What makes a DXF ready for laser cutting?

A DXF is ready for laser cutting when CAM can read every contour in it as a closed path to cut, and finds nothing else. That means the outer profile and each hole are single closed loops whose ends meet exactly; nothing is drawn twice, overlaps or has zero length; curves are true arcs and circles; every hole sits wholly inside the profile; the part is at true size in known units, usually millimetres; and there are no dimensions, text, centre lines, hatching or title block on the layers that get cut. Keeping the profile and the holes on separate layers, and using simple entities in a widely read version such as R12, takes away most of the remaining guesswork.

Why do contours have to be closed?

CAM works contour by contour. To decide which side of a line is the part, where the kerf goes and where to pierce and lead in, it needs a loop with an inside and an outside. An open contour has neither. Depending on the software, it’s refused, cut as an open path that never frees the part, or compensated for kerf on the wrong side.

The gaps that cause this are often invisible: two ends that miss by a hair because a coordinate was rounded on the way through a PDF or another program. Many CAM packages join ends within a tolerance on import, but tolerances differ, so a file that relies on one works on one machine and not the next. A contour that crosses itself, like a figure of eight, is closed but has no clear inside, and causes the same trouble.

What’s wrong with duplicate, overlapping and zero-length entities?

On screen, none of them shows. In CAM, each can:

• Duplicates, an edge drawn twice, may be cut twice, which costs time and can burn the edge, or leave three ends meeting at one corner, so CAM can’t tell which way the contour runs.
• Overlaps, a line lying partly over another, do the same along part of an edge.
• Zero-length lines and tiny arcs are invisible at any zoom, but can break a contour into pieces or add a pierce where there’s nothing to cut.
• Stray points and specks far from the part don’t get cut, but they can stretch the drawing’s extents, so zooming to fit shows an empty screen with the part as a dot.

Most CAD programs have a command that deletes duplicate and overlapping entities, and a zoom to the drawing’s extents shows up strays at once.

Outer and inner contours: do layers matter?

CAM tells the outer profile from the holes by which contour encloses which: the outermost loop is cut with the kerf outside it, and loops inside it are holes, cut with the kerf inside and usually first, so the part doesn’t move before its holes are finished. That only works if every hole lies strictly inside the profile. A “hole” that touches or crosses the outer edge is really a notch, and belongs in the profile itself.

Layers aren’t essential for that, but they help. With the profile on one layer and the holes on another, you can check the part at a glance, and many CAM packages can map layers to processes on import. That matters more when the file carries anything that isn’t a through cut: lines for marking or etching, and bend lines, should each sit on a layer of their own that you map to the right process, or leave out, so nothing is cut that shouldn’t be.

Arcs, polylines or splines: which entities should a DXF use?

• LINE, ARC and CIRCLE are read by every CAM package, and an arc is cut as an arc: one smooth move rather than many short ones.
• Polylines are fine in most CAM, including their arc segments, which are stored as a “bulge” on each vertex. Check that a closed polyline really is closed, not just one whose last point happens to sit on its first.
• Splines and ellipses have to be approximated, either as arcs or as many short lines. Short lines leave faint flats on a curved edge and can make the head move jerkily, so convert curves to arcs before they reach CAM if you can.
• Chains of short lines standing in for a curve, typical of a PDF conversion or a traced image, cause the same trouble as a spline approximated badly, and are worth replacing with true arcs and circles.
• Blocks group entities into one object. Some CAM ignores them or reads them oddly, so explode them into plain entities first.
• Anything 3D. Every entity should be flat at Z = 0. Some CAD exports mirror an arc by flipping its extrusion direction rather than redrawing it, and a reader that ignores the flip draws the arc on the wrong side.

Which DXF version should you save?

If your CAM has a preferred version, use that. Otherwise R12 is the safe choice: it’s the most widely read, and saving to it drops splines, ellipses and lightweight polylines, which R12 can’t hold. It can still hold blocks, text and dimensions, so it doesn’t clean the file for you. Check the result, because some programs save curves to R12 as many short lines. The catch is that an R12 file can’t record its units, which is the usual reason a DXF comes in at the wrong size; see why a DXF imports at the wrong scale.

What size and units should it be?

True size, 1:1, in the units your CAM expects, which in most UK shops is millimetres. Draw to the nominal dimensions on the drawing, not offset for the kerf: CAM or the machine applies kerf compensation, and a part offset twice comes out the wrong size.

What shouldn’t be in the file?

Anything on a cutting layer is a candidate for cutting. Take out dimensions and their arrowheads, text and notes, centre lines, hatching, hidden lines, construction lines, the border and the title block. A DXF that came from converting a drawing usually has all of them, and how to remove dimensions, notes and title blocks from a DXF sets out the clean-up.

How do you check a DXF before it’s programmed?

1. Zoom to extents. If the part isn’t filling the screen, something stray is out there.
2. Look at the layers and entity types. Most CAD programs list what a selection holds: look for text, dimensions, blocks, splines or a layer you didn’t expect.
3. Delete duplicates with your CAD program’s command for it, and see whether it removed anything.
4. Check each contour is closed. Make a region from it, which fails on an open loop, or join it into one polyline and check that its properties say it’s closed.
5. Measure two dimensions at right angles against the drawing, and a hole diameter.
6. Import it into your CAM and look at what it found: the number of parts, which contours it treats as outside and inside, and any warnings.

These are checks on the file. The checks on the drawing that come first, from revision to material and small features against thickness, are in how to prepare customer drawings for laser cutting.

What does a Nest Ready DXF contain?

Nest Ready is our product, and it writes DXFs from drawings, so here is what its files contain. Each is R12 ASCII, with LINE, ARC and CIRCLE entities and nothing else:

• One closed outer profile on layer OUTER, coloured green.
• Holes and cut-outs on layer INNER, coloured red, each a closed contour inside the profile.
• True size in millimetres, built from the dimensions written on the drawing, with inch drawings converted, and the part moved to start at 0,0. Like every R12 file it doesn’t record its units, so import it as millimetres.
• No text, dimensions, centre lines, blocks or splines. One DXF per part; several parts download as a zip.

Before a part is written, the DXF it would ship as is checked against a written output contract, reading the file the way a strict CAM package would: every contour closes exactly, no curve is written as a run of short lines, no contour crosses itself or another, nothing is drawn twice, every hole lies inside the one outer profile, and nothing is too short or too small to cut. A part that breaks any of these is flagged for review. You can see the result in the flange example, whose bore and six bolt holes are circles on INNER. How this fits a laser cutting workflow is set out on the laser cutting page.

The limits: there are no layers for marking, etching or bend lines, and no text for engraving, so anything beyond the cut outline comes from the drawing. Review is advisory, so flagged parts you haven’t decided on still download. Kerf, lead-ins, tabs and nesting are set in your own CAM. Check every DXF against the drawing before cutting.