A tolerance block may be the most expensive sentence on your drawing. Send the same 2 mm aluminium enclosure to five competent fabricators and the quotes will spread by far more than the material cost ever justifies — and almost every time, the spread traces back to how sheet metal fabrication tolerances are written, or not written, in the title block. This guide prints the actual numbers from the standards, the numbers each process really holds, and a tolerance block you can paste onto your own drawing before you send it out.
Consider what actually happened to one of our own customers. A German audio OEM sent us a folded aluminium chassis — 2 mm 5052-H32, six bends, a perforated front face, and a tolerance note that simply read "TOLERANCES ±0.1 UNLESS NOTED". Of the 84 dimensions on that drawing, four controlled whether the chassis would mate with the machined front panel; eighty did not. Three of the four crossed two bends each, so ±0.1 was not purchasable at any price. The drawing had to be re-released twice, and six weeks disappeared. The fix took four sentences in the title block.
There are three ways sheet metal fabrication tolerances go wrong on a drawing, and they cost different things:
- Over-toleranced. Every dimension carries ±0.05, so every bidder prices the cheap ones as if they were expensive. You get a risk premium on parts you never needed tight — or no quote at all.
- Under-toleranced. No individual callouts on functional features, everything deferred to a general class that permits more variation than the assembly can absorb. The parts pass inspection and still will not fit.
- Un-toleranced. Nothing named at all. Every bidder silently assumes a different standard, which is why the quotes cannot be compared even though they all look like numbers in the same currency.
Ruijin Fenghui has been machining and fabricating metal in Dongguan for over 23 years, with more than 200 machines across turning, milling, five-axis, stamping, sheet metal and finishing. We hold ±0.01 mm on machined features and return quotations within 24 hours. Everything below is written from the inspection bench, not from a marketing page — and where published sources disagree, we say so.
If you want the process-side context before diving into the numbers, start with our full sheet metal fabrication guide.
The three tolerance systems that can sit on one drawing
Most engineers assume a drawing runs on one sheet metal tolerance standard. A sheet metal drawing actually runs three systems side by side, and they are not equal partners.
System 1: general tolerances, ISO 2768-1
A general tolerance supplies the standard tolerances for sheet metal dimensions that carry no individual tolerance — one blanket value applied to everything you did not call out. It exists because you cannot realistically tolerance all sixty dimensions on a bracket, and because inspecting to nothing is worse than inspecting to something.
Here is the precedence rule that appears in almost no fabrication guide. When two rules could govern the same dimension, the order is: 1) an individual callout, 2) a GD&T frame, 3) a process-specific standard, 4) the general note. ISO 2768-1 governs *only* those linear and angular dimensions that have no tolerance of their own. If that sentence is news to you, you have probably been over-relying on your title block.
ISO 2768-1:1989 remains published and was reviewed and confirmed in 2022, with a revision under development. Always check the edition you cite before release.
System 2: geometric tolerancing, ISO 1101 and ASME Y14.5
A size tolerance does not control position. A hole called Ø10 ±0.1 can sit 0.5 mm off its nominal location and still be a perfectly legal Ø10 ±0.1 hole. You need geometric dimensioning and tolerancing — formally, ISO 1101 or ASME Y14.5 — for three things that show up constantly on sheet metal:
- Position tolerance on hole patterns that share a plane and must accept fasteners.
- Profile tolerance on formed contours and flanged edges.
- Flatness on sealing faces, mounting pads, and any surface that touches a machined part.
Datum selection matters more than the tolerance value: your datums must describe how the part is actually fixtured on the brake and in the gauge, or the inspection result will be unrepeatable.
System 3: process-specific standards that override all of the above
This is where most drawings fail. Four separate process standards govern specific sheet metal operations, and each one supersedes the general sheet metal tolerance standard on the features it covers:
Position callouts are where most of that argument lands, and our true position tolerance guide explains why the datum order moves the reported number more than the machine does.
- ISO 9013:2017 — quality of thermal cut edges (laser, plasma, flame).
- DIN 6930-2 and DIN 6935 — limit dimensions and angular deviation for cold-formed parts.
- ISO 13920:2023 — general tolerances for welded constructions.
