Laser cutting holes, slots and small features

One ratio decides whether a small feature is a laser job

Laser cutting holes, slots and small features is limited by the ratio of feature size to material thickness, not by the machine nameplate. A 3 mm hole in 1 mm CRCA is a normal cut. The same 3 mm hole in 8 mm mild steel is a pierce that takes a second or more, risks blowing out the top surface, and produces a bore that tapers towards the exit. The drawing looks identical; the route does not.

The practical rule for a fibre laser is a minimum hole of 0.5 × thickness in mild steel and 0.8 × thickness in stainless steel or aluminium. At 3 mm CRCA, that is a 1.5 mm hole; at 6 mm stainless, it is 4.8 mm. Anything smaller is still possible, but it moves from routine cutting into a process the planner has to think about, and the quotation should say so.

What follows matters more on production parts than on prototypes. A single 1 mm hole in a bracket is a curiosity. Four hundred 1 mm holes in a perforated panel is a machine-time line in the price, and it is also the point where dross, taper and pierce marks start to affect the part's function.

Material moves the ratio. Brass and copper conduct heat away from the cut, so a small hole in 2 mm brass needs more power and a slower pierce than the same hole in CRCA, and the reflective surface of aluminium makes a low-power pierce less stable. A design transferred from mild steel to stainless keeps its hole sizes and loses its cut speed, which is why the material belongs on the drawing next to the feature.

Minimum sizes, webs and margins

Three dimensions set the geometry. The hole itself, the material left between two features, and the distance from a feature to an edge. All three scale with thickness, which is why a design that works in 1 mm CRCA fails when it is moved to 2 mm without changing anything else.

Webs between holes need at least 1 × thickness. Closer than that, the second cut heats the ligament the first one left, and on thin sheet the web bows enough that neither hole passes a pin gauge. Edge margins follow the same rule: 1 × thickness from the cut edge, more where the edge is also a bend line.

Corners are the quiet failure. A sharp internal corner is a crack starter in a formed or loaded part, and the laser naturally leaves a small radius of about half the kerf. Draw a 0.5 mm radius rather than a sharp corner, and the part matches the drawing instead of relying on the cutter to add a radius nobody recorded.

Feature limits against thickness

What a small hole costs in machine time

Put 400 holes of 2 mm diameter in a 6 mm stainless panel. Each hole needs a pierce that is slower than the contour around it, because the beam has to establish a clean keyhole without spatter before it can travel. If the pierce adds 0.8 s per hole compared with a 5 mm hole pierced in the same plate, the panel carries 320 extra seconds — 5.3 minutes of machine time — before any cutting is counted.

At that scale, three drawing changes are worth more than any machine setting. Group holes of the same diameter so the machine can run one condition. Rotate the part in the nest so adjacent holes share a common cut line instead of two separate contours. And allow a larger pilot where the hole exists only for a fastener that has a washer under it, because a 2.5 mm clearance hole costs less than a 2.0 mm one and does the same job.

The same arithmetic explains why a perforated panel is often punched rather than cut. At high volume, a perforating tool makes every hole in one stroke, and the tool cost is recovered long before the laser time is. The laser cutting cost estimator is the quick way to see where the crossover sits for a specific pattern.

Piercing thick plate without spatter

A pierce on plate above about 6 mm is its own operation. The beam dwells, the metal erupts, and if the pierce point sits on the finished contour, the eruption leaves a notch on the edge. Two countermeasures are standard: pierce away from the contour and lead in with an arc, and use a ramped or pulsed pierce that steps the power up rather than hitting the plate at full output.

On stainless above 8 mm, nitrogen assist keeps the cut face bright but makes the pierce slower, because the gas does not help oxidise the metal out of the keyhole. On mild steel, oxygen speeds the pierce and leaves an oxidised edge. Neither choice is wrong; they produce different edges and different machine times, and the drawing should say which one the part needs.

Slots, webs and tabs that survive handling

A slot is a hole with a length problem. Cut a 2 mm wide, 40 mm long slot in 2 mm CRCA and the middle of the slot bows, because the ligament on each side heats unevenly and the part relieves itself as it cools. Keep the length-to-width at 10:1 or less, and where a longer slot is functionally necessary, cut it in two passes with a pause between them rather than one continuous run.

