Most drawings that arrive at our shop carry one line that determines how hundreds of dimensions will be judged: a general tolerance note. Usually it reads ISO 2768-mK or ISO 2768-m, sometimes just "general tolerances per ISO 2768".
That one line is doing a lot of work. It defines the acceptable variation on every dimension you did not tolerance individually — and, read wrongly, it is the source of more rejected parts and assembly surprises than any other single item on a drawing.
This page lays out the actual ISO 2768 tables, explains which class to choose, and covers the part most articles skip: what the standard does not mean, and where buyers get caught by it.
ISO 2768 in one paragraph
ISO 2768 is a two-part standard for general tolerances — the default rules that apply to dimensions without an individual tolerance.
- ISO 2768-1 covers linear and angular dimensions (lengths, radii, chamfers, angles).
- ISO 2768-2 covers geometric tolerances (straightness, flatness, perpendicularity, symmetry, run-out).
You invoke it with a note on the drawing. ISO 2768-mK means: medium class for linear and angular dimensions (Part 1), class K for geometric tolerances (Part 2). Every dimension without its own tolerance box is then governed by those tables.
The reason the standard exists is simple economics. A drawing with an individual tolerance on all 200 dimensions is unreadable and takes an engineer a day to produce. A general note plus individual callouts on the handful of functional features communicates the same intent in two minutes.
ISO 2768-1: linear tolerances (the main table)
This is the tolerance chart you will use most. All values are in millimetres, applied as ±.
| Nominal size range (mm) | f — fine | m — medium | c — coarse | v — very coarse |
|---|---|---|---|---|
| 0.5 to 3 | ±0.05 | ±0.1 | ±0.2 | — |
| Over 3 to 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| Over 6 to 30 | ±0.1 | ±0.2 | ±0.5 | ±1.0 |
| Over 30 to 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| Over 120 to 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| Over 400 to 1000 | ±0.3 | ±0.8 | ±2.0 | ±4.0 |
| Over 1000 to 2000 | ±0.5 | ±1.2 | ±3.0 | ±6.0 |
| Over 2000 to 4000 | — | ±2.0 | ±4.0 | ±8.0 |
Two observations that matter in practice:
The tolerance scales with size. A 20mm feature under class m is ±0.2mm; a 500mm feature is ±0.8mm. This is not arbitrary — thermal expansion, machine geometry and measurement uncertainty all grow with size. When you see a drawing that calls ±0.1mm on a 600mm-long aluminium profile, someone has not looked at the table.
The jump from f to m is not a rounding difference. On a 30-120mm feature, class f is ±0.15mm and class m is ±0.3mm. Specifying f because "tighter is better" doubles the band you are demanding across every untoleranced dimension on the part — and it is charged for.
ISO 2768-1: angular tolerances
Angular tolerances depend on the length of the shorter side of the angle, not on the angle itself.
| Length of shorter side (mm) | f — fine | m — medium | c — coarse | v — very coarse |
|---|---|---|---|---|
| Up to 10 | ±1° | ±1° | ±1°30′ | ±3° |
| Over 10 to 50 | ±0°30′ | ±0°30′ | ±1° | ±2° |
| Over 50 to 120 | ±0°20′ | ±0°20′ | ±0°30′ | ±1° |
| Over 120 to 400 | ±0°10′ | ±0°10′ | ±0°15′ | ±0°30′ |
| Over 400 | ±0°5′ | ±0°5′ | ±0°10′ | ±0°20′ |
Note that f and m are identical for angular dimensions. That surprises people who assume "fine" always means tighter. If your angular requirements are driven by the general note, moving from m to f buys you nothing at all.
Also worth internalising: an angular tolerance of ±0.5° on a 100mm arm translates to roughly ±0.87mm of linear movement at the far end. Angles are a convenient way to specify position, and a very unforgiving one when the feature is long. On a long part, control the linear dimension at the point that matters rather than the angle.
ISO 2768-2: geometric tolerances
Part 2 defines three classes: H (tightest), K (middle, and by far the most common), and L (most relaxed). It is normally invoked together with Part 1 — hence the familiar ISO 2768-mK.
