On our 3 kW CNC fibre laser at Layer X, we hold ±0.1 mm on profile dimensions across mild steel to 16 mm, stainless steel 304/316 to 12 mm, and aluminium 5052/6061 to 10 mm — with a kerf of roughly 0.1–0.25 mm depending on gauge. That headline figure is the number most drawings need, but it is not the whole story: as material gets thicker the edge picks up taper, small holes stop cutting cleanly, and positional accuracy across a full 1500×3000 mm sheet behaves differently from a single feature. This guide breaks tolerance down by material and thickness so you can dimension, GD&T and specify a part that actually cuts to print the first time.
What “±0.1 mm” actually covers
When we quote ±0.1 mm on our laser cutting service, that is the profile tolerance on cut geometry — the position of an edge or hole relative to the part datum, on thin to mid gauge material, under stable thermal conditions. It is a repeatable, process-qualified figure, not a best-case one-off. What it does not silently include:
- Edge squareness (taper). A laser kerf is very slightly wider at the top than the bottom. On 1–3 mm it is negligible; on 12–16 mm it becomes a real perpendicularity deviation you should account for on mating faces.
- Kerf compensation. The beam removes 0.1–0.25 mm of material. We offset the toolpath so your nominal dimension is met, but a slot drawn at exactly beam width will not cut — design to nominal, not to kerf.
- Thermal growth on large profiles. Heat input distorts long thin ribs and tight nests. A 2500 mm-long part will not hold the same absolute accuracy end-to-end as a 100 mm bracket.
The international reference for these edge attributes is ISO 9013, the standard that classifies thermally cut edges by perpendicularity tolerance and mean surface roughness. When a part is genuinely critical, we recommend calling out an ISO 9013 quality range on the drawing rather than the word “laser cut” alone.
The tolerance chart by material and thickness
This is the table to spec from. Every thickness and edge description below reflects what our fibre laser actually runs; the profile tolerance is our qualified ±0.1 mm, with the practical notes telling you where to add margin as gauge climbs.
| Material & grade | Max thickness | Assist gas | Kerf width | Profile tolerance | Edge quality & taper note |
|---|---|---|---|---|---|
| Mild (carbon) steel | 16 mm | Oxygen | 0.1–0.25 mm | ±0.1 mm | Clean square edge to mid gauge; oxide layer and mild taper appear on the heaviest plate — add margin on mating faces above ~10 mm. |
| Stainless steel 304 / 316 | 12 mm | Nitrogen | 0.1–0.25 mm | ±0.1 mm | Bright, oxide-free, weld- and paint-ready edge. Taper stays low on thin gauge; expect measurable perpendicularity deviation approaching 12 mm. |
| Aluminium 5052 / 6061 | 10 mm | Nitrogen | 0.1–0.25 mm | ±0.1 mm | Clean bright edge, minimal dross. High reflectivity makes thick aluminium the most demanding cut; hold tightest tolerances on lighter gauge. |
| Acrylic (PMMA) | 20 mm | — | 0.1–0.25 mm | ±0.1 mm | Flame-polished, glossy edge straight off the bed — no secondary finishing on display and signage work. |
Two patterns run through the whole chart. First, tolerance and edge quality are best on thin and mid gauge and degrade toward each material’s maximum — 16 mm mild steel and 10 mm aluminium are the two edges of the envelope where you should design in the most margin. Second, assist gas dictates edge finish: oxygen gives an economical square cut on thick mild steel but leaves an oxide skin; nitrogen gives the bright, weld-ready edge on stainless and aluminium at a higher running cost. Choosing the grade and gauge fixes the achievable edge before we ever nest the sheet.
Edge taper: why thickness changes everything
Taper — the difference in a cut’s width from top face to bottom face — is the tolerance most engineers forget until a thick-plate part refuses to sit flush. The physics is simple: the focused beam and the assist-gas jet do their cleanest work near the focal plane, so the kerf opens slightly toward the top surface and the bottom edge can lag. On 1–3 mm sheet the effect is inside our ±0.1 mm profile band and you can ignore it. From roughly 8 mm upward it becomes a genuine perpendicularity term.
Practical rule from our shop floor: if a thick-plate part has a face that mates, seals or locates against another surface, treat perpendicularity as a separate GD&T callout rather than assuming the profile tolerance covers it. On stainless approaching 12 mm and mild steel approaching 16 mm we will flag this at DFM and, where the face is critical, recommend a light secondary machining pass. Our overall studio precision runs to ±50 µm across processes, so squaring a critical edge downstream is well within capability when the drawing demands it.
