Flat patterns and DXF for the laser cutter

A laser cutter cuts the flat pattern: the sheet before it is bent. Solid Vibes computes it from the same model as the 3D part, so the blank is exactly the size that bends back into your design.

1. Look at the flat pattern

Any of these switches the viewport from the bent part to the unfolded blank (and back):

• the Flat pattern toggle in the Sheet metal section of the Parameters tab,
• right-click on the sheet → Flat pattern,
• ⌘K → Show flat pattern.

The banner reads the blank size and the number of bends, e.g. Flat pattern · 100.3 × 40 mm · 2 bends. Bend centre lines are dashed, each with its note: UP 90° R2 means "bend up (toward the top face) by 90° with a 2 mm inside radius". The Sheet metal section lists every bend with its bend allowance.

2. Check the numbers (K-factor or bend table)

The length of sheet a bend uses is its bend allowance: BA = angle × (R + K × T), with the angle in radians, R the inside radius, T the thickness and K the K-factor (where the neutral axis sits, 0.3–0.5). A flat length is the sum of the outside flange lengths minus one bend deduction per bend: BD = 2 × (R + T) × tan(angle / 2) − BA.

Example: 2 mm aluminium, R 2 mm, K 0.44, an L-bracket with two 30 mm legs: BA = 4.524 mm, BD = 3.476 mm, blank = 30 + 30 − 3.476 = 56.52 mm.

Your shop's numbers win: if they give you a K-factor, set it in the Sheet metal section. If they give a bend table (allowances or deductions per thickness, radius and angle), the agent can add it ("use this bend table: 2 mm, R2, 90° → deduction 3.2"); rows that match the thickness and radius replace the K-factor, other angles are interpolated. The bend list says which source each bend used.

3. Download the DXF

Open Make → Export, choose DXF. For a sheet-metal piece the DXF content switch defaults to Flat pattern (the other choice is the classic drawing views). Press Download flat-pattern DXF. The banner's download icon and ⌘K → Export flat pattern (DXF) take you to the same place.

The file is DXF R12 in millimetres, ready for laser, plasma or punch CAM:

Several sheet-metal pieces in one Thing are laid out side by side in one file. Tell your CAM to cut OUTLINE only.

4. Drawings for the bending shop

In Make → Drawings, sheet-metal pieces get a FLAT PATTERN view next to the usual views: the blank, its size in the label, the bend lines and their notes. Add or remove it under Sheet & views.

Troubleshooting

• "Some solid steps … can't be unfolded": only round holes made by hole or extrude-cut steps are carried into the flat pattern. Make other cut-outs with Cut through the sheet (a sketch on the base flange's plane), which also works across bends.
• "The flat pattern overlaps itself": two flanges need the same sheet. Shorten one, use a partial flange (offsets) or a corner relief.
• The blank is a little off from a test bend: measure a test piece and adjust the K-factor (or add a bend-table row) — the flat pattern updates immediately.