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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.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Twisted loft between a square and a rotated square next to a failed sweep along a tight bend

Applies to: SOLIDWORKS 2020–2027 swept and lofted bosses, cuts and surfaces.

Most likely causes

  1. The path does not pierce the plane of the profile (most common)
  2. Profile, path or result intersects itself (common)
  3. Guide curves not related to the profile, or over-related (common)
  4. Loft profiles picked at different points, misplaced connectors (common)
  5. Loft profiles with different numbers of segments (common)
  6. Open profile used for a solid sweep (occasional)

Sweep checklist

Sweep profile on a plane with its centre pierced by the path curve
The path must pass through the profile's plane — tie them with Pierce.
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

Loft connectors misaligned causing twist and the same loft with connectors lined up
Line up the connectors and the twist disappears.
  1. Each profile is a planar sketch or a face; only the first and last may be a point.
  2. All profiles have the same number of segments, split where needed.
  3. Pick profiles at matching points in the graphics area.
  4. Check the connector lines in the preview before you click OK.
  5. 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. 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. 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. 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. 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. 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. 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. 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. 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

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?

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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.