General tolerances, ISO 2768
A dimension with no tolerance on the drawing is still toleranced. Enter its value and the class from the title block to find the limits it must fall within.
Your dimension
The most common class in general engineering.
Enter a dimension to see its limits
The values come from the ISO 2768-1 and 2768-2 tables, the very ones CoteCote applies to a drawing.
Full table, linear dimensions
Permissible deviations in millimetres, by nominal size.
| Range, in mm | f · fine | m · medium | c · coarse | v · very coarse |
|---|---|---|---|---|
| 0.5 to 3 | ± 0.05 | ± 0.1 | ± 0.2 | ± 0.5 |
| 3 to 6 | ± 0.05 | ± 0.1 | ± 0.3 | ± 1.0 |
| 6 to 30 | ± 0.1 | ± 0.2 | ± 0.5 | ± 1.5 |
| 30 to 120 | ± 0.15 | ± 0.3 | ± 0.8 | ± 2.5 |
| 120 to 400 | ± 0.2 | ± 0.5 | ± 1.2 | ± 4.0 |
| 400 to 1,000 | ± 0.3 | ± 0.8 | ± 2.0 | ± 6.0 |
| 1,000 to 2,000 | ± 0.5 | ± 1.2 | ± 3.0 | ± 8.0 |
| 2,000 to 4,000 | — | ± 2.0 | ± 4.0 | — |
Full table, angular dimensions
The permissible deviation depends on the length of the shorter side of the angle.
| Shorter side, in mm | f · fine | m · medium | c · coarse | v · very coarse |
|---|---|---|---|---|
| up to 10 | ± 1° | ± 1° | ± 1° 30′ | ± 1° 30′ |
| 10 to 50 | ± 30′ | ± 30′ | ± 1° | ± 1° |
| 50 to 120 | ± 20′ | ± 20′ | ± 30′ | ± 30′ |
| 120 to 400 | ± 10′ | ± 10′ | ± 15′ | ± 15′ |
| 400 to 10,000 | ± 5′ | ± 5′ | ± 10′ | ± 10′ |
What a general tolerance is for
A mechanical drawing carries dozens of dimensions. Tolerancing each one individually would clutter the drawing for nothing: most have no particular requirement, they simply need to be right. The general tolerance settles this with one line in the title block — every untoleranced dimension follows the class stated there.
It saves reading, not requirement. A dimension of 28.4 on a drawing marked ISO 2768-m must fall between 28.2 and 28.6. Outside that, the part is non-conforming, exactly as if the limits had been written beside it.
Reading the title block
The note takes two forms. On its own, ISO 2768-m sets only the dimensional tolerances. Doubled, ISO 2768-mK adds a class of geometrical tolerances, here K, which bounds straightness, flatness, parallelism and runout without a single feature control frame being drawn.
The four dimensional classes run from tightest to widest: f fine, m medium, c coarse and v very coarse. Class m is by far the most common in general engineering. Class v is only used on as-cast or flame-cut parts.
What a general tolerance doesn't do
It never applies to a dimension that's already toleranced. As soon as a size carries its deviations, a fit such as H7, or a geometrical feature control frame, that indication prevails. This is the most common inspection mistake: applying the general class to a dimension that has its own, and passing a part that should have failed.
It doesn't go below 0.5 mm. Under that, the standard is silent and the dimension must carry an explicit tolerance. Above 4 000 mm, the same. This calculator returns nothing in those cases rather than extrapolating a value that doesn't exist.
It is no substitute for a tolerance stack-up. Across several stacked dimensions the deviations add up: five dimensions at ± 0.2 in 2768-m can produce a cumulative error well beyond what the function allows. Checking that is the design office's job, not the general class's.
One example, carried to a verdict
Drawing marked ISO 2768-m. A dimension of 65.98 with no tolerance. It falls in the 30 to 120 range, where class m allows ± 0.3. The limits are therefore 65.68 and 66.28. A reading of 65.95 passes, a reading of 66.35 doesn't, and the difference is written nowhere on the drawing: it follows from the title block.
Frequently asked questions
- What does ISO 2768-mK on a drawing mean?
- The first letter is the class for dimensional tolerances, here m for medium. The second is the class for geometrical tolerances, here K. A drawing may carry only the first.
- Does the general tolerance apply to every dimension?
- No. It only covers dimensions that carry no tolerance of their own. As soon as a dimension is written with its deviations, or with a fit such as H7, that indication prevails.
- What happens below 0.5 mm?
- The standard defines no general tolerance below 0.5 mm. Those dimensions must carry an explicit tolerance on the drawing.
- What is the difference between ISO 2768-1 and ISO 2768-2?
- Part 1 covers dimensional tolerances, linear and angular. Part 2 covers geometrical tolerances, with classes H, K and L.
This calculation, on every dimension of a drawing, in one pass
CoteCote reads the note in the title block, applies the class to every dimension that has none of its own, and hands you an inspection table ready to fill in.