ISO 2768-m Explained: The Tolerance Chart on Your Drawing

What the note actually says

ISO 2768 is a standard for general tolerances — a set of default tolerance bands that apply automatically to any dimension on a drawing that does not carry its own tolerance.

The purpose is practical. A fully toleranced drawing is unreadable: every dimension carrying a plus and a minus, most of them saying the same thing. The general note replaces all of that with a single line in the title block, and the drawing only calls out tolerances where the dimension needs something different from the default.

It works in two parts:

• ISO 2768-1 covers linear and angular dimensions, with four classes: f, m, c and v
• ISO 2768-2 covers geometric tolerances — straightness, flatness, perpendicularity, symmetry — with three classes: H, K and L

A drawing may invoke either or both, and when it invokes them it usually says so as ISO 2768-mK, meaning the medium linear class and the K geometric class.

The linear tolerance table

This is the table the note refers to for ISO 2768-1. All values are in millimetres, and they are the permitted deviation for a dimension falling in that size range.

Basic size range	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 things are worth reading off that table.

The band widens with size. A 2 mm feature under class m is allowed ±0.1 mm; a 500 mm feature under the same class is allowed ±0.8 mm. This is not an arbitrary relaxation — it reflects that the errors which cause variation, from thermal expansion to machine geometry to tool deflection, all scale with the dimension being produced.

The classes are a factor apart, not a step. Moving from m to c roughly doubles or triples the band; moving from m to f roughly halves it. The choice of class sets the accuracy of the whole drawing at once, which is why it is a design decision rather than a note.

What medium means in practice

The m class is the usual default, and the reason is worth stating plainly: it describes what an ordinary machine shop achieves without special effort.

Under ISO 2768-m, a dimension between 6 and 30 mm is allowed ±0.2 mm. That is not a demanding tolerance on a milled or turned part — it is what the process produces as a matter of course, with normal tooling, normal feeds and a normal setup. Nothing has to be done differently to hold it. The same applies whether the part is produced on a CNC milling machine or a CNC turning lathe.

That is why the general tolerance block costs nothing. It is not a requirement imposed on the shop; it is a description of the default outcome.

It also explains why the tight tolerances on a drawing are the ones that drive the price. Everything inside the general block is free. Everything outside it — the features carrying their own ±0.05 or ±0.01 — is where the extra passes, the tool-wear management and the measurement come in, which is the subject of the comparison on how tolerances drive cost.

Where the m class is not enough

The m class is a general default, and general defaults do not fit everything. Where a dimension has to do a job, it needs its own tolerance.

The features that always need one:

• Bearing seats and bores — a bearing needs a defined fit, and a general band will not provide it
• Spigots, mating diameters and location features — where two parts have to locate on each other
• Sealing faces and groove dimensions — where a seal has to work
• Gear and spline features where the mesh depends on the accuracy
• Threads with a defined class where the fit of the fastener matters
• Any dimension that has to relate to another feature, which the general note does not control at all

For everything else — overall sizes, clearance holes, non-mating surfaces, internal cavities, the outside of a part that simply has to be roughly the size shown — the general block is doing exactly what it was designed for.

What the general note does not cover

This is the part that causes the most trouble, because the note reads as though it covers everything and it does not.

Threads and other standardised features. A thread is governed by its own designation. A callout of M8 carries the tolerance of that thread class; the general block does not apply to it, and it cannot be used to tolerate a thread into existence. The same applies to any feature whose dimensions come from another standard.

Dimensions marked as reference. A reference dimension is shown for information only — typically a derived or duplicated value — and is not inspected. A general tolerance does not turn a reference dimension into a controlled one.

Radii and chamfers. These have their own table in ISO 2768-1, separate from the linear dimensions, and the deviation permitted depends on the nominal radius or chamfer size. They are not covered by the linear bands above.

The geometric relationships between features. Flatness, straightness, perpendicularity, concentricity, position and symmetry are not controlled by ISO 2768-1 at all. Part 2 covers some of them, but only when it is invoked and only for the features it addresses. A drawing with a general linear tolerance and no geometric callouts does not control whether a face is flat or whether a bore is perpendicular to it.

Surface finish. Not covered at all. Ra values, if they matter, are specified separately.

The consequence is worth stating in one line: a drawing that says ISO 2768-m and nothing else has controlled the sizes of the features and almost nothing about their relationships. Where a part has to assemble, the relationships are usually what matters more.

Angular tolerances, radii and chamfers

Angular dimensions have their own table under the same classes, and the permitted deviation depends on the nominal length of the shorter side of the angle. It follows the same pattern as the linear table: shorter reference lengths get tighter bands, longer ones get wider ones.

Radii and chamfers likewise have a table of their own, keyed to the nominal size. The values are small in absolute terms because the features themselves are small — a radius of a few millimetres is not permitted to deviate by a millimetre.

The practical point is simply that these are separate tables under the same note. A drawing that invokes ISO 2768-m has invoked all of them, and that is usually what a designer intends.

The geometric half: ISO 2768-2

Part 2 of the standard handles geometric tolerances at a general level, with three classes:

Class	Meaning
H	Closest of the three
K	Middle
L	Coarsest

It covers straightness and flatness of surfaces, perpendicularity of surfaces, and symmetry of features. Where the drawing does not carry an individual geometric callout for a feature, the class invoked applies.

