ISO 2768 general tolerances explained, with a practical class table

What ISO 2768 actually does

ISO 2768 is a general tolerance standard. It allows a drawing to state one tolerance class in the title block instead of writing a tolerance on every dimension. Dimensions without an individual tolerance are then covered by that class.

The standard has two parts. Part 1 covers linear and angular dimensions. Part 2 covers geometrical tolerances for features without individual geometrical callouts. They are often used together, but they are separate callouts.

The important limit: ISO 2768 is a default, not a substitute for engineering judgement. A dimension that controls a fit, a contact gap, a sealing surface or a safety function still needs its own tolerance.

The four linear classes

ISO 2768-1 defines four linear classes: f (fine), m (medium), c (coarse) and v (very coarse). The table below shows the tolerance for a nominal dimension in each range. The values are in millimetres.

How to choose a class

Class m is the usual default for machined, stamped and formed parts in general engineering. It gives a practical tolerance for a process that is already capable, without turning the drawing into a list of special callouts.

Choose f when the part has several features that must locate together and the process can hold the tolerance without a special route. Be ready for a higher inspection cost. Choose c or v for non-critical fabrication, brackets, covers and features that are cut or formed without a precision operation. Do not use a loose class to hide a process that cannot hold the part.

How to put it on the drawing

Put the class in or near the title block, in a form that names the standard and the part. A common callout is: general tolerances ISO 2768-m. If part 2 is also being used, state the geometrical class as well, for example ISO 2768-mK.

The callout must be visible and unambiguous. If the drawing has a mix of standards, or a note that says all dimensions are in millimetres, keep the general tolerance note close to the units and the revision.

What the standard does not cover

ISO 2768 does not cover every feature. It does not replace a fit callout, a surface finish callout, a geometrical control for a critical surface or a tolerance for a feature that is not a linear or angular dimension. It also does not tell the supplier which process to use.

If a feature is critical to assembly, put a direct tolerance and a datum framework on it. If a surface must be flat for a seal, use a flatness callout even if the general geometrical class would allow more. The general standard is there to reduce drawing noise, not to remove engineering decisions.

Inspection and cost

A general tolerance still has to be inspected. The difference is that the inspector can prioritise. Start with the features that locate the part and the features that carry the function. Then sample the rest.

Tightening every dimension to class f does not improve a part. It increases the number of measurements, the chance of a false rejection and the cost of the inspection pack. Use the class that matches the process, then mark the critical-to-quality dimensions separately.

• State the class in the title block and keep the revision visible.
• Mark critical dimensions with a direct tolerance and a datum.
• Use ISO 2768-2 for geometrical defaults, not part 1.
• Check that the process can hold the class before the drawing is released.
• Agree the inspection level with the supplier at RFQ stage.

Angular dimensions and the shorter side rule

Part 1 also covers angular dimensions, but the tolerance class is read against the shorter side of the angle, not the nominal angle itself. The standard tabulates the allowance by the length of that shorter side, because the side length controls how far the far end of the feature can move.

This matters on formed and machined parts where an angle sets a face. A bend callout of 90 degrees under the general angular tolerance may be acceptable for a routing feature and too loose for a joint face. In that case, give the angle its own tolerance in degrees, or control the face with a profile or angularity callout and a datum.

Chamfers and radii have their own small table under the standard, separate from the linear table. Do not assume the linear class value applies to a small chamfer. If the chamfer is functional, such as an entry lead on a bore, call it out directly.

Angles written in degrees and minutes are easy to misread. State the unit on the drawing and keep the format consistent. A tolerance written as 30 minutes is clear to a trained reader and ambiguous to everyone else, so avoid the shorthand unless the drawing standard requires it.

Legacy drawings and mixed standards

Many drawings in circulation were made under an older national adoption of the same standard. A title block may cite BS EN ISO 2768, DIN ISO 2768 or ISO 2768, and the class table is generally the same. The market status of each edition is not, so check the standard named on the drawing against the contract rather than silently substituting a newer one.

A drawing can also cite two systems at once. A title block may say ISO 2768-m while a note requires ASME Y14.5 for geometrical controls. That is not necessarily a conflict, but the drawing should say which document takes precedence when the two give different answers.

Newer drawings may use ISO 22081 for general geometrical specifications instead of ISO 2768-2. The two are not identical in method, so a supplier who assumes part 2 because that is what the last drawing said can misread the requirement. Confirm the intent with the designer before release.

When a drawing is revised, carry the general tolerance note forward deliberately. A class that was right for a machined prototype may be wrong for a stamped production part, and a note copied from the old revision can outlive the process it was written for.