ISO 2768 is the first thing a machinist looks for in the title block, and often the last thing a designer thinks about. Used properly, it says what you mean without a hundred individual tolerances. Used carelessly, it either buys precision the part does not need or starts an argument about a component that was made exactly to the drawing.
What the standard actually covers
ISO 2768-1 covers linear and angular dimensions that carry no individual tolerance. ISO 2768-2 covers geometric tolerances: straightness, flatness, perpendicularity, symmetry and runout. Together they define four classes — f (fine), m (medium), c (coarse) and v (very coarse). Machined prototypes almost always sit at m. Class f appears where fits, gaps and visible part lines matter.
The linear values behind the class letter
| Nominal range | f | m |
|---|---|---|
| 0.5 – 3 | ±0.05 | ±0.10 |
| 3 – 6 | ±0.05 | ±0.10 |
| 6 – 30 | ±0.10 | ±0.20 |
| 30 – 120 | ±0.15 | ±0.30 |
| 120 – 400 | ±0.20 | ±0.50 |
| 400 – 1000 | ±0.30 | ±0.80 |
Two consequences follow. First, the allowance scales with size: a 200 mm dimension at class m may move ±0.5 mm, which is more than most designers assume. Second, the gap between f and m is roughly a factor of two, so switching the whole drawing to f doubles the measurement effort on features that may not matter at all.
How to call out the exceptions
Put the general class in the title block, then tolerance only the features that drive function. A bearing bore, a mating face and a cosmetic gap deserve their own callout; the position of a cable clip usually does not.
- State the class once, in the title block, and stop repeating it on individual dimensions.
- Tolerance fits, sealing faces and assembly datums individually, with the fit designation rather than a symmetric number.
- Add a datum scheme before adding tight tolerances — without datums, a ±0.02 mm callout is not measurable.
- If two features must move together, tolerance the relationship (position, profile) rather than each dimension separately.
Where prototype drawings usually go wrong
- Tolerancing the CAD model rather than the function. A ±0.02 mm note on a non-critical pocket adds cost and inspection time for nothing.
- Mixing standards on one sheet — an ISO title block with ASME position symbols and no datum reference.
- Leaving the title block blank and letting the shop assume general tolerance. It will, and it may assume coarse.
- Calling a tight tolerance without saying how it will be measured. If the method is not defined, the reading is negotiable.
A practical default for a machined prototype is 2768-m in the title block, 2768-f on the assembly interfaces, and a named ±0.02 mm on two or three critical features — with the datum scheme drawn. That combination is cheap to inspect, honest about what matters, and easy for a shop to quote without a clarification email.