Most of the questions engineers ask about kerf compensation assume the problem is in the DXF. It almost never is.
SolidWorks exports flat patterns with nominal dimensions — exactly as modeled, no offset applied. That’s correct behavior. The question is whether you understand where kerf compensation actually happens, and what breaks when it happens in the wrong place.
What Kerf Is and Why It Varies
Kerf is the width of material removed by the laser beam — the slot left behind after a cut. On a fiber laser cutting 3mm mild steel, typical kerf width runs 0.08–0.15mm. For thicker material (12mm+) or plasma, it can exceed 1mm.
The critical point engineers miss: kerf is not a constant. It varies continuously based on:
- Material type and grade (mild steel, stainless, aluminum, brass all cut differently)
- Sheet thickness
- Laser power and cutting speed
- Assist gas type and pressure (nitrogen vs oxygen produce different kerfs)
- Cutting geometry — tight inside corners and small radii slow the head and widen the cut
- Lens condition and beam focus
An engineer who hard-codes a 0.15mm kerf offset into their DXF based on one test cut on 2mm mild steel will ship incorrect parts when the shop uses a different power setting, cuts the same job on 3mm, or switches to nitrogen assist.
Where Kerf Compensation Actually Belongs
Industrial laser cutting systems apply kerf compensation in one of two places:
Controller-level offset (G41/G42). CNC controllers support left/right cutter radius compensation via G41 and G42 codes. In milling this is standard practice. For laser cutting, most shops avoid it — the offset is specified in machine units and doesn’t adapt to material or speed changes. Rarely seen in modern laser workflows.
CAM software. This is where compensation actually happens in practice. Bystronic’s BySoft, Trumpf’s TruTops, Prima Power’s Maestro, and JETCAM all apply kerf compensation as part of the nesting and toolpath generation step. The CAM system knows the current material, thickness, and cutting parameters, so it can apply a geometrically correct offset — inward on external profiles, outward on holes and slots — calibrated to what that machine produces on that material today.
CAM-side compensation has one decisive advantage: it’s calibrated against the actual cutting process. The shop runs test pieces, measures them, and dials in the offset. When the material batch changes or the laser gets serviced, the offset gets recalibrated. Your DXF plays no role in any of this.
The Double-Compensation Trap
The worst kerf-related failure mode is double-compensation. It works like this:
- Designer calculates that the shop uses a 0.15mm kerf, so they offset all external contours outward 0.075mm and all holes inward 0.075mm in the DXF.
- Shop receives the DXF, doesn’t notice the geometry has been pre-offset, and runs it through CAM as usual.
- CAM applies its standard 0.075mm offset on top of the existing geometry.
- Every external dimension ends up 0.15mm oversized. Every hole ends up 0.15mm undersized.
- Tabs don’t fit slots. Assembly holes miss their patterns. Everything needs to be remade.
This is not a theoretical concern. It’s a routine failure mode in shops that do both in-house cutting (where the designer controls the full chain) and outsourcing (where they don’t). A DXF that was correct for one job gets sent to a second shop that compensates differently, and the parts fail.
The rule is simple: never pre-offset DXF geometry for kerf unless you control both the design and the machine. Even then, document it explicitly on the drawing.
How SolidWorks Exports Flat Patterns
SolidWorks ExportFlatPatternView — the API method behind every flat pattern DXF export — outputs geometry at nominal dimensions. There are no kerf-related parameters in the method signature. The export options control which entities are included (bend lines, construction geometry, hidden edges, sketch entities) and the coordinate system, but not dimensional offsets.
If you inspect the output DXF from SolidWorks on a part modeled as 100mm × 50mm, the outline in the DXF measures exactly 100mm × 50mm. A 5mm hole is exactly 5mm. There is no offset.
This is correct. It matches what every fabrication shop expects to receive: nominal geometry that their CAM system will adjust.
The only legitimate use of pre-offset DXF geometry is when you’re driving a machine directly from DXF without a CAM layer — for example, some hobbyist laser controllers (LightBurn, RDWorks) that accept DXF with no toolpath processing. In those cases, the kerf offset belongs in the controller’s settings, not in the DXF, because the controller still provides a kerf offset field. Pre-offsetting the DXF and then applying a controller offset produces the same double-compensation problem at smaller scale.
K-Factor Is Not Kerf
There’s a related confusion worth addressing: K-factor affects bend allowance (how much flat material gets consumed during a bend), not the outline of the flat pattern. Getting K-factor wrong shifts the position of the bend lines and changes the blank size. Kerf is an entirely separate concern, applied after the flat pattern is unfolded.
If your flat pattern outline dimensions don’t match the folded part, that’s a K-factor problem. If your parts come back from the shop slightly oversized or with holes that are too small to accept a fastener, that might be a kerf problem — but more often it’s a tolerance coordination problem with the shop.
The K-factor setup in SolidWorks has its own set of traps around material database defaults vs per-feature overrides. Worth understanding separately from kerf.
What the Shop Actually Needs From You
The most useful thing you can do regarding kerf is communicate clearly:
Tell the shop the DXF contains nominal geometry. Most shops assume this, but confirming it avoids any guessing about whether you’ve pre-offset. If you’re using a template or repeating a job, explicitly note whether the geometry matches previous runs.
Specify critical tolerances on the drawing, not in the DXF. If a slot needs to be 10.0 ± 0.05mm for a press-fit, call that out on the print. Let the shop determine what offset achieves it on their machine with their material. They cut more parts than you do. They know their process.
Run test pieces before production on tight-tolerance parts. A kerf offset that worked on last year’s 2mm mild steel job may not work on the same shop’s new fiber laser at a different power density. An empirical test cut costs almost nothing compared to a production run of incorrectly sized parts.
For a deeper look at what metadata and entity settings fabricators actually care about in a DXF, what fabricators need in DXF files covers the layer mapping, bend line requirements, and file naming that actually affect shop floor success.
CadShift and Kerf
CadShift exports flat patterns via the SolidWorks API — the same ExportFlatPatternView mechanism SolidWorks itself uses. The output is nominal geometry. No kerf offsets are applied.
This is deliberate and correct. The flat pattern you export through CadShift is the same geometry that defines your modeled part. Kerf compensation belongs in the CAM software at the shop, calibrated to the specific machine, material, and cutting parameters for that job.
If you’re cutting in-house with a controller that doesn’t have a CAM layer, apply the kerf offset once in the controller settings — not in your SolidWorks model or your DXF.
The DXF entity export settings that matter for laser cutting shops — end-point merging tolerance, bend line layer, construction geometry — are separate from kerf and worth reviewing if you’re seeing profile fragmentation or bend lines on the wrong layer.
The Practical Checklist
When handing off DXF flat patterns for laser cutting:
- Export nominal geometry from SolidWorks — no manual offsetting.
- Tell the shop the DXF is nominal. Ask how they apply kerf compensation.
- If there are tight tolerance fits (slots, tabs, press-fits), call them out on the drawing with explicit ± values.
- For a new material or shop, run a test piece first. Measure the actual kerf on a sample cut before committing to production.
- Never send a pre-offset DXF to a shop that also runs CAM compensation without explicitly flagging it.
- If something doesn’t fit, ask whether kerf was applied once or twice before assuming the model is wrong.
The part that’s 0.15mm oversize has almost certainly been compensated twice, not once.