Straightness and flatness
| Range (mm) | H | K | L |
|---|---|---|---|
| Up to 10 | 0.02 | 0.05 | 0.1 |
| Over 10 to 30 | 0.05 | 0.1 | 0.2 |
| Over 30 to 100 | 0.1 | 0.2 | 0.4 |
| Over 100 to 300 | 0.2 | 0.4 | 0.8 |
| Over 300 to 1000 | 0.3 | 0.6 | 1.2 |
| Over 1000 to 3000 | 0.4 | 0.8 | 1.6 |
Perpendicularity
| Range (mm) | H | K | L |
|---|---|---|---|
| Up to 100 | 0.2 | 0.4 | 0.6 |
| Over 100 to 300 | 0.3 | 0.4 | 1.0 |
| Over 300 to 1000 | 0.4 | 0.4 | 1.5 |
| Over 1000 to 3000 | 0.5 | 0.5 | 2.0 |
Symmetry
| Range (mm) | H | K | L |
|---|---|---|---|
| Up to 100 | 0.5 | 0.6 | 0.8 |
| Over 100 to 300 | 0.5 | 0.6 | 1.0 |
| Over 300 to 1000 | 0.5 | 0.6 | 1.5 |
| Over 1000 to 3000 | 0.5 | 0.6 | 2.0 |
Circular run-out
| Range (mm) | H | K | L |
|---|---|---|---|
| Over 0.5 to 3 | 0.1 | 0.2 | 0.2 |
| Over 3 to 6 | 0.1 | 0.2 | 0.2 |
| Over 6 to 30 | 0.1 | 0.2 | 0.2 |
| Over 30 to 120 | 0.1 | 0.2 | 0.2 |
| Over 120 to 400 | 0.1 | 0.2 | 0.3 |
| Over 400 to 1000 | 0.1 | 0.3 | 0.4 |
| Over 1000 to 3000 | 0.1 | 0.3 | 0.4 |
If you only remember one thing from this section: mK is the default pairing for general machining. Class m for dimensions, class K for geometry. It is what most shops assume when a drawing says nothing more specific, and it is the pairing we see on the majority of drawings from Europe and North America.
⚠️ The default-tolerance trap
Here is the failure mode this standard causes most often, and it has nothing to do with the table values.
A buyer sends a drawing with the note ISO 2768-m and no individual tolerances. The part is a machined aluminium housing with a bearing bore, two dowel-pin holes for a mating cover, and a sealing face. The drawing does not call out any of those three features.
The shop reads the drawing correctly. Every dimension — including the bearing bore — is governed by ISO 2768-m. On a 25mm bore, that is ±0.2mm. The parts are machined within that band and inspected to it. They pass.
At assembly, the bearing will not seat properly, the cover will not align to the dowel pins, and the seal leaks.
Nothing illegal happened. The drawing said what it said.
| Feature | What the drawing communicated | What the part needed | Result |
|---|---|---|---|
| Bearing bore Ø25 | ISO 2768-m → ±0.2mm | ±0.01mm (H7 fit) | Bearing loose or seized |
| Dowel holes Ø6 | ISO 2768-m → ±0.1mm | ±0.02mm position | Cover misaligned |
| Sealing face | ISO 2768-mK → flatness 0.1mm | 0.02mm flatness | Leak path |
The rule this illustrates: the general tolerance note is a floor, not a specification. It covers the dimensions you genuinely do not care about. Every feature that fits, seals, aligns, rotates or carries load must be toleranced individually, because those are the features whose variation causes the part to fail at the assembly stage rather than at the inspection stage.
A useful test before sending an RFQ: go through the drawing and mark every feature that touches another part, carries a load, or forms a seal. If any of them has no individual tolerance, the general note is standing in for a functional requirement it was never meant to express.
Standard ≠ capability: the misconception that costs buyers money
ISO 2768-m allows ±0.2mm on a 25mm dimension. It is a common misreading of the standard to conclude that a shop working to ISO 2768-m "can only hold ±0.2mm".
The tolerance you grant and the tolerance a shop can achieve are two different numbers.
| Feature (25mm nominal) | ISO 2768 class limit | What a competent CNC shop actually holds |
|---|---|---|
| Non-critical outline | m: ±0.2mm | ±0.2mm (deliberately — no reason to do better) |
| General machined feature | m: ±0.2mm | ±0.05mm routinely, at no extra cost |
| Precision feature | f: ±0.1mm | ±0.01mm as standard practice |
| Critical bore | f: ±0.1mm | ±0.005mm on a stable machine, with inspection |
This matters in two directions.
