General Tolerances and Drawing Notes
ISO 2768 classes, title-block tolerances, how to write the note, and what it does and does not cover.
Most dimensions on a drawing do not need an individual tolerance. A bracket’s overall length, a bend position, the diameter of a clearance hole: if the function does not care within a few tenths of a millimeter, one note in the title block can cover them all. This page explains how general tolerances work, gives the ISO 2768-1 tables, and shows how to write the note. It is part of the Fits & Tolerances guide.
What general tolerances do
A general tolerance applies to every dimension that has no tolerance of its own. It saves effort on the drawing and, more importantly, it makes sure nothing is left without a limit, so no feature is ever “unspecified”. The idea is simple: the drawing states the tolerances that matter, and the general tolerance gives a reasonable default to the rest, set to what the shop can hold without special effort.
- Individual tolerances always win. A tolerance written on a dimension replaces the general tolerance for that dimension.
- It is not free. A general tolerance is still a requirement; parts outside it are non-conforming. Choose it so the normal process meets it without extra inspection effort.
- It does not replace fits. Mating features (bearing seats, pins and holes, shafts) need individual tolerances or a fit designation: see How Fits Work.
ISO 2768-1: linear sizes
ISO 2768-1 defines four tolerance classes: f (fine), m (medium), c (coarse) and v (very coarse). The table gives the permitted deviation, ± in millimeters, by the nominal size range.
| Nominal size (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 up to 3 | ± 0.05 | ± 0.1 | ± 0.2 | – |
| over 3 up to 6 | ± 0.05 | ± 0.1 | ± 0.3 | ± 0.5 |
| over 6 up to 30 | ± 0.1 | ± 0.2 | ± 0.5 | ± 1.0 |
| over 30 up to 120 | ± 0.15 | ± 0.3 | ± 0.8 | ± 1.5 |
| over 120 up to 400 | ± 0.2 | ± 0.5 | ± 1.2 | ± 2.5 |
| over 400 up to 1000 | ± 0.3 | ± 0.8 | ± 2.0 | ± 4.0 |
| over 1000 up to 2000 | ± 0.5 | ± 1.2 | ± 3.0 | ± 6.0 |
| over 2000 up to 4000 | – | ± 2.0 | ± 4.0 | ± 8.0 |
The size ranges, and the ± signs, are the same for external sizes, internal sizes, step sizes, diameters, radii, distances, and the sizes of chamfers and radii (which have their own table below). Sizes below 0.5 mm are not covered by the table and must be given individually.
Radii, chamfers and angles
| External radius and chamfer height (mm) | f and m | c and v |
|---|---|---|
| 0.5 up to 3 | ± 0.2 | ± 0.4 |
| over 3 up to 6 | ± 0.5 | ± 1 |
| over 6 | ± 1 | ± 2 |
| Angles: length of the shorter leg (mm) | f | m | c | v |
|---|---|---|---|---|
| up to 10 | ± 1° | ± 1° | ± 1°30′ | ± 3° |
| over 10 up to 50 | ± 0°30′ | ± 0°30′ | ± 1° | ± 2° |
| over 50 up to 120 | ± 0°20′ | ± 0°20′ | ± 0°30′ | ± 1° |
| over 120 up to 400 | ± 0°10′ | ± 0°10′ | ± 0°15′ | ± 0°30′ |
| over 400 | ± 0°5′ | ± 0°5′ | ± 0°10′ | ± 0°20′ |
The angular tolerance depends on the length of the shorter leg of the angle, because a given angle error shifts a short leg’s end by less. The table is a tolerance on the angle itself, not on the linear dimension of the part.
Writing the note
Put the standard and the class in or near the title block: ISO 2768-m (general tolerances in accordance with ISO 2768, class m for linear and angular dimensions). The wording can also be “Tolerances for dimensions without individual tolerance indications: ISO 2768-m”.