- GB/T 13914 — dimensional tolerances of stamped parts, which is what a Chinese stamping shop is most likely inspecting to.
Buyers routinely leave these out, which is precisely why welded overall dimensions and formed lengths are the features that fail first.
ISO 2768-1: the actual permitted deviations for all four classes
Reading the table is mechanical: the class letter selects a column, the nominal size band selects a row, and the cell is the permitted deviation in millimetres. Most errors we see are people doing one of those two steps wrong.
Welded construction carries its own tolerance classes; the joining side is covered in our sheet metal welding guide.
| Nominal size (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 – 3 | ±0.05 | ±0.10 | ±0.20 | — |
| >3 – 6 | ±0.05 | ±0.10 | ±0.30 | ±0.50 |
| >6 – 30 | ±0.10 | ±0.20 | ±0.50 | ±1.00 |
| >30 – 120 | ±0.15 | ±0.30 | ±0.80 | ±1.50 |
| >120 – 400 | ±0.20 | ±0.50 | ±1.20 | ±2.50 |
| >400 – 1000 | ±0.30 | ±0.80 | ±2.00 | ±4.00 |
| >1000 – 2000 | ±0.50 | ±1.20 | ±3.00 | ±6.00 |
| >2000 – 4000 | ±0.80 | ±2.00 | ±4.00 | ±8.00 |
The second half of any sheet metal tolerances chart is angular. Angular dimensions are not banded by their own value at all — they are banded by the length of the shorter of the two legs forming the angle, expressed in degrees and minutes:
| Length of shorter side (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| ≤ 10 | ±1°00′ | ±1°00′ | ±1°30′ | ±3°00′ |
| >10 – 50 | ±0°30′ | ±0°30′ | ±1°00′ | ±2°00′ |
| >50 – 120 | ±0°20′ | ±0°20′ | ±0°30′ | ±1°00′ |
| >120 – 400 | ±0°10′ | ±0°10′ | ±0°15′ | ±0°30′ |
| > 400 | ±0°05′ | ±0°05′ | ±0°10′ | ±0°20′ |
Part 1 also covers external radii and chamfer heights, a row usually overlooked entirely. Published values for those rows differ between reprints, so read them off the edition you are citing rather than from a web page.
A caution worth more than the table itself. Published copies of this table circulate in shifted form. One well-known fabricator blog labels a row "3–30 mm" while printing the values that belong to >6–30. Another prints the coarse column under a medium heading. A third claims "ISO 2768-m allows ±0.15 mm up to 30 mm" — a value that appears in no column of the standard. So: check the class column and the nominal band row independently, and cite the edition.
And never confuse a class with a capability. ISO 2768-m at 30–120 mm permits ±0.30 mm, while a fibre laser routinely holds ±0.05–0.10 mm on the same cut feature. The class is a contract default; it is not a ceiling, and it is not a promise. Specify the class for the contract, and individual callouts for the function.
ISO 2768-mK meaning: the geometric classes, and why to stop writing it
The ISO 2768-mK meaning is two standards compressed into four characters, and every guide to ISO 2768 sheet metal work has to deal with the legacy shorthand. A drawing that says "ISO 2768-mK" means: general linear tolerances per ISO 2768-1 class m, plus general geometrical tolerances per ISO 2768-2 class K. Here are the class K family values:
| Nominal size of longer side (mm) | H | K | L |
|---|---|---|---|
| ≤ 10 | 0.02 | 0.05 | 0.10 |
| >10 – 30 | 0.05 | 0.10 | 0.20 |
| >30 – 100 | 0.10 | 0.20 | 0.40 |
| >100 – 300 | 0.20 | 0.40 | 0.80 |
| >300 – 1000 | 0.30 | 0.60 | 1.20 |
| >1000 – 3000 | 0.40 | 0.80 | 1.60 |
That table is straightness and flatness. Perpendicularity is banded by the shorter side: class H/K/L give 0.2/0.4/0.6 up to 100 mm, 0.3/0.6/1.0 for >100–300, 0.4/0.8/1.5 for >300–1000, and 0.5/1.0/2.0 for >1000–3000. Symmetry follows the longer side at 0.5/0.6/0.6 up to 100 mm rising to 0.5/1.0/2.0 above 1000 mm. Circular run-out is a single value per class: 0.1 / 0.2 / 0.5.
