DXF preparation checklist for a laser cutting RFQ

A DXF that arrives at 1:2 scale with three duplicated lines and a title block sitting on the cut layer will still cut. That is the problem. The laser follows the file it is given, at 16 m/min, and produces a part that is half size, or a contour the operator has already cut twice. The quotation then comes back two days late with a dimension query attached, and the schedule moves.

This DXF preparation checklist is written from the receiving end. Every item on it is something a cutting supplier has to check, redraw or query, and each one has a cost that lands on either the buyer's schedule or the buyer's price.

DXF preparation checklist: what must be true before it goes out?

A 1:1 scale in millimetres, closed contours, no duplicate entities and no kerf offset are four of the ten conditions a file has to meet; a file that meets all ten can be nested and cut without a conversation.

1. Drawn 1:1 in millimetres. No paper space, no viewport scale, no drawing frame.
2. Every contour closed. A gap of 0.01 mm is still a gap, and the CAM has to decide how to close it.
3. No duplicated or overlapping entities. One line, one place, once.
4. No kerf compensation applied. The cut offset belongs to the CAM, not the designer.
5. One part, one outline. Unless the file is a deliberate nest, with parts spaced by at least the web width.
6. Bend lines on a separate, non-cutting layer. Named, so the CAM can ignore them.
7. Splines exploded to arcs or polylines at a sensible tolerance.
8. Text converted to geometry only where it will be cut, and removed everywhere else.
9. Layers named for their function, not left as Layer 0.
10. Filename carrying part number, material, thickness and revision.

What does each DXF error cost at the laser?

The table gives the physical consequence of each fault, not a lecture about CAD standards. Costs are expressed in machine time or in millimetres, so the reader can scale them to their own part.

The duplicate-line row is worth a worked number. Take a 2 mm CRCA bracket with a 1,200 mm total cut. At a planning speed of 10,400 mm/min, the correct file takes 1,200 / 10,400 = 0.115 minutes per part. With one duplicated 1,200 mm contour, the cut becomes 2,400 mm and the time doubles to 0.231 minutes, plus six extra pierces at 0.3 s each, which is 1.8 s or 0.03 minutes. The part now takes 0.26 minutes, 2.3 times the correct cycle, before the second pass has damaged the edge.

Which layers and entities should the file contain?

The CUT, BEND and NOTES layers are enough for most work, and the discipline is worth more than the convention.

CUT carries the closed contours that the laser will follow. Nothing else goes on it, including the part outline dimension lines, which some CAD packages place on the current layer by default.

BEND carries the bend lines as single lines, with the direction noted in the drawing rather than in the geometry. The CAM excludes this layer from cutting and uses it to confirm the flat pattern against the model.

NOTES carries anything the reader needs and the machine does not: revision, material, thickness, quantity and a note about which faces are visible.

Anything else, title blocks, dimension text, hatching, view labels, belongs on the PDF drawing. A DXF is a manufacturing file, not a print.

Splines are the exception that catches experienced designers. A native spline exports as a curve, and the CAM flattens it at a chord tolerance. On a 150 mm radius arc covering a quarter turn, the arc length is 236 mm. Flattening at 0.01 mm sagitta gives segments of 2 × √(2 × 150 × 0.01) = 3.46 mm, which is 68 segments. Flattening at 0.1 mm gives 10.95 mm segments, which is 22. The cut length is nearly the same, but each short segment costs an acceleration, and on thin sheet that shows as dross at every vertex.

Should the DXF be the flat pattern or the formed model?

The DXF must be the flat pattern, because that is what the laser cuts; the formed model goes separately as STEP. The distinction matters when the part has bends, because the flat pattern carries the bend deduction from the K-factor and radius chosen in the CAD model, and a K-factor that does not match the press brake tooling forms the wrong part from a correct cut. A flat blank needs the DXF alone; a part with four bends and a ±0.5 mm flange height needs both, with the inside radius stated on the drawing. The STEP files for bend review guide covers how the two are reconciled.

What Ganesh checks on receipt

Every cutting enquiry is checked for geometry before it reaches the nest. The check covers units and scale, open contours, duplicate entities, contour count against the drawing, minimum web, hole size against thickness and whether the bend lines match the flat pattern.

