Preparing artwork for the table
Getting a DXF out of an image is the easy part. Getting one that cuts cleanly on the first try is about understanding what the machine does to your geometry.
1. Start with the right image
The tracer finds the boundary between light and dark. So the question to ask of any source image is: is there one brightness value that separates what I want to keep from what I want to remove? If yes, this will take two minutes. If no, no amount of adjustment will help, see the examples page for what that looks like in practice.
Aim for 1000–2000 pixels on the long edge. Below that, curves come out faceted. Above 2000 the tool downsamples anyway, since more pixels past that point add tracing time without adding real detail.
2. Set the threshold
Press Auto first. That runs Otsu's method, which picks the value that best separates the image into two groups, and on clean artwork it is almost always right. Switch to the Threshold view to see what you actually selected before you look at any paths.
If your artwork is light-on-dark rather than dark-on-light, tick Invert selection. If the edges look ragged or speckled, raise Denoise by one. Do not reach for denoise to fix a contrast problem, it blurs detail away and the underlying problem remains.
3. Account for kerf
Your torch, laser, or jet removes material as it travels. That width is the kerf: about 1.5 mm on a hand plasma, 0.8 mm on a fine-cut consumable, 0.1 mm on a laser, and 0.8–1.2 mm on waterjet. Cut exactly on your outline and the finished part comes out half a kerf undersize all the way round.
Most CAM software applies kerf compensation for you, and if yours does, let it — it knows the tool. Use Thicken outer edges here only when your CAM cannot compensate, or when you want the artwork itself heavier for visual reasons.
Positive always means more material. Thicken outer edges pushes the silhouette outward; Thicken hole edges shrinks the holes. Both directions add material, which is why they are labelled separately rather than as one signed offset.
4. Enforce what the machine can actually cut
Two independent limits matter, and they fail in opposite directions.
Minimum metal width is the narrowest strip of material that survives the heat. On thin plasma-cut steel, anything under about 3 mm warps, discolours, or burns away. Ticking Enforce min. material width grows only the strips that are already too thin; a shape with a solid core is left exactly as it was, so squares stay square.
Minimum cut width is the opposite problem: the narrowest slot the tool can fit into. Try to cut a 0.5 mm vein with a 1.5 mm kerf and the two walls merge into one cut, and the detail disappears. Enforce min. cut width widens those slots so they survive.
Set both to your kerf plus a margin. For hand plasma on 3 mm mild steel, 3 mm for each is a sensible starting point.
5. Deal with loose pieces
The middle of an O, the triangle inside an A, an island in the centre of a ring, any material fully surrounded by a cut falls through the slats the moment that cut completes. The tool outlines these in red and counts them in the Loose pieces readout.
You have three options. Bridge it with the Keep brush, which is what a sign shop does, a small tab connecting the island to the surrounding material. Delete the surrounding hole with the Pick tool so it is never cut. Or accept it, and plan to weld the piece back in afterwards.
A loose piece is not a bug in the trace. It is a real physical consequence of the geometry, and it will happen on the table whether or not the software warns you. Decide about it now rather than when you are picking parts out of the water tray.
6. Simplify and smooth
A raw trace of a 2000 px image can carry tens of thousands of vertices, and every one is a deceleration point for the motion controller. Simplify removes vertices that sit within a tolerance of the line they lie on. At 0.8 px the change is invisible and the vertex count typically drops by an order of magnitude.
Corner radius replaces sharp corners with tangent arcs. Beyond looking better, it lets the machine hold feed rate through the corner instead of stopping dead, which reduces the dwell mark plasma leaves at a hard direction change.
Leave Fit arcs & merge lines on. It collapses straight runs into single line segments and true curves into real arcs stored as DXF bulges, so a circle arrives in CAM as an arc rather than a 400-segment polygon. Files get smaller and toolpaths get smoother.
7. Set the size, then export
Enter the finished width in millimetres or inches; the height follows automatically since the aspect ratio is locked. The Cut length readout then tells you the total distance the torch will travel, which is the number to multiply by your feed rate when you are quoting a job.
Tick Mirror if you are cutting face-down. Then export.
What you get
A DXF R12 file: closed polylines on layer 0, arcs stored as bulge values, outer boundaries wound counter-clockwise and holes clockwise. R12 is deliberately the oldest and dumbest DXF revision, because it is the one every CAM package, sign-cutting program, and machine controller reads without complaint.
The winding convention matters more than it sounds: it is how CAM tells a hole from an outline, and therefore which side of the line to put the kerf on. Getting it wrong makes every hole in the part come out oversize.
Common questions
Which software opens these files?
Anything that reads DXF: Fusion 360, SheetCam, FastCAM, LightBurn, Lightning CNC, SolidWorks, AutoCAD, Inkscape, QCAD, Torchmate, plus the controllers built into most tables. R12 is the universal denominator.
Can it trace a photograph of a person?
Not usefully, not directly. A photograph is continuous tone and the tracer needs a hard edge. What people actually do is reduce the photo to a two-tone stencil first , in an image editor, or with a pen tool, and trace that. The stencil is where the artistic judgement lives, and no automatic threshold replaces it.
Does my image get uploaded?
The image never leaves your browser. Tracing happens locally on your own machine, which is why it is instant. Only the finished outline coordinates and file name are sent, and only at the moment you export a file.
Why is my part a bit undersized?
Almost always kerf compensation, either applied twice or not at all. Check whether your CAM is already offsetting for the tool before you add any thickening here.
What does "pierces" mean?
One per closed path, every separate loop needs its own pierce. Pierces are the slowest and most consumable-hungry part of a plasma cut, so the count is a good proxy for how long a job will take and what it will cost in tips and electrodes.