For buyers: specifying ISO 2768-m does not mean you are buying a low-precision part. It means you are declining to measure most of it. If your design needs ±0.01mm on three features, tolerance those three features — the shop will hold them, and the general note keeps the rest of the part affordable.
For the cost conversation: a quote for a part with an m general note and three tight features should not be much above a plain m part. If a shop quotes it 40% higher, ask what they are holding tight across the whole part — that is usually the answer, and it is usually unnecessary.
When to override the general tolerance
Every drawing needs individual tolerances somewhere. These categories always qualify:
| Feature type | Why the general note is not enough | Typical callout |
|---|---|---|
| Bearing bores, shaft seats | Determines fit, clearance, runout | Ø25 H7, or +0.021/0.000 |
| Mating faces, locating features | Determines assembly alignment | Position Ø0.1 M to datum, or ±0.02 |
| Sealing surfaces | Leak paths follow flatness, not size | Flatness 0.02, Ra 0.8 |
| Dowel and pin holes | Function is position, not diameter | Position Ø0.05 to datum |
| Threaded holes in critical joints | Determines clamp load and torque | Position, perpendicularity to face |
| Features controlling motion | Any variation shows up as play or bind | Coaxiality, run-out, position |
| Interfaces to purchased parts | Their tolerances are fixed; yours must match | Match the supplier's spec |
Everything else — outlines, non-mating faces, cosmetic radii, chamfers, cable clearance holes, pocket depths that only need to be deep enough — is exactly what the general tolerance class is for. Leaving them untoleranced is not laziness; it is correct practice, and it is what keeps the part affordable.
ISO 2768 and GD&T: which to use
They solve different problems, and a good drawing uses both.
ISO 2768 answers: "how much variation will I accept on the dimensions I have not thought about?"
GD&T answers: "what does this feature have to do for the part to work?" Position relative to a datum, flatness of a sealing face, perpendicularity of a bore axis — requirements that plus/minus tolerancing cannot express without ambiguity or over-tightening.
The common failure is not choosing one over the other. It is using ISO 2768 where GD&T was needed. A four-hole bolt pattern toleranced with ±0.1mm on each hole's X and Y coordinates, under a general note, produces a rectangular tolerance zone and no control over the pattern's relationship to any datum. The same pattern with 4× Ø8 position Ø0.1 M to A|B|C communicates exactly what matters, usually permits more manufacturing variation, and is cheaper to inspect.
For a deeper treatment of which callouts to write and what they cost, our CNC machining tolerances guide covers achievable tolerance by feature size and material, and the cost of tolerances article shows what each tightening step does to the price.
What ISO 2768 costs you
The class itself is not the main cost driver. What costs money is the number of features held tighter than the class.
| Drawing approach | Effect on price | Why |
|---|---|---|
ISO 2768-m, nothing else |
Baseline | Shop holds the loose band on everything |
ISO 2768-m + 3 tight features |
5–15% above baseline | Only three features need attention and inspection |
ISO 2768-f, nothing else |
20–40% above baseline | Tighter band on every untoleranced dimension |
ISO 2768-m + 15 tight features |
30–60% above baseline | Inspection and cycle time scale with feature count |
±0.02mm on everything (no general note) |
60–150% above baseline | Every dimension becomes a controlled feature |
The pattern is consistent with what we see on real quotes: tightening a few features is cheap; tightening everything is expensive. The f class is a blunt instrument — it tightens the whole drawing at once. Individual callouts are a scalpel.
If you want a quick self-check on a drawing: count the dimensions with individual tolerances. Under five is usually well optimised. Over twenty on a part that does not move or seal anything is usually inherited from a template.
Practical notes for drawings sent to China
A few points specific to sourcing from Chinese shops, since this is where most of our work comes from.
Write the note explicitly. "General tolerances: ISO 2768-mK" leaves nothing to interpretation. A drawing with no general note at all is genuinely ambiguous — shops will assume something, and their assumption may not match yours.