Minimum hole and slot sizes by thickness
A fibre laser cannot pierce and cleanly cut a hole much smaller than the material is thick. Try it and you get a tapered, re-melted, dross-filled bore instead of a round hole. The industry design convention we work to — and the one we check every incoming DXF against — is straightforward:
| Feature | Safe minimum (general DFM rule) | Why it matters |
|---|---|---|
| Round hole diameter | ≥ material thickness | Below 1× thickness the pierce cannot form a clean, round, low-taper bore. |
| Slot / cut-out width | ≥ material thickness | Narrow slots trap heat and dross; the kerf bridges and the edge degrades. |
| Web / land between features | ≥ material thickness | Thin material left between two cuts warps or burns through under heat load. |
| Internal corner radius | ≥ ~0.5× kerf | The beam is round — a truly sharp internal corner is not physically cuttable. |
These are minimums, not targets. A 3 mm hole in 3 mm steel will cut, but a 5 mm hole in the same sheet holds tolerance and roundness far more comfortably. When a design genuinely needs a hole smaller than the plate is thick — a common ask on tapped or dowel-located brackets — the right answer is usually to laser the profile and drill or ream the critical bores afterwards. We flag undersized holes and open contours at the file-prep stage before anything reaches the bed, exactly as described in our kerf, edge quality and dross engineer’s guide.
Positional accuracy across the full sheet
Single-feature accuracy and whole-sheet accuracy are different questions. Our bed is 1500×3000 mm, and the machine positions the head to hold ±0.1 mm on individual profiles. Across a densely nested full sheet, however, cumulative thermal input and material movement mean the absolute distance between a feature in one corner and a feature in the far corner carries more variation than the same two features cut on a small blank.
For most fabrications this never matters — parts are separated and each part holds print. It matters when a single large part spans much of the sheet and needs tight hole-to-hole distances end to end. In that case we dimension from a single datum rather than chaining tolerances, order the cut sequence to balance heat, and where necessary cut the part on its own blank. If your part is large and precision-critical, say so in the enquiry: it changes how we nest and sequence, not just how we quote.
Holding tolerance into bending and assembly
A flat blank cut to ±0.1 mm is only half the tolerance story if the part gets bent. Every bend adds its own variation, and bend-angle error compounds with cut-edge position to move hole locations on the finished part. Because our CNC press brake sits in the same building, a laser-cut profile can go straight to bending as one single-source sheet-metal order — we hold ±0.3° on bend angle across a 160-tonne press and 3200 mm maximum length, and we account for the interaction between cut and bend tolerance at the DFM stage rather than discovering it at assembly.
The general-tolerance framework worth referencing on any sheet-metal drawing is ISO 2768, which defines default linear and angular tolerance classes. Calling out a class (for example, ISO 2768-m for medium) tells us which non-critical dimensions can float and lets us reserve tight tolerances for the features that truly need them — which keeps your part cuttable and your quote sensible. If you are also selecting grade and gauge, our note on choosing mild steel, stainless or aluminium pairs directly with the thickness limits in the chart above.
How to specify a part that cuts to print
Bringing it together, here is the checklist we wish every incoming drawing followed:
- State grade and thickness explicitly — “SS304, 3 mm” not “stainless, ~3 mm”. Achievable tolerance and edge depend on both.
- Keep holes, slots and webs ≥ material thickness, and call out separately any bore that must be tighter or smaller so we can reserve it for drilling/reaming.
- Add a perpendicularity callout on mating faces above ~8 mm, where taper leaves the profile band.
- Apply a general-tolerance class (ISO 2768) so non-critical dimensions are not over-specified.
- Dimension large parts from a single datum rather than chaining tolerances across the sheet.
- Send clean DXF geometry — it imports as exact vectors with no interpretation, unlike a scaled PDF.
Do that, and the ±0.1 mm on the chart is the tolerance you get, not the tolerance you hoped for. It is one reason our shop runs a 99.4% first-pass yield: most tolerance failures are designed in long before the laser fires, and a five-minute DFM check catches them.
Ready to cut? Upload your CAD file for a 24-hour quote — send DXF, DWG or STEP with grade, thickness and quantity, and we will confirm achievable tolerances, flag any features that need attention, and price the job before you commit.