Bad files are the number one reason orders get delayed. This guide walks through every DXF setting — layers, line types, units, closed paths, kerf compensation — so your file manufactures perfectly on the first attempt.
After processing more than 500 orders at our Yeshwanthpur facility, we've seen every type of file error imaginable. The most common culprits are almost always the same: wrong units, open paths, duplicate lines, and missing layer separation. None of these are design errors — they're all file-preparation errors that could be caught in five minutes before upload.
A bad DXF file doesn't just cause a delay. It can result in wasted sheet material, incorrect cuts that are un-recoverable, and in the worst cases, parts that look right but have geometry that the laser head has to interpret by guessing. This guide will make sure that never happens to your order.
Quick stat: In our DFM analysis, approximately 34% of uploaded DXF files have at least one issue that requires either correction or a manufacturing query. This guide will get you to zero errors.
FYORD's laser cutting machines accept DXF files from AutoCAD R12 through AutoCAD 2024 (AC1032). Our preferred format is DXF R2010 (AC1024) or DXF R2013 (AC1027) — these are universally compatible with our CAM software without requiring any conversion.
Avoid DXF R12 if possible. The R12 format lacks support for lightweight polylines and can cause path-joining issues in some CAM programs. If your software only offers R12, contact us before submitting — we can usually work with it but may need to do cleanup on our end.
Unit errors are responsible for more re-cuts than any other single cause. A file that is designed in millimetres but exported without unit metadata — or exported as inches — will be cut at the wrong scale. The most common scenario: a 200mm bracket gets cut at 200 inches, which is 5.08 metres. The laser doesn't care that it doesn't fit the bed; it will simply error out or, worse, scale the part silently.
Design in millimetres (mm). This is the universal standard for metal fabrication. When exporting, ensure your CAD package embeds the unit definition into the DXF header.
INSUNITS to 4 (Millimetres) before exporting| INSUNITS Value | Unit | Use? |
|---|---|---|
| 0 | Unitless (undefined) | ❌ Avoid |
| 1 | Inches | ❌ Not accepted by default |
| 4 | Millimetres | ✅ Preferred |
| 5 | Centimetres | ❌ Will cause 10× scale error |
| 6 | Metres | ❌ Will cause 1000× scale error |
Layers in DXF files serve two purposes for laser cutting: they communicate intent (cut vs. engrave vs. mark) and they separate geometry so CAM software can assign different process parameters per layer. A well-organised file with clear layer names will always process faster and with fewer errors.
Pro tip: Name your layers with intent (CUT, ENGRAVE, BEND_REF), not with colours (RED, BLUE). Layer names survive file conversion better than colour assignments.
Our CAM software reads the following entity types from DXF files. Everything else is either ignored or may cause import errors.
| Entity Type | Supported? | Notes |
|---|---|---|
| LINE | ✅ Yes | Standard line segment |
| POLYLINE / LWPOLYLINE | ✅ Yes — preferred | Joined paths, the most efficient entity type |
| CIRCLE | ✅ Yes | Holes and round features |
| ARC | ✅ Yes | Curved edges, fillets |
| ELLIPSE | ✅ Yes | Elliptical holes and profiles |
| SPLINE | ✅ Yes (converted) | Converted to arc/line segments; verify output after conversion |
| HATCH | ❌ No | Remove all hatch fills before sending |
| TEXT / MTEXT | ❌ Must be converted | Explode text to paths before exporting |
| BLOCK / INSERT | ❌ Must be exploded | Use "Explode All" before exporting |
| REGION / 3DSOLID | ❌ No | Export the flat 2D face only |
Splines are mathematically complex curves that our CAM software converts to arc/line approximations. If your design has splines, increase the spline-to-arc conversion tolerance in your CAD package to 0.01mm or better. Coarser conversions will create faceting visible on the cut edge, especially on shallow curves.
This is the single most important geometry requirement for laser cutting. Every cut boundary — the outline of your part, every hole, every slot — must be a single, fully-closed path. Open paths create ambiguity about what is inside and what is outside the cut, which causes either a bad cut or a machine alarm.
