Key takeaways
- A cut DXF needs three layers: CUT for closed contours, BEND for bend lines that must never be cut, and TEXT or DIM for annotation. A bend line on the cut layer splits the part in half.
- Save at 1:1 in millimetres with the header unit set to millimetres. A 2:1 export cuts a part at double size and passes every visual check.
- Keep contour gaps under 0.01 mm. A 0.1 mm gap on a 2 mm contour is larger than the 0.2 mm kerf allows and the nesting software treats the profile as open.
- Draw the part at nominal size. Kerf of 0.2–0.3 mm is compensated in CAM; a DXF already offset by the designer is compensated twice and the hole comes out 0.4 mm small.
A flat pattern with a 0.1 mm gap at one corner looks perfect on screen. On the nesting table it is an open contour: the laser cuts to the gap, stops, and either leaves the part attached to the skeleton or re-pierces on the other side and leaves a 0.1 mm tab that nobody will find until the blank is bent.
DXF files for sheet metal are cutting instructions, and they are read by software that has no judgement. It finds closed contours and nests them, finds open contours and either rejects the file or cuts a profile nobody intended. The three things that decide which of those happens are layer structure, units and scale, and whether each contour closes.
This page covers the file itself. The wider submission checklist — what to attach to an RFQ, what else the drawing has to say — sits in the DXF preparation checklist, and this page assumes you have already decided to send a DXF rather than a STEP.
What does a nesting software actually read from a DXF?
It reads geometry by layer, in drawing units, and it needs each profile to form one closed loop. Nothing else in the file affects the cut.
The DXF format stores entities — lines, arcs, polylines, splines, text — each with a layer name, a colour and a position. A nesting system is typically configured to take the cut layer, sort the entities into closed loops, apply kerf compensation, nest the loops on a sheet and post the tool path. Anything it cannot close becomes an error or a manual fix.
That is why a DXF that is beautiful in a viewer can be unusable in CAM. The viewer draws overlapping lines and small gaps as if they were solid; the nesting software measures them.
The layer split that survives nesting
Three layers cover almost every flat part. More layers are fine, as long as every one has a defined role and the role is stated.
| Layer | Contents | Failure if it is wrong | Ganesh handling |
|---|---|---|---|
| CUT | Closed outer profile and every internal contour | An open contour stops the nest or cuts a tab | Every loop checked for closure before nesting |
| BEND | Bend lines as single centre-line segments | A bend line cut as geometry splits the part in two | Bends are re-placed from the formed model, never cut |
| TEXT / DIM | Part number, revision, material note, dimensions | Text on the cut layer is cut as a thin slot | Text is read, then excluded from the nest |
| ETCH | Marking or part number that must be engraved | An etch line on CUT becomes a through-cut | Engraved only when the drawing calls for it |
The bend line failure is the expensive one and it happens more often than it should. A designer draws the flat pattern in a 2D package, puts the bend lines on the same layer as the outline because that is how it looked right, and sends it. The laser cuts four neat lines across the middle of the panel. The cut is fast, the blank is scrap, and the mistake is invisible in every screenshot.
Colour is not a reliable layer signal. Plot styles differ between companies and a red line means a cut edge in one drawing office and a centre line in another. The layer name is what survives translation, so name the layers in words the receiving shop will recognise.
Units and scale: two checks that catch most bad files
A DXF has no enforced unit. The header can hold a unit code, and files written by R13 and later normally do: value 4 means millimetres, value 1 means inches. Many exporters leave the code at 0, which means unitless, and the nesting software then applies a default that may not be yours.
The scale error that follows is either catastrophic or subtle. An inch file read as millimetres cuts a part 25.4 times too small, which is obvious on the first blank. A drawing exported from a scaled paper-space view at 2:1 cuts a part at double size and consumes four times the sheet area, and the only clue is the number on the title block.
Two checks close the gap. Set the unit code in the header if your exporter allows it, and put the size on the drawing so the shop can compare an overall dimension to the cut blank. A 620 mm panel that arrives 1,240 mm long is a scale fault, not a nesting fault.
Coordinates should also be sensible. A flat pattern sitting 1,200 mm from the origin still nests, but it wastes preview time and it confuses the comparison against the drawing. Move the profile to the origin with the lower-left corner at 0,0, and keep the part inside positive coordinates.
Closed contours: the 0.01 mm that decides a cut
A contour closes when the last endpoint coincides with the first. In practice the tolerance is set by the receiving system; treat 0.01 mm as the working limit, because a gap smaller than that is bridged by the software and a gap larger is not.
