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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.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Two blocks touching along a single edge highlighted in red as zero-thickness geometry
Unable to create this feature because it would result in zero-thickness geometry.

Applies to: SOLIDWORKS 2020–2027 parts; also failing section views in drawings.

Most likely causes

  1. Two features touching along a single edge or line (most common)
  2. A cut or hole tangent to, or exactly on, an existing edge (common)
  3. Hole Wizard holes placed exactly on an edge (common)
  4. Bodies meeting at a single vertex (occasional)
  5. Sweep cuts whose profiles touch at one tangent point (occasional)
  6. 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.

Three zero-thickness cases — line contact, point contact, cut tangent to a hole — and their fixes
Overlap, gap or separate bodies — the three ways out.
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. 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. 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. 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. 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. 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. 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. 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

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.