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Sheet metal · Lesson 9

Flat patterns in SOLIDWORKS sheet metal

Every sheet metal part in SOLIDWORKS carries its own flat pattern — the blank the laser cuts before the press brake bends it. Flatten shows it; the Flat-Pattern feature at the bottom of the tree holds its options; Unfold and Fold let you cut across bends at their true size. In drawings, a flat pattern view adds a flat configuration and bend notes for you.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Bent sheet metal bracket next to its flat pattern with dashed bend lines and a bounding box

Where to find it

Sheet Metal tab → Flatten; FeatureManager → Flat-Pattern feature (right-click → Edit Feature)

Flat-Pattern options

Option What it does
Fixed face The face that stays still when the part flattens
Merge faces Merges coplanar faces so bend areas show no lines (on by default)
Simplify bends Straightens curved edges in the flat; many users leave it off for laser parts
Corner treatment Smooths corners of the flat blank
Grain direction Pick an edge or line for the grain
Show slit Shows slits added by some corner reliefs
Faces to exclude Leaves chosen faces out of the flat

Flat patterns in drawings

Insert a Flat Pattern view from the View Palette or tick Flat pattern in Model View. SOLIDWORKS adds a derived configuration such as DefaultSM-FLAT-PATTERN to the part and shows bend lines with bend notes. Flip View in the view's PropertyManager mirrors it so engraved text reads correctly. Since 2025, flatten, fold and unfold are faster on parts with many bodies or forming tools. Views in general are covered in drawing views.

When it won't flatten: see flatten errors.

Step by step

  1. 1

    Flatten the part

    Open the bracket and click Flatten on the Sheet Metal tab. The Flat-Pattern feature is unsuppressed and the part lies flat. Click Flatten again to bend it back.

    Flatten button on the Sheet Metal tab and the Flat-Pattern feature in the FeatureManager tree
    Flatten unsuppresses the Flat-Pattern feature at the bottom of the tree.
  2. 2

    Check the flat pattern options

    Expand the Flat-Pattern folder, right-click Flat-Pattern → Edit Feature. Keep Merge faces on — it hides the tangent lines in bend areas. Set the Fixed face and, if the material has a grain, Grain direction.

  3. 3

    Cut across a bend

    Unfold with the base as the fixed face and Collect All Bends, sketch a slot across the bend, Extrude Cut through all, then Fold. The slot wraps around the bend at its true flat size.

  4. 4

    Read the blank size

    Expand the Cut list, right-click the sheet metal item → Properties. Bounding Box Length and Width give the blank size.

Common mistakes

  • Toggling Flatten or suppressing Flat-Pattern while the flat configuration is active — the drawing's flat view then shows the bent part. Activate the SM-FLAT-PATTERN configuration, flatten again and refresh the View Palette.
  • Editing the design in the flat pattern configuration — make changes in the default configuration.
  • Unfold and Fold with different fixed faces.
  • Extra lines in a flat drawing view — Merge faces was turned off.

Lesson 9 of 13 in the sheet metal course.

Practice

Flatten the bracket from lessons 1–2 (100 × 60 base, 30 mm edge flange, 2 mm thick, R2, K 0.5). Check: the cut list's bounding box is 100 × 86.71 mm — the 60 + 30 outside legs minus a bend deduction of 3.29 mm, which you can confirm in the K-factor calculator.

Sources

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

Frequently asked questions

How do I flatten a sheet metal part in SOLIDWORKS?

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Click Flatten on the Sheet Metal tab. It unsuppresses the Flat-Pattern feature; click it again to return to the bent state.

Why does my flat pattern drawing view show the bent part?

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The SM-FLAT-PATTERN configuration had Flatten turned off. Activate it, unsuppress Flat-Pattern or click Flatten, and refresh the drawing.

How do I show bend lines?

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Bend lines live in the Flat-Pattern feature. Since SOLIDWORKS 2022 they are toggled with View → Bend Lines, separate from sketches.

Where do I find the blank size?

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In the sheet metal cut list properties: Bounding Box Length and Bounding Box Width, which are system properties since 2011.