Export a cut-ready DXF from Autodesk Fusion

Fusion exports DXF cleanly, but two of its dialogs have options that quietly put non-cut geometry into the file — and one of them sends your bend lines to the laser. Here is each route with the exact settings.

Last updated 11 August 2026. Options verified against Autodesk’s current Fusion help; UI labels move between releases, so the linked pages are authoritative if yours differ.

First decide which of the two routes you need

• A flat part with no bends — a plate, a panel, a bracket blank, a laser-cut box side. Export the sketch.
• A sheet metal part that gets folded — export the flat pattern, so the developed length and bend allowance are correct. Never draw the flat by hand and hope.

These have different dialogs and different traps, so they are covered separately below.

Route 1: exporting a sketch

Per Autodesk’s documentation:

1. Find the sketch in the Browser — the tree on the left, not the canvas.
2. Right-click it and choose Export DXF.
3. Choose a unit type. The design’s active unit type is the default.
4. Leave the visible-geometry checkboxes alone — see below.
5. Click OK, name the file, save it.

The three checkboxes to leave unticked

The dialog offers to add Points, Projected Geometry and Construction Geometry. For a cut file, all three should stay off.

• Points put POINT entities in the file. They are not cut paths, some CAM tools treat them as drill marks, and a preflight cannot judge them as geometry.
• Construction geometry is your centrelines and reference axes. It is not part of the part.
• Projected geometry is edges pulled in from elsewhere in the model. Sometimes it is your outline — but if it duplicates geometry already in the sketch, you have just exported the same edge twice.

This matters because a cutting service cannot tell your reference lines from your part. Xometry states that “extra-drawn features can be confused with cut geometry and cause the file processing to fail”.

Route 2: exporting a sheet metal flat pattern

Per Autodesk’s documentation:

1. Find the flat pattern in the Browser, right-click it and choose Activate.
2. Click Export DXF on the toolbar.
3. Select a unit type.
4. Optionally enable Convert Splines to Polylines and set a tolerance.
5. Decide on Center Lines and Extent Lines — this is the important one.
6. Click OK, set the file type to DXF, and save.

The bend-line trap

Autodesk states it plainly: “Outer profiles, interior profiles, bend center lines, bend extend lines and text will each be assigned to a different layer in the DXF.”

Bend lines are not cut geometry. They tell a press brake operator where to fold. If you leave Center Lines and Extent Lines enabled and send that file to a laser that cuts every closed path it finds, you can get a part with slots cut along every bend.

Turn both off unless your fabricator has explicitly asked for them — many do want them, on a named layer, precisely so they can bend the part. Ask which they prefer rather than guessing. Either way, know what is in the file: because the layers are separate, this is one of the few problems you can actually see by toggling layers in a viewer.

Convert Splines to Polylines

Autodesk’s own guidance is to “use Convert to Polylines if your laser cutter does not support splines.” This is the fix for a whole class of “it opened fine but the cutter refused it” problems.

The tolerance field is the trade-off: it controls how closely the polyline follows the original curve. Too loose and a smooth arc becomes a visibly faceted one; a value well below your kerf is a sensible starting point. If your service accepts splines, leaving the curve intact is usually cleaner.

Units: Fusion behaves better than most, but still check

Both dialogs let you choose the export unit, which puts Fusion ahead of exporters that write a fixed value regardless of your document. The catch is the default: the design’s active unit type. If you modelled in inches and your cutter expects millimetres, the default is the wrong answer and nothing will warn you.

Set it deliberately every time, then confirm in the exported file. Full detail on how this goes wrong: my DXF is the wrong size at the cutter.

Then check the file you are about to send

Not the sketch, not the model — the DXF. Export is where geometry gets flattened, tessellated and re-encoded, so it is entirely possible for the design to be perfect and the file to not be.

You can drop it into the checker on this site, which runs in your browser and never uploads the file — useful when the part belongs to a client.