The part almost nobody says out loud: ISO lists ISO 2768-2 as withdrawn. Its successor, ISO 22081:2021, governs general geometrical specification — and it deliberately publishes no fixed value tables. You must now state your general geometrical requirement explicitly rather than borrowing a letter. Older drawings carrying -mK or -fH remain valid to the revision they cite; do not silently reinterpret them under 22081, because doing so can change the conformance of parts already in your warehouse.
Process-specific standards: what actually governs cut, bent and welded features
ISO 9013:2017 — thermal cut quality
This standard grades the cut face, not the part. Two characteristics decide it: perpendicularity or angularity tolerance u, and mean profile height Rz5, both functions of material thickness a in millimetres. There are four quality ranges:
If the part starts on a laser, our laser cutting guide gives the kerf, gas and tolerance picture behind that number.
| Range | Perpendicularity / angularity u (mm) | Mean profile height Rz5 (µm) |
|---|---|---|
| Range 1 | u ≤ 0.05 + 0.003a | Rz5 ≤ 10 + 0.6a |
| Range 2 | u ≤ 0.15 + 0.007a | Rz5 ≤ 40 + 0.8a |
| Range 3 | u ≤ 0.40 + 0.010a | Rz5 ≤ 70 + 1.2a |
| Range 4 | u ≤ 0.80 + 0.020a | Rz5 ≤ 110 + 1.8a |
Worked: on 3 mm steel, Range 1 permits u = 0.059 mm and Rz5 = 11.8 µm; on 10 mm, u = 0.08 mm and Rz5 = 16 µm. Range 1 is realistic on thin sheet with nitrogen assist, and it is roughly what shops mean when they advertise a ±0.05 mm laser cutting tolerance. Note that classification takes the worse of the two measured values — a beautiful edge angle with a rough profile still lands in Range 3.
Critically, dimensional accuracy of the part is not governed here. That is still ISO 2768-1. Laser cutting tolerance has two different answers depending on which question you meant: the edge quality (ISO 9013) or where the hole landed (ISO 2768-1 plus machine capability).
DIN 6930-2 and DIN 6935 — the bending tolerance chart for formed steel parts
DIN 6935 gives cold-bend angular deviation by the shortest leg: ±2°00′ up to 30 mm, ±1°45′ for >30–50, ±1°30′ for >50–80, ±1°15′ for >80–120, and ±1°00′ above 120 mm. Compare that with the ISO 2768-1 angular table above and you will see the gap: at a 30 mm leg, ISO class m permits ±30 arcminutes while DIN 6935 permits two full degrees. DIN 6935 is the realistic frame for a press-brake part. Those five values are what a production bending tolerance chart actually looks like once you stop quoting machine specifications, and they belong on any sheet metal tolerances chart you keep beside the brake.
DIN 6930-2 covers limit dimensions for formed lengths at accuracy grade m, and its defining insight is that material thickness matters as much as nominal size — something ISO 2768 ignores entirely:
| Nominal length (mm) | t ≤ 1 | t 1–3 | t 3–6 | t 6–10 | t > 10 |
|---|---|---|---|---|---|
| to 6 | ±0.20 | ±0.30 | ±0.40 | ±0.60 | ±0.80 |
| >6 – 10 | ±0.30 | ±0.40 | ±0.50 | ±0.80 | ±0.80 |
| >10 – 25 | ±0.40 | ±0.50 | ±0.60 | ±0.80 | ±1.20 |
| >25 – 63 | ±0.50 | ±0.60 | ±0.80 | ±1.00 | ±1.20 |
| >63 – 160 | ±0.60 | ±0.80 | ±1.00 | ±1.20 | ±1.60 |
| >160 – 400 | ±1.00 | ±1.20 | ±1.20 | ±1.60 | ±2.00 |
| >400 – 1000 | ±1.60 | ±1.60 | ±2.00 | ±2.00 | ±3.00 |
| >1000 – 2500 | ±2.40 | ±3.00 | ±3.00 | ±4.00 | ±4.00 |
These values are reproduced from published extracts rather than read off the licensed DIN original — verify against your own copy before contractual use.
