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Errors & Fixes

SOLIDWORKS sheet metal won't flatten — causes and fixes

Sheet metal flattens only if SOLIDWORKS can treat the part as one sheet of uniform thickness with bends it understands. Most problems are either in the drawing — the flat pattern view shows the folded part — or in parts that were not built with sheet metal features: imported or converted bodies with uneven walls, closed cylinders, and gaps too large for Insert Bends.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Folded sheet metal bracket with a red warning next to an empty flat pattern outline

Applies to: SOLIDWORKS 2020–2027 sheet metal parts and drawings; cylindrical and conical Rip from 2024.

Most likely causes

  1. Flat pattern configuration saved unflattened — drawing view shows folded part (most common)
  2. Converted or imported body with non-uniform thickness (common)
  3. Closed cylinder or cone with no cut to open it (common)
  4. Gap too large or too small for Insert Bends (No bends found) (occasional)
  5. Flat Pattern annotation view active — Flatten greyed out (occasional)
  6. Bends that are not normal to the sheet, or stamped shapes (occasional)

The flat pattern view problem

ConfigurationManager with the SM-FLAT-PATTERN configuration active and Flatten turned on
The flat view reads this configuration — flatten it and save.

Javelin calls the folded flat-pattern view a workflow mistake, not a bug: the derived configuration was changed by opening the part from the drawing. Make design changes in the main configuration, never in the flat pattern one.

Features above and below Flat-Pattern

Where the feature is What it does
Above Flat-Pattern Part of the formed part; shown folded and flat
Below Flat-Pattern Applies to the flat state only
Cut made between Unfold and Fold Appears in both states

Normal Cut keeps cut edges square to the sheet, which is what laser cutting expects; Javelin lists it with Simplify Bends among the flat pattern options to check.

Parts that cannot be sheet metal

Native sheet metal needs a thin wall, uniform thickness and corner bends. Stamped shapes and bends through the thickness — such as a structural tube bent in two directions — fail that test. Javelin approximates a stamped part's blank with Surface Flatten and notes the result depends on the K-factor; SOLIDWORKS has no built-in way to flatten bent structural members.

The bend settings behind every flat pattern are explained in K-factor and bend tables; export the blank with flat pattern to DXF, and practise on the sheet metal box project.

Fixes, in order

  1. 1. Re-flatten the SM-FLAT-PATTERN configuration

    The flat pattern view uses a derived configuration created the first time the part goes on a drawing. If someone opened it from the drawing and folded it, the view shows the bent part. Open the part, activate the SM-FLAT-PATTERN configuration, click Flatten (or unsuppress Flat-Pattern), save, and refresh the View Palette.

  2. 2. Recreate the configuration if that fails

    Hawk Ridge's fallback: add a new configuration, flatten it, delete the old flat pattern configuration, rename the new one and refresh the View Palette.

  3. 3. PDM — check the part out first

    If the part was checked in before its flat view existed, the new configuration could not be saved and the drawing falls back to a folded one. Check out the part, add the flat view, save and check in.

  4. 4. Make the wall thickness uniform

    Insert Bends only works well on uniform walls. CATI's workaround for imported parts: offset one side as a surface (distance 0), delete the solid and thicken the surface to the sheet thickness.

  5. 5. Cut cylinders and cones open

    A rolled cylinder or cone needs a thin cut along its length. Revolve to 359°, sketch a small gap, or — since SOLIDWORKS 2024 — use a cylindrical or conical Rip.

  6. 6. Fix "No bends found"

    Javelin traces this Insert Bends message to the gap size and fixes it with a very small, dimensioned gap at the corner.

  7. 7. Un-grey Flatten

    Flatten can be unavailable while a Flat Pattern annotation view is active. Activate another annotation view or unsuppress Flat-Pattern1.

  8. 8. Check the flat pattern as you model

    Flatten after each edge or miter flange to catch a problem at the feature that causes it, not twenty features later.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

Why does my flat pattern view show the bent part?

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The SM-FLAT-PATTERN configuration used by the view was saved folded — usually after someone opened the part from the drawing and unflattened it. Flatten it in that configuration, save, and refresh the view.

Why can't SOLIDWORKS flatten my imported part?

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Usually because the wall is not a uniform thickness or the bends are not simple bends. Make the thickness uniform, then use Insert Bends — or Convert to Sheet Metal.

How do I flatten a cylinder in SOLIDWORKS?

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Leave a thin cut along its length: revolve less than 360°, sketch a gap, or use the cylindrical Rip added in SOLIDWORKS 2024.