Tolerance is the cheapest thing to get wrong on a sheet metal drawing. Ask for tighter than the process can hold and you pay for inspection and rework; leave it off entirely and you get the shop’s default, which may not fit your assembly. This page lays out the standard tolerances a fiber-laser shop holds, the tight limits we can reach when you call them out, and how forming stacks error across bends — so you can tolerance a part correctly the first time.
This is the companion to our laser cutting tolerance & kerf chart, which covers cut tolerance by material and thickness in detail.
Standard vs. tight: the quick reference
| Feature | Standard (default) | Tight (call it out) |
|---|---|---|
| Cut / linear dimension | ±0.15mm | ±0.1mm (≤±0.05mm on thin sheet) |
| Bend angle | ±1° | ±0.5° |
| Dimension across one bend | ±0.2mm | ±0.1mm |
| Each additional bend (stacks) | +±0.1mm | — |
| Hole diameter (laser cut) | ±0.1mm | ±0.05mm |
| Hole position | ±0.15mm | ±0.1mm |
| Hole / feature to edge | ±0.15mm | — |
The golden rule: only tighten what actually has to fit. A blanket ±0.05mm on every dimension multiplies cost without improving the part.
Cutting (linear) tolerance by thickness
Cut tolerance widens with thickness because of edge taper and heat. These are summary bands — see the full material-by-thickness chart for per-material values.
| Thickness | Standard cut tolerance |
|---|---|
| ≤ 3mm | ±0.1mm |
| > 3 – 6mm | ±0.15mm |
| > 6 – 12mm | ±0.2mm |
| > 12 – 20mm | ±0.3mm |
| > 20mm | ±0.5mm |
Bend tolerances (and why they stack)
Bending is less precise than cutting. Two things vary: the bend angle and the resulting dimension between a bent face and a reference. Every bend adds its own error, so a 6-bend part is harder to hold than a 1-bend part — tolerance accumulates.
| Number of bends | Typical dimensional tolerance |
|---|---|
| 1 bend | ±0.2mm |
| 2 – 3 bends | ±0.3mm |
| 4 – 5 bends | ±0.4mm |
| 6+ bends | ±0.5mm — or call out the critical dimension |
- Bend angle: ±1° standard, ±0.5° achievable on short, well-supported bends.
- Datum from one edge. Dimension all bend features from a single reference edge, not chained end-to-end — chaining adds every bend’s error together.
- Minimum inside bend radius ≥ material thickness. Tighter radii crack the outside fiber, especially on hard stainless and aluminum.
Need the flat-pattern size before you bend? Set your material, thickness, radius and angle below and read off the bend allowance and blank length:
BA = (π/180)·angle·(R + K·t) · BD = 2·(R+t)·tan(angle/2) − BA · Flat = A + B − BD (two outside flanges, single bend). K-factor presets are typical defaults — confirm on quote.
Hole & feature tolerances
Laser-cut holes are round and accurate, but they are not reamed bores:
- Hole diameter: ±0.1mm typical, ±0.05mm achievable on thin sheet. For a true bearing or dowel fit, call out the bore for a secondary reaming/machining pass.
- Hole position: ±0.15mm standard. Positions hold tighter than diameters because they come straight from the machine’s positioning system.
- Minimum hole diameter ≥ material thickness (min 1mm). Below that the edge rounds over.
General tolerances (ISO 2768) for undimensioned features
For any dimension you don’t explicitly tolerance, most shops fall back to ISO 2768-m (medium). State which class applies in your title block so there are no surprises:
| Nominal length | ISO 2768-m (medium) |
|---|---|
| 0.5 – 3mm | ±0.1mm |
| > 3 – 6mm | ±0.1mm |
| > 6 – 30mm | ±0.2mm |
| > 30 – 120mm | ±0.3mm |
| > 120 – 400mm | ±0.5mm |
| > 400 – 1000mm | ±0.8mm |
How to tolerance a drawing the right way
- Set a default in the title block — e.g. “General tol. per ISO 2768-m; laser-cut edges ±0.15mm.”
- Call out only critical features individually — mating holes, locating edges, press-fit bores.
- Datum from one edge for all bend dimensions.
- Flag anything below ±0.05mm or any true bore fit — we’ll plan a finishing pass into the quote rather than fail the first article.
FAQ
What is the standard tolerance for laser-cut sheet metal? ±0.15mm on cut dimensions as a default; ±0.1mm or tighter on called-out features. Bends add ±0.2mm per bend and ±1° on angle.
Why can’t you hold ±0.05mm everywhere? Forming and thermal effects make sub-0.05mm impractical across a whole part. We hold it on specific thin-sheet features, or add a machining pass — just tell us which dimensions matter.
Do tolerances get looser on thick plate? Yes. Expect ±0.3mm above 12mm and ±0.5mm above 20mm, plus wider kerf.
Get a part reviewed for free
Send your DXF and we’ll tell you exactly which tolerances we can hold and which need a finishing pass — before you commit. Request a quote or see transparent pricing.
