Designing parts for laser cutting

1. Understand the kerf

The laser removes a narrow strip of material as it cuts — the kerf. On our CNC fibre laser it's roughly 0.1–0.3 mm wide depending on material and thickness, and the cut sits centred on your drawn line. Two things follow from that:

• Holes come out slightly larger and pegs/posts slightly smaller than the nominal line, because half the kerf is taken from each side of the profile. For general fabrication this is well within tolerance; for a press-fit or bearing seat, call it out and we'll compensate.
• Two cut lines can't sit closer than about one kerf width or they merge into one. That's why very thin webs and slots have a practical minimum — covered below.

You don't need to offset your geometry for kerf yourself — draw the part at its nominal size and tell us any critical dimensions. We set the cut compensation in the machine.

2. Minimum feature size scales with thickness

The single most useful rule of thumb in laser design: the thicker the material, the larger the smallest feature it can hold. A fibre laser cuts a slightly tapered, slightly wider channel as plate gets thicker, so fine detail that's effortless in 1 mm becomes marginal in 10 mm.

Two guidelines cover most cases:

• Minimum hole diameter ≈ material thickness. A hole noticeably smaller than the plate is thick pierces poorly and can come out tapered or rough. In 5 mm steel, keep holes to about 5 mm and up; below that, expect a cleaner result from drilling.
• Minimum slot width / web thickness ≈ material thickness. A 6 mm-wide slot in 6 mm plate is fine; a 1 mm slot in 6 mm plate is not. The same goes for the thin wall left between two close features.

3. Give internal corners a radius

A laser beam is round, so it can't cut a perfectly sharp inside corner — there's always a small radius equal to about half the beam plus a touch. If you draw a dead-sharp internal corner, you'll get a tiny natural radius anyway. Better to design it in:

• Add a small fillet of at least 0.5× the material thickness to internal corners. It cuts cleaner, relieves stress, and looks intentional.
• If a sharp corner is functionally needed (for a tab to seat fully, say), add a small relief / dog-bone notch at the corner rather than expecting a knife-edge.
• External corners can be sharp — break them only if you want them safe to handle.

4. Space holes and edges sensibly

• Keep a hole at least 1× thickness from any edge, and ideally 2× for tapped or countersunk holes — too close and the thin remaining wall can pull or distort.
• Leave at least 1× thickness of material between adjacent holes.
• If the part will be folded, hold holes back from the bend line by at least 2.5× thickness plus the bend radius, or they'll deform. See the secondary operations guide.

5. Use bridges and tabs to hold small parts

When a part — or a feature inside it — is fully cut free, it drops into the machine or tips up into the cutting head. For most parts that's fine; the part is big enough to stay put. But two cases need bridges (a.k.a. micro-tabs or tags):

• Very small or very light parts — tiny washers, fine lettering, delicate filigree — that would otherwise fall through the bed slats and be lost, or move and re-cut. A few small bridges hold each part in the sheet until you snap them out by hand.
• Loose internal islands — the centre of a letter "O", a captured ring, the middle of a washer pattern — which need a bridge or they drop out and the laser cuts over the gap.

A bridge is a short un-cut segment, typically 0.3–1.0 mm wide, left in the profile; you twist or file the part free afterwards. We add and place them as part of the engineering review, so you don't have to draw them in — but do flag any part where a clean, untabbed edge is critical, and we'll position bridges where they won't show.

Keep reading