOLIDWORKS (Jan 2015)
- Hawk Ridge Systems — Advanced Sweep Feature Techniques in SOLIDWORKS (Jan 2015)
- LibreTexts — Introduction to SolidWorks (Hortman), 6.04 Sweep
- Javelin — How to Use Swept Features in SOLIDWORKS (Oct 2026)
- Solid Solutions — Sweeps with Guide Curves when they don't work (Oct 2014)
- GoEngineer — SOLIDWORKS Sweeps FAQ (Dec 2014)
- CATI — Modeling beyond the limitations (Oct 2012)
- GoEngineer — Managing SOLIDWORKS Loft Connectors (Dec 2022)
- GoEngineer — SOLIDWORKS Lofts FAQ (Jan 2015)
- Hawk Ridge Systems — 3 Steps to Better Lofts and Boundaries in SOLIDWORKS (Sep 2019)
- Javelin — Creating a Simple Loft Feature in SOLIDWORKS (Nov 2023)
- Javelin — Getting to Know the Loft Feature to Take Your Modeling to New Heights (May 2025)
- GoEngineer — Check Sketch for Feature explained
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
Why will my sweep not work in SOLIDWORKS?
+
Most often the path does not pierce the profile's plane, the profile is not closed, or the profile, path or result would intersect itself.
How do I stop a loft from twisting?
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Pick every profile near the same corner in the graphics area, line up the connectors, and make sure each profile has the same number of segments.
What is a Pierce relation?
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A sketch relation that makes a point lie where a curve from another sketch passes through the sketch plane. It is the standard way to tie a sweep profile to its path or guide curves.
Related
- SOLIDWORKS SweepHow to use Swept Boss/Base and Swept Cut in SOLIDWORKS: profile and path rules, Pierce, circular profiles, orientation, twist and guide curves.
- SOLIDWORKS LoftHow to use Lofted Boss/Base in SOLIDWORKS: profiles on offset planes, profile order, guide curves, end tangency, and fixing twisted lofts.
- SOLIDWORKS sketch errors — over defined, unsolvable and open sketchesFix SOLIDWORKS sketch errors: over defined, no solution found, dangling relations, open or self-intersecting contours, with SketchXpert and Repair Sketch.
- 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.