If the flat-pattern side of this interests you, our bend allowance and K-factor breakdown covers the maths behind why the flat develops at all.
ISO 13920:2023 — welded constructions
Welding tolerance ISO 13920 is the least-covered and cheapest-to-win topic in this whole space. It gives two families: classes A–D for length and angle, classes E–H for shape and position.
| Nominal size (mm) | Class A | Class B | Class C | Class D |
|---|---|---|---|---|
| 2 – 30 | ±1 | ±2 | ±3 | ±4 |
| >30 – 120 | ±1 | ±2 | ±4 | ±7 |
| >120 – 400 | ±1 | ±3 | ±6 | ±9 |
| >400 – 1000 | ±2 | ±4 | ±8 | ±12 |
| >1000 – 2000 | ±3 | ±6 | ±11 | ±16 |
| >2000 – 4000 | ±4 | ±8 | ±14 | ±21 |
| >4000 – 8000 | ±5 | ±10 | ±18 | ±27 |
| >8000 – 12000 | ±6 | ±12 | ±21 | ±32 |
Angular tolerances use three bands by the shorter side — l ≤ 400 (±20′/±45′/±1°/±1°30′ for A/B/C/D), 400 < l ≤ 1000 (±15′/±30′/±45′/±1°15′), and l > 1000 (±10′/±20′/±30′/±1°). Four-band versions circulating online are not the published standard. Straightness, flatness and parallelism classes E/F/G/H run from 0.5/1/1.5/2.5 mm at 30 mm up to 8/16/25/40 mm at 20 000 mm.
Class B is the practical production default and is the level referenced by EN 1090-2 for Execution Class 2–3 work. ISO 13920 deliberately excludes weld-bead imperfections — that is ISO 5817, and you should cite both, separately.
GB/T 13914 — what a Chinese stamping shop is measuring to
If you buy stamped parts from China and your drawing names no standard, there is a good chance the inspection sheet is written to GB/T 13914, which uses two families: ST1–ST11 for flat/blanked parts and FT1–FT10 for formed parts. FT grades are systematically looser than their ST equivalents because springback introduces variation that a flat blank never sees.
The commercial sweet spot is ST3–ST5 and FT3–FT5. ST1/ST2 and FT1/FT2 exist but are rare and expensive. This matters commercially: if your supplier's inspection report cites ST/FT grades and your drawing cites nothing, you are being inspected to a different sheet metal fabrication tolerance standard than you think — and you will lose the argument when parts disagree. See also our deeper articles on sheet metal stamping, progressive die stamping and compound die stamping.
Feature by feature: which sheet metal fabrication tolerances a supplier can really hold
Capability and the standard are two different answers. Sheet metal fabrication tolerances are what the drawing permits; capability is what the machine actually repeats on a good Tuesday — ±0.05 mm on a hole cut in one plane, ±0.20–0.50 mm once the dimension crosses a bend. Design to this table, not to the class letter.
| Feature | Same plane / as-cut | Across one or more bends | Notes |
|---|---|---|---|
| Hole diameter | ±0.05 – ±0.10 | n/a | Degrades as thickness-to-diameter rises; min hole ≈ 1×t |
| Hole-to-hole centre distance | ±0.05 – ±0.10 | ±0.20 – ±0.50 | Add the per-bend allowance below |
| Hole-to-edge | ±0.10 – ±0.15 | ±0.25 – ±0.40 | Keep ≥1×t, recommend 1.5×t |
| Slot width | ±0.05 – ±0.10 | ±0.20 – ±0.40 | Min slot width ≈ 1×t |
| Bend angle | ±0.5° – ±1.0° | ±1.0° – ±2.0° on long bends | Springback plus thickness variation |
| Bend-to-hole | n/a | ±0.25 – ±0.40 | The most over-toleranced dimension in the industry |
| Overall formed dimension | ±0.20 – ±0.30 (one bend) | ±0.50 – ±1.00 (three or more) | See the sheet metal tolerance stack-up rule |
| Flatness, as-cut sheet | 0.2 – 2.0 mm over 1 m | n/a | Raw stock flatness is a hard floor |
| PEM / self-clinching insert location | ±0.05 – ±0.12 | ±0.25 – ±0.40 | Hole size must follow the fastener maker exactly — see our precision fasteners guide |
| Welded assembly overall | n/a | ±0.5 – ±2.0 (ISO 13920 B/C) | Distortion governs, not machine accuracy |
Two honest conclusions follow from this sheet metal tolerances chart. Cut features hold tight; formed and welded features drift. If your real question is how tight can sheet metal tolerances be, the answer is ±0.05 mm on a same-plane feature, and nothing tighter without a second operation. That is physics, not quality control. And note the flatness row: a fabricator generally cannot improve the flatness of the raw coil by cutting it. A realistic specification acknowledges the mill's own flatness tolerance instead of inventing one.