The gap has three common causes. Geometry snapped by eye instead of by an endpoint object leaves 0.02–0.5 mm of air. A fillet applied after the outline was drawn can leave a short straight segment overlapping the arc. A contour copied and moved leaves a duplicate underneath, and the duplicate is read as a zero-width sliver that the loop-finding routine cannot resolve.
| Fault | Typical size | What the software does | What the blank shows |
|---|---|---|---|
| Endpoint gap | 0.02–0.5 mm | Reads the profile as open | Tab or unburnt bridge at the gap |
| Duplicate entity | 0 mm apart | Two passes on one line | Doubled heat input, dross, rounded edge |
| Overlapping arcs | 0.1–0.3 mm | Loop fails or self-intersects | Witness mark and a burr at the joint |
| Self-intersecting contour | Any | Rejected, or cut twice at the crossing | Slot burned wider at the crossing |
| Spline exploded into arcs | 0.01–0.1 mm step | Loop closes, shape is faceted | Out-of-round hole, flat spots on a radius |
Duplicate entities deserve a paragraph of their own. A line cut twice receives roughly twice the energy in the same place. On 2 mm mild steel that shows as a widened kerf, heavy dross on the underside and a rounded top edge, and it doubles the cut time on that feature. Remove duplicates with an overkill or purge command before sending, and check for them after any copy-and-paste operation.
Splines, arcs and the hole that comes out out-of-round
A true arc costs the controller nothing and cuts as a circle. A spline converted to a polyline does not. If a Ø10 mm hole is exported as 16 straight segments, the sagitta — the distance from the chord to the true circle — is R × (1 − cos(180°/N)). With R = 5 mm and N = 16, that is 5 × (1 − cos 11.25°) = 0.096 mm.
Nearly a tenth of a millimetre of out-of-round on a hole that may be a locating feature. The part still passes a ±0.5 mm general tolerance, so nobody flags it. It fails when the hole takes an M8 bolt through a 9 mm clearance and the assembly jig needs the hole centred, or when the hole is a dowel location.
Export from the native sketch rather than from an exploded view, keep arcs as arcs, and if a spline must be used, set the export deviation to 0.01 mm or finer. A 0.01 mm deviation on a Ø10 hole needs about 50 segments and adds a few kilobytes — a cheap trade against a rejected first article.
Kerf belongs in CAM, not in the DXF
The laser removes material. On 2 mm mild steel the kerf is roughly 0.2–0.3 mm depending on the nozzle, the gas and the power; the CAM system offsets the tool path by half the kerf so the finished hole is the size on the drawing.
If the DXF already contains that offset, the offset is applied twice. A designer who offsets a Ø10 mm hole outward by 0.2 mm to "allow for the beam" hands over a Ø10.4 mm circle, which the CAM then trims by 0.2 mm to Ø10.2 mm, or in the other direction to Ø9.8 mm, depending on the sign convention. Either way the hole is wrong by a few tenths and the error repeats on every feature.
Draw the finished part. State the grade and thickness so the CAM can pick the right kerf. If a fit needs a specific clearance, put the clearance in the hole size on the drawing, where it is visible and reviewable, rather than in the DXF geometry.
The edge condition is a separate call-out. ISO 9013 classifies thermal cuts by dimensional and surface quality, which is the language to use when a visible edge has to meet a standard: state the class and the inspection applies to the cut edge, rather than describing it as "clean".
How many DXF files for sheet metal does one part need?
One per part number, unless you are sending a nest you have already frozen. A file holding six different blanks on one sheet cannot be quoted per piece without a manual sort, and the six blanks share a layer, so nobody can tell which profile belongs to which part number.
A customer-supplied nest is legitimate for a single-part, repeat order where the sheet size is fixed by contract. It becomes a problem when it locks the shop to your sheet size rather than the one on the rack. Ganesh nests on the 12 kW machine's 40 ft × 16 ft bed and on standard sheets, and a supplied nest built for a 1,250 × 2,500 mm sheet will not use the bed any better than the CAM system can.
The spacing rule matters more than most designers expect. Parts need 5–8 mm between profiles to hold the skeleton together, and a lead-in needs 2–3 mm of clear material before the contour. A nest drawn at 2 mm spacing cuts, but the skeleton flexes and the last parts on the sheet slide, which shows up as a burr on one edge and a witness mark on the face.
