A DXF that looks fine on screen can still fail at the machine. The CAM software refuses to generate a toolpath, the part comes out at a quarter of its size, letters lose their centers, or the laser cuts the same line twice and scorches the edge.
Almost all of these come from a handful of file problems. Here's a checklist to run through before you send a DXF to your laser, plasma table or router, or to a cutting shop.
1. Every cut outline is a closed path
CAM software needs to know what's inside and outside each shape. That only works if every outline is a closed loop where the end point meets the start point exactly.
Open paths cause the most trouble: the software may skip the shape, cut it on the wrong side of the line, or refuse to apply an offset. Small gaps are easy to miss because they're invisible at normal zoom.
How to check: most CAD and design programs can select open paths or show path end points. In AutoCAD-style programs, joining lines into a polyline (the JOIN command or PEDIT) will tell you if pieces won't connect. Zoom in on corners where separate lines meet.
2. No duplicate or overlapping lines
Stacked lines are lines drawn on top of each other. They often come from auto-tracing, copying and pasting, or exporting from a program that draws both a fill and a stroke. On screen you see one line. The machine sees two and cuts twice, which wastes time and can burn or widen the edge.
How to check: use a duplicate-removal tool if your software has one (OVERKILL in AutoCAD, for example), or select a line and move it to see if another one is hiding underneath.
3. The units and scale are right
A DXF file stores numbers, and the units those numbers mean aren't always carried along reliably. A part drawn at 12 inches can open as 12 millimeters, or the other way round.
- Decide on inches or millimeters before you start, and draw at full size (1:1).
- Put one known dimension on your notes, like "overall width 18 in", so the person cutting can check it.
- After exporting, re-open the DXF and measure one feature to confirm the size.
4. Text is converted to outlines
If your design has lettering, the cutting machine doesn't know your fonts. Live text may disappear, swap to a default font or show up as single lines. Convert text to outlines or curves before exporting (in Illustrator, Create Outlines; in Inkscape, Object to Path; in CAD, an explode or text-to-geometry command).
5. Letters and islands won't fall out
Cut a letter "O" out of a sheet and the center drops out with it. The same happens with "A", "B", "D", "P", "R" and any logo with enclosed shapes. If you're cutting the letters themselves as parts, that's fine. If you're cutting a stencil or a sign panel where the letters are holes, the centers need bridges: small tabs that keep the inner pieces attached. Stencil fonts are one way to get these; otherwise they're added by hand.
6. Arcs and curves are machine-friendly
Some CAM programs and older controllers handle splines poorly. They may turn them into hundreds of tiny segments that make the machine stutter, or reject them. True arcs and polylines are the safest. If your design software exports splines, check whether your CAM setup has an option to convert them, or ask the shop what they prefer.
Auto-traced images are the worst offenders here: they often produce jagged outlines made of thousands of tiny nodes. Those cut slowly and look rough on the edge. A clean redraw with straight lines and smooth curves cuts better.
7. Small features fit the process
Every cutting process has a minimum feature it can cut cleanly, and it depends on the machine, the material and its thickness. A common starting rule of thumb for metal is to keep holes at least as large as the material is thick, but check with whoever runs the machine. Watch for:
- holes and slots that are too small,
- thin bridges or webs that will warp or burn through,
- inside corners that are too sharp for a router bit (a round bit always leaves a radius).
8. Kerf is handled in one place only
The kerf is the width of material the beam, torch or bit removes. Usually, the CAM software or the machine operator applies the kerf offset. If you also offset the drawing yourself, the part ends up undersized. Draw the part at its finished size unless your shop specifically asks you to offset it, and say which you've done.
9. Layers or colors match what the shop expects
If the job mixes through-cuts, engraving and scoring, separate them by layer or color. There's no universal standard: one shop's red is cut, another's is engrave. Ask, then label your layers plainly, like CUT, ENGRAVE and SCORE.
10. The file is clean
Before exporting:
- remove dimensions, borders, title blocks and notes that aren't meant to be cut (or put them on a clearly named non-cutting layer),
- delete stray points and tiny leftover segments,
- move the part near the origin (0,0),
- save in a widely readable DXF version if your shop's software is older. Many programs let you pick an older version on export.
Quick pre-send checklist
- All cut outlines closed
- No duplicate or stacked lines
- Drawn 1:1, units confirmed by measuring after export
- Text converted to outlines
- Bridges added where islands would fall out
- Arcs or polylines, not jagged auto-trace
- Small holes and webs suit the material
- Kerf left to the CAM/operator (or noted if applied)
- Cut, engrave and score separated by layer or color
- Extras removed, part near the origin
When it's faster to have the file made
If you're starting from a logo image, a phone photo of a part or a sketch on paper, getting to a clean DXF can take longer than the cut itself. That's the work DXF Desk does: we trace images and sketches into closed-path DXF and SVG files, with no double lines, scaled to the measurement you give us. See our cut file services and the two flat prices.
We deliver files; we do not cut the parts, sell material or set your machine's speeds and feeds.
FAQ
Why won't my DXF generate a toolpath?
The most common causes are open paths, duplicate lines or splines your CAM software doesn't handle well. Join the outlines into closed shapes, remove duplicates and try again.
Should I send DXF or SVG?
Use whatever your machine's software imports best. Most laser and CNC software reads DXF; many hobby lasers also read SVG. If you're unsure, send both.
Have a logo or a sketch that needs to become a cut file? Send it with one real measurement, and we'll confirm the price before any work starts.