When a feature genuinely needs ±0.01 mm, it has stopped being a sheet metal feature. Machine it after forming — that is our ±0.01 mm CNC capability — or rethink the datum. Our sheet metal fabrication line and precision stamping cell both feed straight into that machining step under one roof.
Four quantified rules that most tolerance guides skip
Rule 1: sheet metal tolerance stack-up across bends, as an equation
Sheet metal tolerance stack-up starts here: a dimension that crosses n bends does not inherit the single-bend tolerance, it accumulates it. The worst-case formula is:
T(n) = T₀ + n · k · t
where T₀ is the equipment baseline, about 0.15 mm in a modern brake; n is the number of bends the dimension crosses; k is roughly 0.05, i.e. about five per cent of material thickness; and t is thickness in millimetres. For a 2 mm part crossing four bends: T = 0.15 + 4 × 0.05 × 2 = ±0.55 mm.
What a running line actually delivers is closer to root-sum-square:
T(n) = √(T₀² + n·(k·t)²)
For the same part: √(0.15² + 4 × 0.10²) = ±0.25 mm. Use worst-case when you have no process data and no buffers; use RSS once you do. What you must not do is apply worst-case maths and *also* demand a tight callout — that is paying twice for the same risk. The corollary is more valuable than either formula: dimension critical features from the same flat surface. Removing two bends from a chain is worth more than any inspection you can buy, and it is free. See our DFM review guide for how we flag this before tooling.
Rule 2: coating build-up eats your clearance
Usable clearance = designed clearance − 2 × coating thickness per surface, expressed diametrally.
Powder coat typically builds 60–120 µm per surface. Anodize Type II is around 5–25 µm, Type III hardcoat 25–75 µm, with roughly half of that growing outward. Now take an H7/g6 slip fit on Ø20: its designed clearance is only 0.007–0.041 mm. A 60 µm powder coat on the male part alone consumes 0.120 mm of that — three to seventeen times the entire designed band. The part is seized before it is assembled, having passed inspection.
Fixes, in order of cost: mask the fit surfaces, specify coating thickness *with a measurement method* on the drawing, or design the clearance for the post-coat condition. Read more in our finishing and dimension guide and the anodizing build-up deep dive.
Rule 3: why ±0.2 mm on a 1 m part is not a specification
ISO 2768-1 class f — the finest class the standard offers — permits ±0.30 mm up to 1000 mm and relaxes to ±0.50 mm beyond it. Calling ±0.2 mm on a 1 m dimension therefore asks for 1.5× better than the standard's own best class, and 2.5× better the moment the part passes a metre — and none of that accounts for thermal expansion. Steel moves about 12 µm per metre per °C; aluminium about 23 µm. A 1 m aluminium part measured 10 °C away from the ISO 1 reference temperature of 20 °C shifts 0.23 mm — your entire tolerance band, spent on the thermometer.
Either specify measurement at 20 °C and say so on the drawing, or do not write ±0.2 mm on a metre.
Rule 4: worst-case versus RSS across an assembly
Five features at ±0.10 mm each: worst-case gives ±0.50 mm, RSS gives ±0.22 mm. RSS is defensible because not every feature sits at its limit simultaneously — it reflects roughly 3σ coverage — and it lets you loosen individual tolerances while holding the assembly result. This is usually the single cheapest cost reduction available to a buyer, and it requires no change to the part at all.
