How to Prepare a DXF File for Plasma Cutting.

Most files that fail here fail for one of four reasons, and all four are quick to fix once you can see them. This guide shows each one.

What a DXF is, and why cutting runs on it

DXF (Drawing Exchange Format) was published by Autodesk in the early 1980s as an open way to move 2D geometry between CAD applications. It stores lines, arcs, splines and polylines as exact coordinates — no proprietary structures, no software lock-in. That openness is why CNC manufacturing still runs on it: any CAD program can write one, and any cutting software can read one.

When you upload a DXF to Can-Cut, our parser reads the geometry, measures cut length and pierce count, nests the part and prices it — in a few seconds, with no human in the loop. Everything below is about giving that parser something it can read.

Software that exports DXF

• Fusion 360 — exports DXF straight from the Sketch environment
• AutoCAD / LT — native DXF in any version
• SolidWorks — export the flat face or flat pattern, not the 3D body
• Onshape — free for hobbyists; DXF from any sketch or face
• Inkscape (free) — DXF via Save As, good for artwork
• Adobe Illustrator — DXF via Export As
• QCAD / LibreCAD (free) — purpose-built 2D CAD

No CAD at all? Skip to the Drawing Board.

Rule one: every path must be closed

This is the single most common reason a file is refused.

A closed path is a loop with no gap — the last segment ends exactly where the first began. The cutter uses that loop to work out what is inside the part and what is outside. An open path leaves that undecidable, so the file is rejected before it can be priced.

The gap is almost never visible. It is typically a few thousandths of an inch, invisible at drawing zoom, which is exactly why it survives to export. Usual causes:

• Snap tolerance set too loose, leaving a hair gap at a junction
• Geometry copied and nudged, leaving near-coincident but unjoined endpoints
• Imported from SVG, DWG or PDF, which did not preserve connectivity

Every CAD tool has a fix. In Fusion 360, open sketch profiles will not shade — if the interior is not filled, it is not closed. In AutoCAD, PEDIT > Join, or OVERKILL to clean duplicates first. In QCAD, use the polyline join tool.

Rule two: features have to be bigger than the kerf

Plasma does not cut a line — it removes a channel of metal roughly 0.060″ to 0.090″ wide, called the kerf. Anything narrower than that has nothing left once both edges are cut. A 1/16″ hole in 1/4″ plate does not come out small; it does not come out at all.

Working rules:

• Holes: diameter at least equal to the material thickness
• Slots: width at least 1.5× the thickness
• Webs and tabs: thinner than the material will warp from heat even if it survives

A note on honesty here: our uploader does not automatically reject small features. It will price and cut them. If your part depends on a fine detail, tell us before you order and we will tell you whether it will survive.

Rule three: text must be outlines, not text

A TEXT entity in a DXF is a reference to a font — a string, a height, a style name. It contains no geometry, so there is nothing for the torch to follow. It has to be converted to curves before export.

If it is stored as text rather than geometry, we do not cut it. We cannot: the shapes of the letters are not in your file. Your font lives on your computer, not inside the DXF, so there is nothing for us to convert on your behalf and nothing to guess from.

This does not come back as an error, and that is the part to watch for. We quote whatever real geometry the file does contain. If your design is a plate with a name on it, the plate is real geometry and the name is not — so you will get a normal-looking price, for a blank plate. Nothing warns you.

So check the preview. After you upload, the preview shows exactly what the torch will follow. If your lettering is not in the preview, it is not in your file, and it will not be in the metal. Convert it to outlines and upload again.

• Fusion 360 — right-click the sketch text → Explode Text
• Illustrator / Inkscape — Type → Create Outlines / Path → Object to Path
• AutoCAD — TXTEXP, then join the results into polylines

Then there is the second problem, which catches people out after they have done the first. Once letters are outlines, the middles of A, B, D, O, P, R, 4, 6, 8, 9 are separate closed loops inside the letter. Cut them and those centres fall out as loose slugs. If you want the letter to read, use a stencil face, where bridges hold the centres in place.

Our Drawing Board has a text tool with 8 stencil faces for this reason, and it warns you on screen when the face you picked would drop its centres.

Rule four: get the units right

DXF stores numbers, not sizes. Whether 10 means ten inches or ten millimetres is carried by the $INSUNITS header variable — and plenty of exporters leave it unset.

Our parser reads $INSUNITS (1 = inches, 4 = millimetres). When it is missing or ambiguous, we ask you rather than guessing, because guessing wrong here is a 25.4× error in either direction. If a part quotes at an absurd size or an absurd price, units are almost always the reason. You can correct the unit on the part itself without re-uploading.

How big can it be?

Anything up to 48″ × 96″ quotes automatically online. Between that and 60″ × 120″ we can still cut it, but it needs a manual quote — the uploader will tell you so and point you at the contact form rather than just refusing. Past 60″ × 120″ is genuinely beyond the table.

Leave roughly 0.5″ of margin: parts are nested with a gap around them, not cut edge to edge.

Things that are fine

Worth saying explicitly, because people ask:

• Holes inside your part. Completely normal. Each one is a separate closed loop inside the outer profile, pierced and cut on its own. More holes means more pierces and a slightly higher price, nothing more.
• Several parts in one file. We split them automatically and list them as separate line items, each with its own quantity.
• Parts on different layers. When parts sit on two or more layers, we let you import one layer at a time — useful when your drawing uses layers for different thicknesses.
• Splines and arcs. Fully supported; no need to convert them to line segments.

What we cannot cut from

• A 3D model. STEP, IGES, SLDPRT and 3D DWG describe a solid, not a flat profile. Export the flat face — or, if the part has bends, send us the drawing and we will quote it manually.
• A picture. JPG, PNG, PDF and scans contain pixels, not geometry. Tracing a photo produces jagged edges that scale up with the part.
• A cut program. A DXF whose layers are named Cut and Rapid Move is a toolpath export, with lead-ins and travel moves that do not form closed loops. Export the part geometry instead.

If any of those describe your file, use the no-drawing form — send whatever you have and a person will work it out with you.

No CAD software? Draw it in your browser

The Can-Cut Drawing Board is free, needs no account and runs in the browser. Lines, polylines, curves, rectangles, circles, ellipses, a break tool for trimming arcs, a measure tool, and text in 40 fonts. You can import a photo as a tracing backdrop and set its scale from a known dimension.

It will not let you export until the geometry is actually closed, which means anything it produces will price on the first try.

What happens when you upload

1. Every closed loop is found and checked — open ends and crossings are reported per part
2. Multi-part files are split, and layers offered if there are several
3. The bounding box is measured against the table
4. Cut length and pierce count are computed for pricing
5. The part is drawn back to you at its true size, so you can confirm the scale before you pay

Anything we cannot use is explained in plain language on the part itself, with the fix, before you reach checkout.

Ready?

Upload your DXF for an instant price — no account needed. Most files go from upload to priced quote in under a minute.