BOUNDARY command — it will fail or create incorrect regions where paths are open. Use PEDIT → Join to close them.Duplicate lines are as bad as open paths. If two lines perfectly overlap, the laser will make two cuts at the same location — doubling heat input, causing wider kerfs, and burning material unnecessarily. Use your CAD tool's "delete duplicate" or "overkill" command before exporting.
Laser cutting has physical limitations based on the laser spot size and the kerf width. Features smaller than these minimums will either not cut cleanly, will be distorted by heat, or will physically fall out during cutting.
| Feature | Mild Steel | Aluminium | Stainless |
|---|---|---|---|
| Minimum hole diameter | ≥ material thickness | ≥ 1.5× thickness | ≥ 1.2× thickness |
| Minimum slot width | ≥ material thickness | ≥ 1.5× thickness | ≥ 1.2× thickness |
| Minimum bridge/web width | ≥ 2× thickness | ≥ 2.5× thickness | ≥ 2× thickness |
| Minimum part size | 10 × 10 mm | 10 × 10 mm | 10 × 10 mm |
| Minimum inside corner radius | 0.5 mm | 0.5 mm | 0.5 mm |
| Edge-to-edge clearance (nesting) | ≥ 8 mm | ≥ 10 mm | ≥ 8 mm |
Kerf is the material removed by the laser beam during cutting. Our fibre laser has a typical kerf of 0.1–0.3 mm depending on material type and thickness. For most parts, you do not need to compensate for kerf in your file — our CAM software applies an automatic kerf offset.
However, you should compensate for kerf in your file if:
In these cases, offset your inner profiles (holes, slots, internal features) outward by half the kerf (≈ 0.1 mm for most materials on our machine), and offset outer profiles inward by the same amount. Or better — tell us in your order notes that you need tight tolerances, and our engineering team will apply the correct compensation.
Text entities in DXF are not supported by laser CAM software — they are metadata, not geometry. If you want text engraved on your part, you must convert all text to outlines (vector paths) before exporting your DXF.
TXTEXP or EXPLODE to convert text to polylinesFor text that will be cut out (hollow letters), ensure that enclosed areas like the inside of the letter 'O', 'B', 'D', 'P', 'Q', 'R' remain attached to the part with small tabs (bridges) or they will fall away when cut. A tab of 0.5–1mm width is sufficient.
Hatching must be removed. Hatch fills are not a geometric entity — they are a display representation. All hatch entities must be deleted before exporting. Use the "HATCHEDIT" command to remove them in AutoCAD, or simply delete the hatch layer entirely.
Print this or run through it before every file submission:
Use the AUDIT command to detect and fix database errors before exporting. Run -OVERKILL to remove duplicate entities, then BOUNDARY to verify closed regions. Export via SAVEAS → DXF, not via plot/print which may add margins or scaling.
Always unfold your sheet metal part fully before exporting. Use the flat pattern (Flat-Pattern1 in the feature tree). In the DXF/DWG Export Options, set the sheet to the flat pattern view, and export all bend lines as a separate layer. Set decimal precision to 0.001mm.
In the Manufacture workspace, use the Sheet Metal → Save DXF option rather than exporting from the Design workspace directly. This ensures proper flattening with bend allowances applied. Set the sketch tolerance to 0.001mm in the export settings.
Flatten your surface with Unroll or Squish first. Then export via File → Export Selected → .DXF. Set the export scheme to "AutoCAD 2013 Lines" and check "Export open curves" and "Export closed curves." Disable "Export surfaces" and "Export solids."
Inkscape is a graphic design tool, not a CAD tool, but it works reasonably well for simple laser cut files. Key settings: ensure the document units are mm, set the document scale to 1:1 (not 90 dpi or 96 dpi), and use Extensions → Render → DXF Output rather than the built-in DXF exporter, which has known unit issues. Alternatively, export as SVG and we can convert it on our end.
Our automated DFM engine checks your file for all the issues described in this guide — instantly, before you place your order.
Get an Instant Quote →