Cost–tolerance: which bands are free and which multiply
We will not quote you a dollar figure that will be wrong next quarter. What does hold across markets is the *shape* of the curve: as sheet metal fabrication tolerances tighten, the index below shows where the price stays flat and where it turns. It is scaled so that 1.0 is a default ISO 2768-m, as-cut-and-formed part with standard inspection.
| Tolerance band | Example | Relative cost index | What actually changes on the floor |
|---|---|---|---|
| ISO 2768-c or looser | ±1.2 mm at 120–400 | 0.9 – 1.0 | Nothing |
| ISO 2768-m (default) | ±0.3 mm at 30–120 | 1.00 | Baseline process |
| ISO 2768-f on cut features | ±0.10 mm at 6–30 | 1.1 – 1.3 | Slower cut, calibrated machine, tighter pierce control |
| ISO 2768-f across bends | ±0.15 mm linear, ±0.5° | 1.3 – 1.8 | In-process angle measurement, trial bends, sorted material |
| Tighter than process capability | ±0.05 mm formed | 2.0 – 3.0+ | Dedicated fixture, 100% CMM, rework allowance in the price |
| Tighter than sheet metal physics | ±0.01 mm | — | Not a sheet metal operation. Machine it after forming. |
Three practical notes. Multipliers add across features, not parts — tightening three dimensions out of forty should not triple the price, and if a quote says otherwise, the shop has priced the whole drawing to the tightest single callout, which is a genuine red flag worth challenging. The cheapest saving is almost always deleting callouts rather than loosening them. And when in doubt, mark the three to five dimensions that control function and let the general note carry the rest. The same logic drives the cost model in our machining guide.
How to specify sheet metal fabrication tolerances on the drawing
The tolerance block, line by line
This is a sheet metal drawing tolerance callout set you can paste into a title block. Each line replaces a paragraph of argument later.
| Line | Wording to paste |
|---|---|
| General linear and angular | GENERAL TOLERANCES: ISO 2768-1 CLASS m UNLESS OTHERWISE SPECIFIED. |
| Geometry | GENERAL GEOMETRICAL SPECIFICATION: PER ISO 22081:2021. LEGACY ISO 2768-2 CLASS K NOT APPLICABLE. |
| Cut edges | THERMAL CUT EDGES: ISO 9013 RANGE 2 UNLESS NOTED. |
| Bends | BEND ANGLE ±1.0°. FORMED LENGTHS PER DIN 6930-2 GRADE m UNLESS NOTED. |
| Welds | WELDED CONSTRUCTION: ISO 13920 CLASS B. WELD QUALITY: ISO 5817 LEVEL C. |
| Coating | POWDER COAT 60–100 µm PER SURFACE. CRITICAL FIT DIMENSIONS X, Y, Z ARE POST-COAT. |
| Material | MATERIAL THICKNESS PER ASTM A480 / EN 10130. MEASURE AND RECORD ACTUAL THICKNESS BEFORE BENDING. |
| Inspection | FAI REQUIRED. CMM REPORT FOR DIMENSIONS MARKED ▶. |
"UNLESS OTHERWISE SPECIFIED" is a legal sentence, not a courtesy. It must name the standard, the class, and the edition. A note reading "Tolerances ±0.1 unless noted" is not a sheet metal drawing tolerance callout — it is an invitation to argue later. The eight lines above are what one actually looks like.
Bad versus good callouts
| Bad callout | Why it fails | Write this instead |
|---|---|---|
| ALL DIMENSIONS ±0.05 | Prices every cosmetic edge to the tightest functional requirement | ISO 2768-m general, plus ±0.05 on the three marked functional dimensions |
| Ø10 HOLE (bare) | Size falls to the general note and position is simply uncontrolled | Ø10 ±0.05 with position Ø0.15 A-B-C |
| 90° BEND | Tip position floats; at 0.5° over a 60 mm leg the tip moves ~0.5 mm | 90° ±0.5° plus a bend-to-hole dimension from the datum face |
| FLAT AND SQUARE | Unmeasurable, therefore unenforceable | FLATNESS 0.4 OVER 300 mm (explicit value and span) |
| ±0.2 ON 1000 | Below ISO 2768-f at this size, and below thermal drift | ±0.5, or machine the feature after forming |
On cosmetic versus functional surfaces specifically — the distinction shows up constantly on our amplifier front panels and brushed aluminium audio panels — name the cosmetic requirement in a note and keep it out of the dimensional callouts entirely.
