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SOLID WORKS ClubSOLID WORKS Club

Sheet metal · Lesson 8

Forming tools in SOLIDWORKS sheet metal

Forming tools press shapes into sheet metal — louvers, lances, dimples, ribs, embosses. You drag a tool from the Design Library onto a face and position it with a sketch. Your own tools are ordinary parts with a Forming Tool feature that marks the stopping face and any faces to remove, saved as .sldftp. Since 2024, simple indents can also be made with the Stamp feature.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Sheet metal panel with louvers, dimples and an emboss made with forming tools

Where to find it

Design Library → forming tools; Sheet Metal tab → Forming Tool; File → Save As → Form Tool (*.sldftp)

Forming tool parts

Element Use
Stopping face Face that butts against the sheet and sets depth (teal in preview)
Faces to remove Become holes in the sheet (red in preview)
Insertion point Placement point; by default the stopping face centroid
Configurations Different sizes of one tool, chosen when placing
Split Line Removes only part of a face

Shipped tools may still use the older method with an orientation sketch and red faces; they can be updated with a Forming Tool feature. The Design Library itself is covered in Design Library.

Step by step

  1. 1

    Model the tool

    In a new part, extrude a 60 × 60 × 10 block. On its top face, extrude a 20 × 10 slot-shaped boss, 3 mm high, and fillet its edges with a radius of at least 2 (the sheet thickness).

  2. 2

    Add the Forming Tool feature

    Forming Tool (Sheet Metal tab). Stopping face: the top of the block. Leave Faces to remove empty for an emboss. Check the insertion point.

    Forming Tool feature with the stopping face in blue and the formed shape in yellow
    The stopping face sets the depth; faces to remove become holes.
  3. 3

    Save as a form tool

    File → Save As → Form Tool (*.sldftp) into a folder the Design Library can reach.

  4. 4

    Place it

    Drag the tool from the Design Library onto the base flange's top face, set the rotation, then position it on the Position tab and click the tick.

Common mistakes

  • Multibody tool parts — join the geometry into one body.
  • Inside fillets smaller than the thickest sheet the tool will form — the tool can fail.
  • Saving any part as .sldftp without a Forming Tool feature — no warning, but it errors when used.
  • Forming downwards — forming upward avoids marking the part and bowing the sheet.

Lesson 8 of 13 in the sheet metal course.

Practice

Make the 20 × 10 × 3 emboss tool and place it on the 100 × 60 base flange. Check: the emboss stands 3 mm above the top face, and the tree shows the placed tool as one feature.

Sources

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

Frequently asked questions

How do I make a custom forming tool in SOLIDWORKS?

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Model the shape on a block, add the Forming Tool feature with a stopping face (and faces to remove for holes), and save as a .sldftp form tool.

Where are forming tools stored?

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.sldftp tools can live in any folder the Design Library reaches. Older .sldprt tools need a folder marked as a Forming Tools Folder.

How do I show forming tools in the flat pattern?

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The form tool feature has flat pattern visibility settings, and form feature colours for flat pattern views are set in Document Properties.

What is the Stamp feature?

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Added in SOLIDWORKS 2024, Stamp makes an indent from any closed sketch with depth, draft and radii, without a forming tool.