DXF preparation for laser and plasma cutting: a checklist

Every laser and plasma shop has a folder of DXF files that could not be cut as received: drawn at the wrong scale, with open contours, duplicated lines, a title block in the middle of the nest. Each one costs a phone call and a day. This checklist is what we check before a DXF leaves our hands.

The checklist

Geometry

1. Scale 1:1 and the unit stated in the file name or the order (mm or inch). Do not rely on the DXF header units; many importers ignore them.
2. Closed contours only. Every outer profile and every hole is a closed loop. Gaps of a few hundredths of a millimetre stop the CAM from recognising a part.
3. No duplicate or overlapping entities. Lines drawn twice get cut twice, burning or widening the kerf.
4. No zero-length entities or stray points.
5. Arcs and polylines instead of splines where possible. Some machines and nesting tools convert splines into many tiny segments, which slows cutting and roughens edges.
6. The finished part geometry, not the toolpath: no kerf offset, no lead-ins or tabs, unless the shop asks for them.

Layers and content

7. One layer for cut geometry. Nothing else on it.
8. Engraving or marking on its own layer, named clearly (for example ETCH). Text to be marked should be exploded to geometry or use a single-line font the shop supports.
9. Bend lines on their own layer (for example BEND), never on the cut layer.
10. No dimensions, notes, title block or border in the DXF. Put those on a matching PDF drawing.

Manufacturability

11. Holes and slots large enough for the process. As a starting rule, laser holes no smaller than the material thickness, and plasma holes about 1.5 times the thickness; ask your shop for its limits.
12. Web widths between holes and to the edge that will not distort or burn through.
13. Relief cuts at bends where flanges meet, if the part will be bent.
14. Grain or finish direction marked on the PDF when it matters (brushed stainless, bending across the grain).

File handling

15. One part per file, unless the shop asks for nests.
16. File name with the essentials: part number, revision, material, thickness, quantity. For example PN1042_revC_S235_3mm_qty20.dxf.
17. DXF version the shop can import (ask; older versions are the safest).
18. A matching PDF with dimensions, bend directions and angles, tolerances and finish.

Flat patterns from 3D models

If the DXF is unfolded from a sheet-metal model, the flat size depends on the bend allowance or K-factor used. Shops calibrate these for their own press brakes and tooling. Two options work:

• Use the shop’s values. Ask for their K-factor or bend table per material and thickness and set the model to it before exporting.
• Send the 3D model too. Let the shop unfold with its own settings, and use your DXF only as a reference.

What does not work is a flat pattern made with a default K-factor and no mention of it, followed by bent parts that come out a millimetre short.

What goes wrong most often?

When a shop sends a DXF back, the reason is usually one of these:

Problem	What the shop sees	Fix
Wrong scale or units	Part 25.4 times too big or too small	Export 1:1, state the unit
Open contour	CAM cannot create a part from it	Join entities, check with a closed-loop tool
Duplicate lines	Edge cut twice, burned or wider	Run overkill or delete duplicates
Dimensions on the cut layer	Text and arrows cut into the plate	Keep dimensions on the PDF only
Splines	Thousands of tiny segments, rough edge	Convert to arcs and lines
Bend lines on the cut layer	Part cut in half along the bend	Move to a BEND layer

Exporting from SolidWorks sheet metal

When the DXF comes from a sheet-metal part, export the flat pattern directly rather than drawing a view and exporting the drawing. In the export dialog, choose to include only the geometry you need (outer profile, interior features, bend lines on their own layer) and exclude sketches, library features and annotations. Check the export options for splines, and set the DXF version the shop asked for. Save these settings so every export in the team behaves the same.

Laser versus plasma: what changes in the file

The file rules are the same; the process limits are not. Plasma has a wider kerf and a larger heat-affected zone, so small holes come out tapered and imprecise, sharp internal corners round off more, and narrow webs distort. For plasma, give holes that must be precise a note on the PDF (“drill/ream after cutting”) and draw them at the nominal size anyway, so the shop can mark the position. For laser, small holes and fine features are more reliable, but very thick material still limits them. Either way, your shop’s parameter tables beat any generic rule.

Marking and engraving

Part numbers marked on the part save time in assembly and in the warehouse. Put the marking on its own layer, use a single-line font or geometry the shop’s software can process, and size it for the process (laser marking can be small; plasma marking needs larger, simpler characters). State on the PDF whether marking is on the visible face or the back.

Nesting considerations you can help with

You do not have to nest parts yourself, but you can make nesting easier: send the grain or brushing direction when it matters, say whether parts can be rotated, and give the quantity per order rather than per year. Parts that can rotate freely nest more tightly, which lowers the material cost on the quote.

Before you hit send

Open the DXF in a free viewer or a fresh CAD session and check: does it import at the right size, are all contours closed, is there anything on the cut layer that should not be cut? Two minutes of checking saves the shop a call and you a day.