Inspection and verification: what to ask for, and when
| What you need | Method | Why |
|---|---|---|
| Overall size, non-critical | Caliper or tape | Fast, adequate for ±0.5 mm bands |
| Hole pattern on one plane | Go/no-go pin gauge or optical comparator | Cheapest way to prove a pattern at volume |
| Anything at ±0.05 mm or tighter | CMM | Operator-independent and produces a record |
| Formed or welded 3D geometry | Portable CMM arm or laser scan | A fixed CMM cannot reach most formed datums |
| First piece of a new programme | FAI / FAIR | It proves the *process*, not the part |
Ask for a first article inspection when it is a new part or a new supplier, when the drawing carries tolerances tighter than ISO 2768-m across bends, or when the part mates with a machined component. Do not ask for a full CMM report on a ±0.5 mm bracket — you are buying inspection, not quality. Pair it instead with sensible prototyping rather than paper.
The governing rule: the gauge must be able to resolve the tolerance. Aim for resolution no coarser than one tenth of the band. A 0.02 mm-resolution caliper cannot adjudicate a ±0.05 mm callout, whatever the display implies. And always state whether critical dimensions are pre-coat or post-coat — most assembly disputes trace to that one missing sentence.
Whether the gauge can repeat that reading at all is a separate question, answered by a gage repeatability and reproducibility study.
We are certified to IATF 16949, ISO 9001 and ISO 13485, and every programme ships with the inspection record the drawing asked for. If you are comparing vendors, our supplier evaluation guide lists the metrology questions worth asking.
RFQ checklist: twelve things to write before you send the drawing
- Name the general standard and its class in the title block, including edition or year.
- List the three to eight dimensions that actually control function, and tolerance only those.
- State how many bends each critical dimension crosses.
- Say whether critical dimensions are pre-coat or post-coat, and give the coating thickness range.
- Give material and thickness with its mill tolerance, and ask for actual thickness to be measured before bending.
- Specify cut-edge quality by ISO 9013 range if the edge seals, welds, or is visible.
- State your welding tolerance the standard way: ISO 13920 class A–D for the assembly, separately from weld quality per ISO 5817.
- Give the hole-to-bend minimum distance — at least 2.5–3× t plus the inside radius — or accept the distortion.
- Mark which dimensions need a CMM report and leave the rest to standard inspection.
- State whether an FAI is required and to which standard; see our part traceability guide for serialisation options.
- Confirm the measurement temperature (ISO 1: 20 °C) for anything tight on a large part.
- Ask your supplier to quote the part twice: once as drawn, once with their recommended relaxation. The gap between the two numbers is the most useful feedback you will get.
None of the twelve items above asks you to tighten anything — a good sheet metal fabrication tolerances specification mostly consists of removing callouts you did not need. Then send the STEP file plus a PDF carrying the tolerance block, and ask for a DFM review on any callout you are unsure about. Getting those twelve decisions right matters more than getting the material right.
FAQ
What are standard sheet metal fabrication tolerances?
Standard sheet metal fabrication tolerances are ISO 2768-1 class m for most commercial work: ±0.10 mm at 0.5–3 mm nominal, ±0.20 mm at >6–30, ±0.30 mm at >30–120, ±0.50 mm at >120–400. Angular features follow the shorter leg: ±30 arcminutes from 10–50 mm. Individual processes may hold tighter.
What is the ISO tolerance standard for sheet metal?
There is no single sheet metal tolerance standard — four share the load: ISO 2768-1 for general linear and angular tolerances, ISO 22081:2021 for general geometrical specification, ISO 9013:2017 for thermal cut edges, and ISO 13920:2023 for welded constructions. DIN 6930-2 and DIN 6935 cover formed lengths and cold-bend angles.
The quantity where the two routes cross is the whole decision: our stamping vs laser cutting comparison shows the formula and a worked bracket.