Tabs and micro-joints are how parts stay in the nest until they are knocked out. A tab of 0.8 mm holds a small bracket and snaps cleanly. A tab that is too wide leaves a burr at the break line, and too narrow a tab lets the part lift and catch the head. Either way, the tab marks belong on the drawing if the part is visible, because they are the one place a laser-cut edge is not straight.

Thin webs between slots are the hardest geometry to hold. Below about 1.5 × thickness, the web can twist during cutting, and the finished part looks fine on the bench and out of flat on the fixture. If the drawing needs a decorative grille with 1 mm webs, that is a different process conversation — usually an etch, a punch or a redesign that accepts wider bars.

A slot within 3 mm of a bend line behaves like a hole within the same distance: the outer wall stretches and the slot closes at the bend end. Put the slot past the bend, or orient it parallel to the bend line so the stretching acts along its length rather than across its width.

Tolerances after deburring and coating

The cut is the most accurate step in the route. Deburring, forming and coating each add variation, so the tolerance a buyer should specify belongs on the finished feature, not on the blank. A laser-cut 6.0 mm hole is typically within ±0.1 mm off the machine; after a vibratory deburr and 70 µm of powder, the same hole measures about 5.9 mm on a pin gauge, which is still inside a ±0.5 mm general tolerance but outside a ±0.1 mm one.

That difference matters when the hole locates a bought-in component. If a 6 mm dowel has to pass, specify an 8 mm hole and accept the clearance, or mask the bore during coating. If the hole is a datum for the assembly, mask it or plan a ream after coating — never assume the as-cut size survives the paint line.

Hole position drifts for a different reason. Two holes cut 200 mm apart are within 0.1 mm of nominal on the blank, but if they sit either side of a bend, the bend allowance error moves them relative to each other. That is why the drawing should dimension hole positions from a datum on the same face wherever the design allows it.

What we run on small features

Holes, slots and fine geometry run on the 12 kW fibre laser, whose bed measures 40 ft × 16 ft, with two 6 kW and two 3 kW machines taking the thinner work where a smaller spot and lower heat input suit the feature. Mild steel, CRCA, stainless, aluminium, brass and copper all run on the same lines, and the cutting parameters change with the material rather than with the operator's preference.

Downstream, small features are deburred before they are coated, because a burr inside a 4 mm hole is harder to remove after powder than before it. Deburring and edge control are handled on the laser cutting route alongside the cut, with first article inspection and PPAP available where the programme needs a documented record. Work for Mahindra, Godrej & Boyce and Minda runs through the same inspection sequence.

The rest of the route sits in the laser cutting and fabrication hub. Two pieces next to it: laser cutting tolerances for OEM parts covers how feature tolerances stack on a finished component, and deburring and edge quality after laser cutting covers what happens to the edge after the nest is broken.

What the cut drawing has to settle

• Every hole with a function, its size and its tolerance — clearance holes and fit holes are not the same call-out.
• The thread call-out with the tap drill size, not the nominal bolt size, if the hole will be tapped after cutting.
• Slot width, slot length and the direction the slot must run, especially where it is a locating feature.
• Web widths on any grille or perforated pattern, plus the distortion you can accept on the panel.
• Tab and break-line positions for parts that will be handled in the nest.
• The tolerance class for everything else, stated as ISO 2768-1 medium rather than left blank.
• The hole-to-bend dimension on every formed part, checked against the rule in the hole-to-bend guide.

When the hole should be drilled, not cut

Holes under 0.5 mm are drilled or EDM-cut, not laser-cut. Threads, counterbores, spotfaces and reamed fits are machined, because the laser gives a through hole and no shoulder. A hole that must hold an H7 fit needs a drilled and reamed bore; a laser-cut hole is a clearance feature even when it is accurate.

Deep holes are the other case. A hole whose depth exceeds about five times its diameter is a drilling job, whatever the diameter, because the laser loses the cut front and the exit hole wanders. Small features in thick plate generally cost more on the laser than they cost to drill, and on a part that already needs machining, adding a drilling step is often the cheaper route.

The last case is appearance. A laser-cut hole in a visible face carries a small pierce mark on the entry side and a dross ring on the exit. Deburring removes most of it, but on a polished stainless panel or a visible anodised aluminium fascia, a drilled and countersunk hole may be the only finish that passes inspection.