Where a file fails, the query goes back with the specific entity marked, not a general request to resend. That is faster for both sides: a file with one open contour is a two-minute fix, and a file with a systematic scale error needs a re-export.

Ganesh cuts mild steel, CRCA, stainless, aluminium, brass and copper from 0.8 mm to 20 mm on the 12 kW fibre laser, and handles 30–40 mm plate work on the iron worker. The plants hold ISO 9001:2015 and ISO 14001:2015. The laser cutting capability page lists the machine and material scope, and the laser cutting and fabrication hub collects the related tolerance, nesting and edge guides.

What does a redrawn DXF cost in time?

More than the cutting, on a small order, and almost nothing on a large one.

A bracket with 20 features is a 20–30 minute redraw. A canopy panel with 60 features, a louvre pattern and four bend lines is 2–4 hours of engineering, plus a query cycle that costs a working day each way. Call it 45 minutes and two days for the bracket.

Compare that to the cut. The 2 mm bracket from the worked example above takes 0.26 minutes of machine time per part. At 200 parts, 45 minutes of redraw is 13.5 seconds per part, which is nearly a whole cutting cycle added to every unit. At 5,000 parts the same 45 minutes is 0.54 seconds per part, and the redraw disappears into the setup.

The decision rule follows: if the part will run once, a redraw may be the fastest route to a quote. If it will run for a year, fix the file at source and re-issue it, because the redraw has to be approved, revision-controlled and repeated for every subsequent change. A file that is rebuilt at the supplier is a file the customer no longer owns.

How should a multi-part nest be sent?

Send it only if you are sending a deliberate nest, and state the rules with it.

The web between parts is the first rule. Below about 2 mm the part can move as the cut progresses, and a moving part produces a stepped edge and, occasionally, a head collision. The practical minimum is 3–5 mm on thin sheet, widening to 8 mm on 6 mm plate. A nest drawn with 1 mm webs on 3 mm plate will be rejected, and re-nesting it costs the same engineering time as drawing it again.

Rotation, rolling direction, common-line cutting and mixed thickness are the four other things the covering note should settle:

• Rotation allowed or not. Rotation is usually fine, but not on a part with a visible brushed grain direction.
• Grain or rolling direction, if the part is formed or visible.
• Common-line cutting, where two parts share an edge. It saves one kerf per pair, but it couples the parts: if one drops, the other loses its edge. Agree it explicitly.
• Mixed thickness. Do not mix gauges in one nest file. The laser cuts one thickness at a time, and a nest with two gauges splits into two jobs with two quotes.

If the nest is not deliberate, send one part per file. A supplier can nest a single part more efficiently than a customer can guess, because the supplier knows the sheet sizes, the remnant stock and which other jobs are running the same week.

How should the file be named and sent?

Name the file for the part, not for the project. A filename such as GM-4471-BRKT-REV-C-CRCA-2.0mm-DXF.dxf tells the receiving engineer four things before the file opens, and it survives being attached to an email that gets forwarded three times.

Include in the covering email:

• Part number, revision and quantity, split by release if there is a schedule.
• Material grade and actual thickness in millimetres.
• Any tolerance tighter than ±0.5 mm, on the specific feature.
• Edge requirement: burr limit, deburred or as-cut.
• Whether the part is formed after cutting, and on which machine if known.
• Delivery destination, because packing for a long panel differs from packing for a bracket.

Send the files for a geometry check against the drawing. The DXF RFQ checklist resource is the same list in a form the design team can sign off before release, and the laser cutting cost estimator gives an indicative machine cost once the cut length and pierce count are known.

When a DXF is the wrong format

For a part with a formed feature that cannot be described by a flat outline, a deep drawn cup, a coining, a louvre, a DXF is not enough on its own. The cut is one operation in a chain, and the drawing has to carry the rest.

For a part that will be pressed rather than cut, the flat pattern is a tool design output, not a customer input. Sending a DXF invites a laser quote for a part that should be stamped, and the piece price will be wrong by an order of magnitude at volume. The guide to choosing laser cutting for a new part sets out when the cut route is the right first answer and when it is not.

And for a part with a hole smaller than the material thickness, the DXF will be cut, but the hole will taper and may need drilling afterwards. That is a design decision, not a file decision. The holes, slots and small features guide gives the ratios that hold on a fibre laser.