- The old Part 2 is gone. ISO 2768-2 (general geometrical tolerances, classes H, K and L, written as “ISO 2768-mK”) has been withdrawn and replaced by ISO 22081:2021, which covers general geometrical and size specifications with a different method. A drawing that still says “ISO 2768-mK” follows the old convention; for new drawings, check ISO 22081 and name it explicitly.
- Part 1 is still current, but a new edition of ISO 2768 is reported to be in preparation. Always write the standard’s number and, if the drawing is controlled, its year.
- With ASME drawings, general tolerances are given as a note or in the title block (next section); they are not an ISO class. ASME Y14.5-2018 requires every dimension and feature to have a tolerance, by individual indication or by a general note.
US title-block tolerances
US drawings usually set the general tolerance by the number of decimal places in the dimension, in a title-block table. The values below are typical practice, not a standard; every company sets its own, and the numbers must be stated on the drawing.
| Dimension written as | Typical general tolerance | Meaning |
|---|---|---|
| 2.5 (one place) | ± 0.1 in | Rough features |
| 2.50 (two places) | ± 0.01 in | Ordinary machined features |
| 2.500 (three places) | ± 0.005 in | Precision machined features |
| 2.5000 (four places) | ± 0.0005 in | Tight tolerance; usually better to state it individually |
| Angles | ± 0.5° to ± 1° | Depends on the part and process |
The weakness of the method is that the decimals of a dimension then decide its tolerance, so adding a trailing zero for neatness quietly tightens a requirement. Many designers prefer to write the tolerance of anything that matters, and keep the decimals for appearance.
Choosing a class
| Class | Typical for | Typical process |
|---|---|---|
| f (fine) | Precision parts, mating features that are not given individual tolerances | Precision machining, grinding |
| m (medium) | The usual default for machined parts | General machining (CNC milling and turning) |
| c (coarse) | Fabrications, sheet metal, castings with machining allowance | Sheet metal, welding, rough machining |
| v (very coarse) | Large, rough or non-critical dimensions | Flame cutting, heavy fabrication |
ISO 2768-1 leaves the choice to the usual accuracy of the workshop. The matching process capabilities are on the Tolerances by Process and Surface Finish page. If one process makes the part and a different one finishes it (a cast part with machined faces), give the machined features their own tolerances.
What they do not cover
- Theoretically exact (basic) dimensions in a feature control frame, and reference dimensions in brackets: they have no tolerance of their own.
- Geometric tolerances of features that carry an individual feature control frame. The general geometric class (old ISO 2768-2, now ISO 22081) is a separate matter; see the GD&T guide for the individual controls.
- Fits. Do not leave a bearing seat or pin to a general tolerance. A class m tolerance on a 25 mm size is ± 0.2 mm, a band 0.4 mm wide; an H7 hole of the same size is 0.021 mm wide, nearly twenty times tighter.
- Special processes with their own standards: castings (ISO 8062-3), plastic moldings (ISO 20457), welded structures (ISO 13920) and so on, which have their own general tolerances. Invoke those standards directly.
- Sizes below 0.5 mm, which ISO 2768-1 leaves to individual indication.
Worked examples
Example 1: reading the table
| Dimension | f | m | c | v |
|---|---|---|---|---|
| 4.5 mm | ± 0.05 | ± 0.1 | ± 0.3 | ± 0.5 |
| 12 mm | ± 0.1 | ± 0.2 | ± 0.5 | ± 1.0 |
| 45 mm | ± 0.15 | ± 0.3 | ± 0.8 | ± 1.5 |
| 150 mm | ± 0.2 | ± 0.5 | ± 1.2 | ± 2.5 |
| 650 mm | ± 0.3 | ± 0.8 | ± 2 | ± 4.0 |
A 45 mm dimension under class m may be anything from 44.7 to 45.3 mm: a band of 0.6 mm. Under class f, 44.85 to 45.15.