GB/T 1804 is equivalent. The Chinese national standard for general tolerances aligns with ISO 2768-1, so there is no translation problem in the values. If a supplier quotes to GB/T 1804-m, that is the same tolerance band as ISO 2768-m.
Put critical callouts in the drawing, not the email. Requirements that arrive in an email get lost between the RFQ and the shop floor. If a bore is H7, it belongs on the drawing revision the shop machines from.
Ask what the quote assumes. A line-item quote that lists material, machining, finishing and inspection separately lets you see whether the shop priced the tight features or quietly priced the whole part as though everything were tight. Our guide to reading a CNC quote explains what the line items should show.
Frequently asked questions
What is ISO 2768 in simple terms?
ISO 2768 is a two-part standard that sets default tolerances for dimensions you do not tolerance individually on a drawing. Part 1 covers linear and angular dimensions; Part 2 covers geometric tolerances like straightness, flatness and perpendicularity. On the drawing you write a single note such as "ISO 2768-mK", and every untoleranced dimension is then governed by that class instead of being left undefined.
Which ISO 2768 class should I use?
ISO 2768-m (medium) for linear and angular dimensions, combined with class K for geometric tolerances, is the most widely used pairing in general CNC machining and the safest default for most parts. Use f (fine) only when the part genuinely needs tighter untoleranced dimensions, and expect a higher price because the shop must hold it everywhere. Classes c and v suit welded fabrications, castings and non-critical parts.
Does ISO 2768-m mean the shop can only hold ±0.2mm?
No, and this is the most common misunderstanding. ISO 2768-m is the tolerance you are granting for untoleranced dimensions — the minimum you will accept, not the maximum the shop can achieve. A competent CNC shop holds ±0.01mm on critical features every day. If a feature needs to be tighter than the general class, tolerance it individually on the drawing; do not assume the general note covers it.
What happens if I only write ISO 2768-m and nothing else?
Every untoleranced dimension falls under medium-class limits — for example ±0.2mm on a 6–30mm feature and ±0.3mm on a 30–120mm feature. If a bearing bore or a mating face needs ±0.02mm, that requirement is not communicated, and parts will be made to the loose general tolerance and rejected at your incoming inspection. Critical features must always be toleranced individually.
What is the difference between ISO 2768 and ISO 286?
ISO 2768 sets general tolerances for untoleranced dimensions. ISO 286 defines fits between mating parts — the hole and shaft tolerance zones (H7, h6, g6 and so on). They complement each other: a drawing may carry an ISO 2768-mK general note for non-critical dimensions while specific mating features are called out as, for example, Ø25 H7.
Should I use ISO 2768 or GD&T?
Use both, for different things. ISO 2768 handles the dimensions nobody is going to measure — outlines, non-critical hole positions, cosmetic features. GD&T communicates functional requirements that a plus/minus tolerance cannot express: position of a hole pattern relative to a datum, flatness of a sealing face, coaxiality of two bores. Replacing GD&T with ISO 2768 everywhere usually means paying for precision on features that do not need it, or failing to communicate the ones that do.
Does ISO 2768 affect the price of my parts?
The general class affects price indirectly, through how much of the part the shop must hold to a tighter band. ISO 2768-m is routine work and priced as such. ISO 2768-f forces tighter control across every untoleranced dimension, which increases inspection and cycle time even if no individual feature is difficult. The bigger cost driver is not the class itself but how many features you tighten beyond it.
Is ISO 2768 used in China?
Yes. Chinese CNC shops quote and machine to ISO 2768 routinely, and "ISO 2768-m" or "ISO 2768-mK" is the most common general note on drawings we receive from Europe and North America. Chinese national standard GB/T 1804 is technically equivalent to ISO 2768-1, so the tolerance values are the same.
Send the drawing and we will check the tolerance block
Tolerance decisions are where a part's cost is decided, and they are almost always made before anyone talks to a shop. If you want a second opinion on a drawing — which features are driving your price, where the general note is standing in for a functional requirement, which callouts you could loosen without any functional consequence — send it over.
You get a DFM review and a line-item quote within 24 hours. We will tell you where tightening to ISO 2768-f is costing you money for nothing, and where a feature that is currently covered only by the general tolerance needs its own callout. No minimum order quantity, and the review is free whether or not the job comes to us. Send your drawing or see our CNC machining services.