What does ISO 2768-m mean on a drawing?
ISO 2768-m invokes ISO 2768-1 class m — the ISO 2768 sheet metal default — for any dimension carrying no individual callout. It is a contractual fallback, not a capability promise — a laser may well hold ±0.05 mm where class m permits ±0.20 mm. Individual callouts always override it.
How tight can sheet metal tolerances be?
About ±0.05 mm on cut features, and ±0.20–0.50 mm once a dimension crosses a bend. Cut features routinely reach ±0.05–0.10 mm on hole diameter and hole-to-hole distance in one plane. Formed dimensions are looser: ±0.20–0.30 mm across one bend, ±0.50–1.00 mm across three or more, because each bend adds roughly five per cent of material thickness to the chain. Below that, machine it after forming.
Is ISO 2768-2 still valid, and what replaced it?
No — ISO lists ISO 2768-2 as withdrawn. ISO 22081:2021 succeeded it for general geometrical specification and publishes no fixed value tables, so you must state the requirement explicitly. Legacy drawings citing -mK or -fH remain valid to the revision they cite — do not reinterpret them silently.
What tolerance should I use for a bend angle?
±1.0° is a safe production default for press-brake work: it sits in the middle of every bending tolerance chart above and matches DIN 6935 roughly. ±0.5° is achievable with in-process angle measurement and sorted material, at a cost penalty. Remember that an angular tolerance does not locate the flange tip — add a bend-to-hole dimension if tip position matters.
What is the ISO standard for laser cutting tolerance?
ISO 9013:2017 classifies the cut face — perpendicularity u and mean profile height Rz5 — across four quality ranges. On 3 mm steel, Range 1 permits u ≤ 0.059 mm. The part's dimensional accuracy is separately governed by ISO 2768-1; the two standards answer different questions.
Does powder coating change sheet metal dimensions?
Yes. Powder coat typically builds 60–120 µm per surface, consuming twice that diametrally on a shaft-in-hole fit. On an H7/g6 Ø20 fit whose designed clearance is only 0.007–0.041 mm, a 60 µm coating seizes the assembly. Mask the fit surfaces or design the clearance for the post-coat condition.
Where to go from here
Get three decisions right and ninety per cent of tolerance disputes disappear: name the class, tolerance only what functions, and ask for two quotes. Those three turn sheet metal fabrication tolerances from a negotiation back into a specification. Everything else on this page is backup for the argument.
Our sheet metal team supports audio chassis, automotive brackets and 3C electronics housings with the finishing lines in the same building. Send a STEP file and a PDF carrying your tolerance block for a quotation inside 24 hours — with any unachievable callout flagged before the laser starts cutting. See our inside-line finishing capability, or read about our work in audio equipment, automotive and 3C electronics. Start here.
References
- ISO 2768-1:1989, *General tolerances — Part 1: Tolerances for linear and angular dimensions without individual tolerance indications* (still published; reviewed and confirmed 2022).
- ISO 22081:2021, *Geometrical product specifications (GPS) — Geometrical tolerancing — General geometrical specification* — successor to the withdrawn ISO 2768-2.
- ISO 9013:2017, *Thermal cutting — Classification of thermal cuts — Geometrical product specification and quality tolerances*.
- ISO 13920:2023 — Welding: general tolerances for welded constructions
- ISO 1101:2017, *Geometrical product specifications (GPS) — Geometrical tolerancing*; and ISO 8015, *GPS — Fundamentals — Concepts, principles and rules* (the independence principle).
- ASME Y14.5-2018 — Dimensioning and Tolerancing
- The Fabricator — Reasonable tolerancing for press brake bending
- GB/T 13914, *Dimensional tolerances of stamping parts* (ST1–ST11 / FT1–FT10) — the grade system most Chinese stamping inspection reports are written to. Confirm the current edition in your own standards subscription before citing it contractually.
Note also that ISO 1 fixes 20 °C as the reference temperature for geometrical and dimensional measurement. Standards get revised: before any standard number goes into a purchase order or a drawing title block, confirm its edition and status in your own subscription — several general-tolerance standards have changed status recently, and a withdrawn reference is unenforceable.