Invoked together with the linear class, the note reads ISO 2768-mK. That combination — medium linear tolerances and the middle geometric class — is a sane default for most machined parts, and it is worth knowing that the two letters are doing different jobs rather than being alternatives.

What part 2 does not do is control everything geometric. Position, concentricity and runout are not addressed by the general classes, so a part whose function depends on them needs individual callouts.

What a shop does with the note

Knowing what happens to the note on the shop floor explains why it is the cheapest line on the drawing.

The class is read as the working tolerance for anything not called out. A machined part under ISO 2768-m is planned so that the general dimensions land inside the band without any special effort: normal tooling, normal feeds, a normal setup, and the dimensions come out within the permitted deviation as a consequence of the process rather than as a target being chased.

What changes the picture is anything outside the class. The moment a feature carries its own tolerance, the operation stops being routine:

• A tighter tolerance on a diameter means finishing passes at reduced feed, and often a different tool for the final cut
• A tighter tolerance on a bore means boring or reaming rather than interpolating
• A geometric callout means the setup has to control the relationship, not just the size — which usually means planning which features are cut in the same setup
• A tight tolerance far from the datum means the sequence has to be arranged so that the error does not accumulate

That is why the general note and the individual tolerances are not two ways of saying the same thing. The general note describes a process; the individual tolerance changes it. A drawing with four tight tolerances is not “an ISO 2768-m drawing with a few extras” — it is a part that needs a different plan from the one the general note implies.

There is a corollary worth carrying into a design review. Where a part is quoted higher than expected and the geometry looks ordinary, the reason is usually a small number of callouts rather than anything about the shape. Checking whether each of them is doing a job is the fastest route to a cheaper part, and it acts on every piece in the batch rather than once.

ISO 2768 and the rest of the drawing

The general note is one line among several, and it interacts with the others. Three combinations come up most often.

General note plus a thread callout. The thread is controlled by its designation, not by the general class. The two coexist, and the thread is the one that has to be written properly — a designation missing its fit class is a thread that has not been specified.

General note plus a geometric class. ISO 2768-mK invokes both halves. The linear bands cover the sizes, and the K class covers straightness, flatness, perpendicularity and symmetry at a general level. It is a compact way of making a drawing mean something about geometry rather than nothing.

General note plus individual callouts. The individual callout always wins for the feature it applies to. The general note fills in everything else, which is exactly how the standard is designed to work — a small number of specific requirements and a default for the rest.

The failure mode is a drawing where the general note is present but the specific requirements are missing. That is the drawing described earlier: the sizes are controlled and almost nothing about how the features relate. Where a part has to assemble reliably, those relationships are usually the part that matters, and they need to be written down.

Five mistakes that come up often

1. Naming the standard without naming the class. ISO 2768 alone is incomplete. The class is what sets the tolerance, so a drawing without one asks a question rather than making a statement.

2. Assuming the note covers the threads. It does not. Threads are controlled by their own designation, and a drawing that leaves a thread to the general block has left the thread uncontrolled. Thread callouts and designations are set out on the thread standards page.

3. Assuming the note covers geometry. A general linear tolerance does not make a face flat or a bore perpendicular. Where those matter, they need callouts — or part 2 invoked.

4. Combining a general note with tight tolerances on non-functional features. The note is there to keep the drawing readable and the part economical. Carrying a set of tight tolerances on features that do not fit, seal, locate or align defeats both purposes, and each one is a per-part cost.

5. Applying a class that does not match the part. Class f on a large, rough part imposes accuracy nobody needs and the process cannot deliver economically. Class c on a small precision part produces a drawing that does not control the dimensions that matter. The class should follow the part, and m is the right answer far more often than not.

Why m is the sensible default, and when to move off it

The argument for m is not that it is the best tolerance. It is that it is the tolerance that costs nothing, because it matches what ordinary practice achieves. Everything within it comes for free; everything outside it has to be paid for.

Moving to f makes sense where most of the part genuinely needs closer control — a small precision component where most dimensions are functional. Moving to c or v makes sense where the part is large and rough, and where imposing a tighter class would mean measuring and reworking dimensions that do not matter.

What rarely makes sense is specifying a class and then contradicting it. A drawing marked ISO 2768-c covered in ±0.05 callouts is not a coarse part with a few tight features; it is a tight part written the long way, and it will be quoted and made as one.

What to write on the drawing

Instead of	Write
ISO 2768	ISO 2768-m — always name the class
ISO 2768-m with no geometry	ISO 2768-mK where flatness, straightness or perpendicularity matter
Thread left to the general block	The full thread designation, with its class
Radii left to the linear table	Radii and chamfers stated, or accepted as the general note handles them
Tight tolerance on everything	General block, plus tolerances only on the fits and locations
A part that must assemble	Individual callouts for the relationships, since the general note does not control them

The most useful habit is to write the general note and state the small number of features that have to do a job. The note handles everything else, which is what it exists for, and precision features are held to ±0.01 mm with ISO 2768-m as the general block — see tolerances we hold for what the machine actually delivers.

Send the drawing with the general note and the functional features identified, and the quote comes back within 24 hours with DFM feedback, including a note where a feature carries a tolerance the function does not need. The drawing conventions we can read are on the drawing requirements page. Orders start at 50 pieces per style and material, samples from a single piece in 5–10 days, and every batch ships with a material certificate (MTR) tracing the grade to its mill heat plus pre-shipment photos.