Laser-cut hole limits: aspect ratio and minimum diameter

A laser will cut a Ø0.5 mm hole in 1 mm stainless and it will look correct on the screen. Whether it is round, whether it is the size the drawing asked for, and whether the underside is clean are separate questions, and thickness answers all three. The limit is not the beam. It is the kerf, the taper and the assist gas.

Laser-cut hole limits reduce to one ratio: material thickness divided by hole diameter. At 1:1 the cut is stable, the kerf is 0.2–0.3 mm wide in thin sheet, and the hole can hold ±0.10 mm on diameter. At 2:1 the contour needs a slower pass and a controlled pierce. At 3:1 the exit tapers, dross adheres, and a drill becomes the cheaper route. A hole the laser can make is not always a hole worth making.

This is written for design engineers and buyers checking a DXF before release, and it applies to flat-bed fibre laser cutting of CRCA, mild steel, stainless and aluminium. It gives the minimum diameter and aspect ratio by thickness, works through the taper arithmetic, and sets out the callout that separates a hole the laser owns from one that belongs on a drill.

What actually limits a laser-cut hole

The hole limit is set by how much energy reaches the bottom of the kerf, not by how small the beam can focus. A 12 kW fibre laser focuses to a spot around 0.1 mm, so geometry alone would allow a hole far smaller than the process can deliver. Three things stop it:

• Kerf width. The cut removes 0.2–0.3 mm of material in 1–3 mm mild steel, and 0.3–0.6 mm at 10–20 mm. A hole has to be several kerf widths across or the cut path is mostly kerf, and the hole is oversized and out of round.
• Taper. Energy density and gas pressure fall as the kerf deepens, so the exit diameter is smaller than the entry. The deeper the hole relative to its diameter, the larger the difference.
• Gas flow. Assist gas has to reach the molten front and blow it out of the hole. In a deep, narrow hole the gas stalls, dross freezes on the underside, and the hole needs a second operation to clean.

The first limit is arithmetic, the second is optical, and the third is the one that decides whether the part leaves the machine without a deburring step. All three get worse as the hole gets smaller relative to the plate.

The rule: diameter, aspect ratio and spacing

The minimum hole diameter is 1.0 times the material thickness for a round hole with a clean underside, and 0.5 times the thickness where a slower pass and some taper are acceptable. Written as an aspect ratio with depth divided by diameter, that is 1:1 by default and 2:1 at the limit. The ratio is the useful number because it travels with the part: a rule in millimetres stops working the moment the gauge changes.

Two spacing rules travel with it:

• Hole to hole. At least 1.0 mm of ligament between adjacent holes, and 2.0 mm where both are functional. Two kerfs plus their heat-affected zones leave less sound material than the drawing suggests, and a narrow bridge warps as the second hole is cut.
• Hole to edge. At least 1.0 mm of ligament, set by handling and finishing rather than by the cut. A 0.4 mm strip survives the laser and rolls over in the deburring bowl.

The rules interact in ways that surprise people. A Ø2 mm hole 1.0 mm from an edge in 3 mm sheet is a 1.5:1 hole, acceptable on its own, but the ligament is only a third of a hole diameter wide. The hole may cut cleanly and still fail inspection because the edge rolled during handling.

Minimum hole diameter by thickness

Values below are for mild steel and CRCA on a flat-bed fibre laser, with nitrogen or oxygen assist selected per thickness. Stainless shifts the small end by one step because the cut runs hotter and dross adheres more readily; aluminium shifts it by two because the reflectivity and thermal conductivity both work against a small, deep hole.

The last three rows are the ones a designer usually meets on a heavy bracket rather than a cover. A Ø20 mm hole in 12 mm plate is 0.6:1 and behaves like a normal contour. A Ø7 mm hole in the same plate is 1.7:1, cuts with visible taper, and needs a slower contour and a clean pierce. A Ø4 mm hole is 3:1 and should be drilled, even though the laser can technically trace the path.

A worked example: Ø3 mm through 6 mm plate

A Ø3 mm hole in 6 mm mild steel is a 2:1 hole, so it is inside the practical limit and outside the default. Two numbers decide whether it is a design feature or a drilling allowance.

The first is taper. Kerf walls lean inward by about 1.5° per side on this thickness, so the entry-to-exit difference is:

Δd = 2 × t × tan(α) = 2 × 6 × tan 1.5° = 12 × 0.0262 = 0.31 mm

A Ø3.00 mm entry measures about Ø2.69 mm at the exit. That is a 10% change across the thickness and larger than the ±0.10 mm diameter tolerance a fastener hole usually carries. If the hole is meant to clear an M3 screw, the exit is below the 3.00 mm major diameter, so the screw will not pass without reaming. Draw the hole at Ø3.2 mm or move it to a drill.

The second is time. The contour length is π × 3 = 9.42 mm. At a contour speed of 25 mm/s that is 0.38 s of cutting, plus a pierce of roughly 0.3 s, so about 0.7 s per hole. A batch of 1,000 holes is 700 s, or under 12 minutes of beam-on time, before moves between holes. Cutting the hole is not the cost. Checking it, or drilling it afterwards, is.

