What file you need for laser cutting sheet metal
Short answer: for laser cutting sheet metal you need a DXF at 1:1 scale in millimetres — only the part contours, closed, without frame, dimensions or title block. If the part is bent afterwards, the DXF must contain not a “projection” but a flat pattern with bend allowance, otherwise the blank comes out the wrong size. Thickness, material grade and quantity go in the order, not in the file.
Which formats shops accept
| Format | Good for cutting? | When to use it |
|---|---|---|
| DXF | Yes — the standard | Flat part contour at 1:1. Opens in any machine CAM program. |
| DWG | Usually yes | AutoCAD’s native format. Some shops ask to re-save it as DXF — easier to send DXF straight away. |
| STEP | As a source | A 3D model: the shop builds the flat pattern itself, but with its own K factor — check the result. |
| Reference only | A vector PDF can be converted to DXF, but the scale often shifts. A scanned PDF is just a picture — it gets redrawn. | |
| JPG, PNG, photo | No | A machine doesn’t cut from a picture: it needs a dimensioned drawing to build the contour from. |
DXF requirements for laser cutting
Open the file and measure the overall size — it must match the drawing to a tenth.
A break in a line — the machine can’t tell where the part is. Overlapping lines — a double cut and a burnt edge.
Remove the frame, title block, dimensions and text or move them to a separate layer — otherwise they get cut too.
Not every machine program reads splines; polylines and arcs work everywhere.
The font you used may not exist on the machine.
AutoCAD 2000–2013 or R12 opens almost everywhere — check with the shop.
Holes and webs no smaller than the sheet thickness. This is a guide: the shop will tell you the exact minimum.
If the part is bent: you need a flat pattern, not a top view
When bent, metal stretches on the outside and compresses on the inside — so the flat blank is shorter than the sum of the outside flange dimensions. By how much depends on three numbers: sheet thickness s, inner bend radius r and the factor K (where the neutral layer lies; usually 0.3–0.5).
Bend allowance per bend: BA = π × angle / 180 × (r + K × s)
What to put in the DXF of a bent part:
- flat pattern contour on its own layer (e.g. CUT): only this is cut;
- bend lines on another layer (BEND), with direction up/down;
- the bend table — angle, radius, K — on a notes layer (NOTES) or in the order.
Every shop has its own K — it depends on the press brake tooling. If the shop has a bend table, calculate the flat pattern from it: the difference in the finished size ranges from hundredths to several tenths of a millimetre.
Common mistakes that get files sent back
The contour is drawn at 1:2 or in inches while the shop reads millimetres — the part comes out half the size or 25.4 times smaller.
They sent a “top view” of a bent part instead of a flat pattern.
A hole right at the bend line — bending pulls it into an oval. You need a relief slot or the hole further from the bend.
No relief cuts in corners where two bends meet — the metal tears.
Duplicate lines from copy-paste — the machine cuts the same place twice.
Several parts in one file and no quantity for each.
How to check a flat pattern before cutting
The most reliable check is to “fold it back”: build a 3D model from the flat pattern with the same bends and compare it with the part drawing. An extra hole, a reversed bend direction or the wrong K show up at once, before a batch is cut. We check every flat pattern this way: the length is checked against the allowance formula to 0.001 mm, then the model is folded back and compared with the part.
Tick what you have already checked
We’ll make the DXF flat pattern
Questions and answers
Can I send the shop a PDF instead of a DXF?
Only if the shop redraws the part itself. The machine needs a 1:1 vector contour; a vector PDF can be converted to DXF, but the scale and arcs must be checked after conversion. A scanned PDF is a picture — it gets redrawn.
Which DXF version should I save?
AutoCAD 2000–2013 or R12: almost every machine program opens them. If the shop asks for a specific version, save in that one.
Who calculates the bend allowance — me or the shop?
Whoever builds the flat pattern calculates it. If you give the shop a 3D model, it builds the flat pattern with its own K. If you send a finished DXF, add the allowance yourself from the shop’s bend table and state K in the order.
Do I need to draw bend lines in the DXF?
For cutting — no, only the contour is cut. For bending — yes: bend lines on a separate layer with direction help the press brake operator and reduce scrap.
What if I only have a paper drawing?
You need a DXF built from the drawing’s dimensions — a scanned picture can’t be cut. A designer or a service like ours can make it: a model is built from the drawing, the flat pattern from the model, and every dimension is checked.