How to prepare customer drawings for laser cutting

To prepare a customer drawing for laser cutting, first confirm you have the right drawing at the right revision, and read what it asks of the job: material and thickness, quantity, units, finish and the general notes. Then get the part as a clean DXF at 1:1 in millimetres, with closed contours, no doubled lines, every hole in place and nothing else on the cutting layers. Finally, check that geometry against the drawing before it goes into CAM and nesting, where kerf, lead-ins, tabs and the nest are added.

Which file should you ask the customer for?

The one with the least guesswork in it. A native DXF or DWG of the part, or the 3D model, beats a PDF, because nothing has to be recreated. A PDF exported from CAD beats a scan or a photo, because its lines and arcs can be read out rather than traced. Ask for any of them alongside the drawing, at the same revision, never instead of it. If you can’t tell which kind of PDF you’ve been sent, how to tell a vector PDF from a raster one settles it in a minute.

What should you check on the drawing first?

Before anyone touches the geometry, read the drawing for:

• Revision. It matches the RFQ or order, and any DXF or model that came with it is at the same revision.
• Material, grade and thickness. A thickness given as a gauge needs converting with the right table: gauge systems differ, and some vary by material.
• Quantity. Per assembly or in total, and whether any are handed: “1 off as drawn, 1 off opposite hand” means a mirrored part, not two of the same.
• Units. Millimetres or inches, usually stated in the title block.
• The scale note against the dimensions. A scale holds only for the sheet printed at its intended size, and detail views often have their own. If a measured length disagrees with its figure, or the drawing says “do not scale”, work from the written dimensions alone.
• Finish. A coating can change how you cut: oxygen-cut mild steel has an oxide layer on the edge that can affect paint adhesion, so some shops cut parts that will be painted or powder coated with nitrogen.
• Anything “unless otherwise stated”. The general tolerance, edge breaks and notes that apply to every hole. Tapped, countersunk and reamed holes need a second operation after the laser.

If the drawing and a supplied DXF disagree, query it with the customer; PDF vs DXF for fabrication explains why the drawing normally counts.

How do you get the part’s geometry?

It depends on what the customer sent:

• From a native file. A customer’s DXF is often the whole sheet exported, or the part in inches, so strip it back to the part. From a 3D model of a flat part, most CAD programs can export the face as a profile at true size.
• From a PDF exported from CAD. The lines are in the file, but a general converter brings across the whole page at the sheet’s scale; the clean-up is covered in why PDF to DXF converters bring across the whole drawing.
• From a scan or a photo of the drawing. There are no lines to read, so the part is redrawn or traced and sized from the written dimensions. A photo also has to be squared up first, because perspective shrinks the far end of the sheet. See how to convert a scanned PDF to DXF.

Either way, keep the DXF at nominal size. Don’t offset it for the kerf yourself: CAM or the machine does that, and a part offset twice comes out the wrong size.

What should you check in the geometry before CAM?

Whoever made the DXF, check it against the drawing:

1. Every contour is closed. The profile and each hole are single loops whose ends meet exactly. CAM may refuse an open contour, or cut one that never frees the part.
2. No duplicate or overlapping lines. A doubled line looks like one on screen, but may be cut twice, burning the edge, or stop CAM finding the contour. Replace chains of short segments with true arcs too.
3. True size in millimetres. Measure two dimensioned lengths at right angles. A DXF read in inches instead of millimetres, or the reverse, comes in 25.4 times too big or too small.
4. Holes and slots are all there, in the right place. Count them, including any shown only in another view or given only by a note, such as a bolt circle. Check sizes and positions from the datums. A tapped hole may be drawn at the tapping size or the thread’s nominal size, so check which.
5. Small features suit the thickness. The thicker the material, the larger the smallest hole, slot or web that cuts cleanly. Where that limit falls depends on the material, the machine and the assist gas, so use your own shop’s experience; smaller holes may need drilling.
6. Nothing but the part on the cutting layers. No text, dimensions, centre lines or title block, because CAM may try to cut whatever is there. Marking and bend lines go on layers of their own.

What’s left for CAD/CAM and nesting?

Clean geometry is where programming starts. Your CAD/CAM and nesting software then add:

• Kerf compensation. The cut path is offset by half the kerf into the scrap: outside the profile, inside each hole.
• Lead-ins and lead-outs. The pierce is made in the scrap and the beam led onto the contour, so the pierce mark stays off the finished edge.
• Tabs and micro-joints. Small uncut bridges that stop a part tipping up or dropping through the slats. They leave a witness mark, so check which edges can take one.
• Part orientation and grain. Brushed sheet has a direction the drawing may specify, and on bent parts the rolling direction can affect cracking at the bend.
• Nesting. Placing parts on the sheet, and the cut order.

Nest Ready does none of these. Its DXF is the part at true size; kerf, lead-ins and lead-outs, tabs and micro-joints, orientation and nesting are all set in your own software.

What about folded parts?

The drawing shows the formed part, but the laser cuts the flat blank. Its flat pattern depends on bend allowances for the material, thickness and tooling, so it’s best developed, or at least checked, by whoever does the bending; a customer’s flat pattern used the designer’s allowances, not your press brake’s. Keep bend lines on a layer that isn’t cut.

Nest Ready doesn’t make flat patterns from 3D or folded models. Developing the blank stays in your sheet metal CAD.

Where does Nest Ready fit?

Nest Ready is our product, built for the geometry step, so here is what it does and where it stops. You upload drawings as PDF, JPG or PNG, up to 25 MB each and up to 50 files in a batch, and each page is read on its own. On a page exported from CAD, the geometry is read from the PDF and the model chooses which closed outlines are parts. A scan is traced from the pixels, and a photo of a drawing, not of a part, is squared up first; for both, the scale comes from the written dimensions when at least two readings agree, and each part shows its stated accuracy. A part from a scan or photo counts as 5 parts against your allowance.

Anything uncertain is flagged for review. The DXF is R12 with LINE, ARC and CIRCLE only: the outer profile on layer OUTER, holes on INNER, at true size in millimetres, with inch drawings converted and no text or dimensions. How that fits a laser cutting workflow is set out on the laser cutting page.

The limits: review is advisory, so flagged parts you haven’t decided on still download. There’s no free-form editing and no way to add a hole, so a part that needs more is re-run with a note or drawn in CAD. And the checks on the drawing itself, from revision to quantity, are still yours. Check every DXF against the drawing before cutting.

Checklist: preparing a customer drawing for laser cutting

1. Ask for a native file or model, with the drawing, at the same revision.
2. Confirm the revision matches the RFQ or order.
3. Note the material, grade, thickness, quantity and any handed parts.
4. Confirm the units; trust the written dimensions over the scale note.
5. Note the finish, and anything “unless otherwise stated”.
6. Get the part’s geometry at nominal size, with no kerf offset.
7. Check every contour is closed, with no duplicate lines.
8. Check the true size in millimetres in both directions.
9. Check every hole and slot is present, sized and placed.
10. Check small features against the material thickness.
11. Check nothing but the part is on the cutting layers.
12. Develop or check flat patterns for your own tooling.
13. Leave kerf, lead-ins, tabs, orientation and nesting to your CAD/CAM and nesting software.
14. Check every DXF against the drawing before cutting.