Example 2: when a general tolerance is not enough
A 25 mm shaft must turn freely in a 25 mm hole, with 0.007 to 0.041 mm of clearance. Class m allows ± 0.2 mm on each part; the worst-case clearance would be ± 0.4 mm either way. Neither part can rely on the general tolerance. Give them individual tolerances or an ISO fit (H7/g6); see Fits – Metric (ISO System).
Example 3: an angle tolerance in millimeters
A bent bracket has a 90° bend with a 30 mm shorter leg and a 100 mm longer leg, general tolerance class m. The angle tolerance is ± 0°30′ = ± 0.5°.
- At the end of the 100 mm leg, ± 0.5° moves the end by 100 × tan 0.5° = ± 0.87 mm.
- If the part has to fit within ± 0.3 mm at that point, class m is not good enough: give the angle an individual tolerance, or dimension the end position directly.
Example 4: general tolerances add up
Five 45 mm dimensions, each class m (± 0.3), are stacked in a chain.
- Worst case: 5 × 0.3 = ± 1.50 mm.
- RSS: √5 × 0.3 = ± 0.67 mm.
- This is why a general tolerance is for features that do not matter. If five features have to line up, they need individual tolerances: see Tolerance Stack-up Analysis.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Parts pass inspection but do not assemble | A mating feature was left to the general tolerance | Give it an individual tolerance or a fit |
| Supplier measures tighter than the drawing intends | Extra decimals imply a tighter tolerance in a decimal-place title block | State the tolerance, or remove the trailing zeros |
| Drawing says “ISO 2768-mK” and the new CAD template does not | Part 2 was withdrawn and replaced by ISO 22081 | Name the standard that applies to geometric tolerances explicitly |
| Bend angles drift | Class m allows ± 0.5° on short legs; springback moves it | Tolerance the angle individually, or the end position |
| Cast and machined features have the same tolerance | One general class for different processes | Cast features to ISO 8062-3, machined features to their own |
Related
- Fits & Tolerances: the overview and quick reference.
- Dimensional Tolerancing Basics: how tolerances are written.
- Tolerances by Process and Surface Finish: what each process can hold.
- Tolerance Stack-up Analysis: adding tolerances up.
- Datums and Datum Reference Frames: the GD&T side of drawing control.
FAQ
What does “ISO 2768-m” mean?
That dimensions with no individual tolerance are held to the medium class of ISO 2768-1: for example ± 0.3 mm for sizes over 30 up to 120 mm.
Is ISO 2768 the same as ISO 2768-mK?
No. The “mK” form combines Part 1 (class m, for sizes) and Part 2 (class K, for geometry). Part 2 has been withdrawn and replaced by ISO 22081:2021.
Which class should I pick?
Pick the class that the normal process meets without extra checking. For general machining, m is usual; for sheet metal and fabrications, c. Do not choose a finer class than you need.
Do general tolerances apply to angles?
Yes, ISO 2768-1 has a table for angles, based on the length of the shorter leg. US title blocks usually give a single angle tolerance such as ± 0.5° or ± 1°.
Can I use ISO 2768 on an ASME drawing?
You can, but ASME Y14.5 drawings normally give general tolerances in a title-block note, and the two systems define size and form differently (Rule #1 against independency). Do not mix them in one drawing without saying which governs.
Why not tolerance everything individually?
Because it clutters the drawing and slows everyone down. Individual tolerances are for features that need them; the general tolerance covers the rest.
References
- ISO 2768-1:1989, General tolerances: tolerances for linear and angular dimensions without individual tolerance indications.
- ISO 22081:2021, Geometrical product specifications (GPS): general geometrical specifications and general size specifications (replaced ISO 2768-2:1989).
- ASME Y14.5-2018, Dimensioning and Tolerancing.
- ISO 8062-3 (castings), ISO 20457 (plastic molded parts) and ISO 13920 (welded structures) for the process-specific general tolerances.
- Machinery’s Handbook, 31st edition, Industrial Press: tolerance definitions in “Allowances and Tolerances for Fits”.
Last reviewed: October 2026. ISO 2768 is under revision; check the current edition before relying on the tables.