The same taper applies to a Ø10 mm hole in the same plate, where 0.31 mm is 3% and comfortably inside a ±0.20 mm tolerance. Taper is set by thickness, so it does not shrink when the hole does. That is the whole argument for a minimum-diameter rule expressed as a ratio.

Taper is absolute, tolerance is relative

The taper number is a property of the thickness and the wall angle, so it stays roughly constant as the hole diameter changes. A 0.31 mm difference is 10% of a Ø3 mm hole, 3% of a Ø10 mm hole and 1.5% of a Ø20 mm hole. The smallest holes therefore carry the largest relative error, which is why the minimum-diameter rule is really a tolerance rule wearing a size label.

ISO 9013:2017 classifies thermal cuts by geometrical quality, covering both the cut surface and the perpendicularity of the cut face, with class 1 the tightest and class 5 the loosest. It describes what the cut face looks like; it does not promise a hole diameter. A drawing that calls a quality class without a diameter tolerance and a measurement face has told the supplier how the wall should look, not what the hole must measure.

The measurement face matters more than most drawings admit. A hole measured at the entry passes; the same hole measured at the exit fails; the same part measured with a plug gauge, which reads the smallest section, fails as well. State the face, state the gauge, and state whether the hole is judged by the entry, the exit or the minimum section. The laser cutting tolerance guide sets out the position and profile values that sit around this.

Slots, corners and square holes

A slot is easier to cut than a round hole of the same width. The kerf is continuous, the assist gas escapes along the path instead of stalling at the bottom, and there is no pierce in the middle of the feature. A 1.0 mm wide slot in 3 mm sheet cuts cleanly, while a Ø1.0 mm hole at 3:1 does not. That asymmetry is useful: replace a row of small holes with a slot when the function allows it.

Internal corners are a different constraint. The beam is round, so a true square internal corner cannot be cut. The minimum inside radius is about half the kerf, 0.10–0.15 mm, and a corner that tight concentrates stress and traps coating. Draw 0.5 mm minimum on a 3 mm part and 1.0 mm on anything structural. Where a square corner is needed for a mating part, add a relief hole at the corner and accept the extra feature.

The holes, slots and small features guide covers the geometry in more detail. The rule to carry into this article is that a slot can be narrower than the smallest hole you would allow, because the gas path is open.

See the process and inspection scope on the capability pages, or send the drawing through the RFQ route.

What Ganesh actually runs

Cutting runs on a 12 kW fibre laser with a 40 ft × 16 ft bed, supported by two 6 kW and two 3 kW machines, in mild steel, CRCA, stainless, aluminium, brass and copper, up to 20 mm on the laser and 30–40 mm on the iron worker for plate. The large bed matters for hole patterns: a 3,000 mm panel with fifty small holes is cut in one setup rather than in sections that have to be aligned afterwards.

Not every hole goes to the laser. Where a hole is 1.5:1 or tighter, or carries a thread, the route moves to a press from 20 T to 300 T with 250 T punching capacity, and the in-house tool room makes the pierce tool. That decision is made at quotation, not after the first part, and it is recorded against the drawing so the next order follows the same route.

Typical sheet metal tolerance is ±0.5 mm, tighter on critical features by agreement, and PPAP plus first article inspection are available. The laser cutting capability page lists the machines and the materials, and the thickness and edge quality guide covers what the cut face looks like at each end of the range.

What to put on the drawing

• Every hole diameter with its tolerance, and the face the tolerance applies to: entry, exit or minimum section.
• A note fixing the rule in one line, for example "holes below 1.0t to be drilled", so the route does not depend on who reads the DXF.
• Position tolerance to named datums, not to the nearest edge.
• Thread callouts as a pilot diameter plus "drill and tap after cutting", with the pilot 0.3–0.5 mm under the tap drill size.
• Minimum internal corner radius, 0.5 mm on thin sheet and 1.0 mm on structural parts.
• Minimum ligament between holes and to the edge, 1.0 mm unloaded and 2.0 mm loaded.
• An ISO 9013 perpendicularity class only where the hole is a bearing surface, and a diameter tolerance alongside it.
• The deburr or edge condition, because a dross-free cut and a rounded edge are different requirements.

When the laser is the wrong route

Below a 1.5:1 aspect ratio the honest answer is a drill. That covers a Ø6 mm hole in 10 mm plate, a Ø4 mm hole in 8 mm plate and almost any hole under Ø3 mm in 12 mm plate. Drilling costs a second setup and leaves a burr, but it produces a straight, round hole at the size the drawing asked for.

Tapped and reamed holes belong on a drill for the same reason: a taper of 0.31 mm cannot hold a thread flank or a reamed fit. So do true square internal corners and holes with a positional tolerance tighter than ±0.05 mm relative to a datum that is not cut in the same nest.

We do not run tube laser cutting, five-axis laser trimming or in-die tapping, so a formed part that needs a hole only reachable after forming, or a tapped hole produced inside the press tool, is outside the route here. Those parts need a post-form operation or a different design.

The cheapest time to settle this is before the DXF is released. Send the file with the smallest holes marked, the material and the thickness to request a quote, and the hole schedule comes back with the ones that cut cleanly, the ones that need a slower pass and the ones that should be drilled. The DXF preparation checklist covers the layer and contour conventions that make that review quick, and the laser cutting and fabrication hub has the rest of the process rules.