File naming is the last of the practical rules. Put the part number, the revision and the material in the name: GM-4412-B-2mm-CRCA.dxf tells the intake desk everything it needs before the file is opened. Drawing1.dxf tells it nothing, and in a batch of forty attachments the wrong revision gets cut.
How Ganesh handles a DXF before it is nested
Files are accepted as PDF, DXF, DWG and STEP. A DXF goes through the same intake for every part: units and scale confirmed against the drawing envelope, layer names mapped to cut and non-cut, every loop checked for closure and duplicates, and the profile compared against the formed model where one exists.
Cutting runs on a 12 kW fibre laser with a 40 ft × 16 ft bed, supported by two 6 kW and two 3 kW machines, on mild steel, CRCA, stainless, aluminium, brass and copper, up to 20 mm plate. The large bed matters for long parts because a 4,450 mm panel is cut in one nesting without a re-index.
Laser-cut parts hold ±0.5 mm as the typical sheet metal tolerance, with tighter features agreed against the drawing. Manufacturing has run since 1992 across five units in Mumbai (Vasai) and Nagpur, under ISO 9001:2015 and ISO 14001:2015, with PPAP and first article inspection available. The laser cutting tolerances page covers what the process holds feature by feature, and the laser cutting capability page lists the machines and the thickness range.
What to check before the DXF leaves your desk
- Layer names: CUT, BEND, TEXT, ETCH. No bend line on CUT.
- Unit code in the header, or the unit in the file name. Millimetres for Indian and most export work.
- Scale 1:1. Compare an overall dimension against the drawing before sending.
- Every loop closed to under 0.01 mm, with duplicates removed.
- Arcs kept as arcs, spline deviation 0.01 mm or finer.
- Kerf not applied. Nominal geometry only.
- Grade, thickness and finish in the accompanying note, even when the file name already says them.
The DXF RFQ checklist resource turns this into a one-page form the drawing office can tick before release.
When a DXF is the wrong handover
A DXF describes a flat shape and nothing else. It cannot say whether two flanges collide, whether a punch clears a return flange, or whether a hole lands on a bend radius after forming. For any part with a bend, the formed model is the controlling geometry and the DXF is the cutting intent; the STEP handover guide covers what the model has to carry.
It is also the wrong file when the part is a weldment made from several plates. Six DXFs with no assembly drawing describe six blanks and no weld sequence, and the sequence is what decides whether the frame squares up. And a DXF cannot carry a datum scheme, so a part inspected in a checking fixture needs the drawing regardless of how clean the cut file is.
Send the DXF, the drawing revision and the grade when the part is flat, and add the STEP when it is formed. Request a quote with the files attached, and the design and CAD hub indexes the rest of the handover guides.
Frequently asked questions
What layers should a sheet metal DXF have?
Three at minimum: CUT for the closed outer and inner contours, BEND for the bend lines, and TEXT or DIM for anything a human needs to read. Bend lines must sit on their own layer, because nesting software cuts everything it finds on the cut layer.
Does a DXF carry units?
The DXF header can carry a unit setting, and R13 and later files normally write it, with millimetres recorded as value 4. Many exporters leave it at unitless, so the receiving software falls back to a default. State the unit in the file name or the accompanying drawing as well.
Why does the nesting software say my contour is open?
Almost always a gap where two entities should meet, a duplicate segment that the software reads as a zero-width sliver, or a spline that was exploded into a chain of arcs with a step between them. Zoom to each intersection and check the endpoints coincide to under 0.01 mm.
Should the DXF include the laser kerf?
No. Draw the finished part size. The kerf is 0.2–0.3 mm on 2 mm mild steel and the CAM system offsets the tool path by half of it. A file that already contains the offset is compensated again and every hole lands undersize.
Can I send a DXF instead of a drawing?
For a flat cut-only part, a clean DXF plus grade, thickness and finish is enough to quote and cut. For anything formed, welded or inspected against datums, the DXF is a cutting file and the drawing or STEP model carries the intent.
Sources and further reading
- ISO 9013:2017 — Thermal cutting: classification of thermal cuts, the quality classes a laser-cut edge is specified against · reviewed 3 Nov 2026
- ISO 2768-1 — General tolerances for linear and angular dimensions where the drawing gives no individual tolerance · reviewed 3 Nov 2026
- IS 513 Part 1 — Cold reduced carbon steel sheets and strips, the grade and thickness basis for a cut blank · reviewed 3 Nov 2026
Send the DXF and we will cut a first article
Attach the DXF, the grade and thickness, and the drawing if the part is formed. We check contour closure and units before nesting, and report anything that would cut open.
Request a quote