ISO 2768-2: geometrical tolerances and what replaced it

What ISO 2768-2 was for

ISO 2768-2:1989 was the geometrical companion to ISO 2768-1. Part 1 gave default tolerances for linear and angular dimensions. Part 2 gave default tolerances for features whose geometry had no individual control. The aim was the same: one note in the title block instead of a frame on every surface.

The designation was written after the linear class, for example ISO 2768-mK. The lowercase letter set the size tolerance and the uppercase letter set the geometrical tolerance. A drawing could also use only the geometrical class, written as ISO 2768-K.

Part 2 applied mainly to features produced by removal of material. It was a machining standard at heart. Applying it to a casting, a moulding or a formed wire part stretches values that were never calibrated for those processes.

The three classes

Class H was the tightest, K was the middle class and L was the loosest. The values depended on the characteristic and on a nominal length. For straightness the length was the line being controlled. For flatness it was the longer side of the surface or the diameter of a circular face. For perpendicularity it was the shorter side of the angle.

The table below gives a representative extract. It is enough to see the pattern: H is roughly half of K, and K is roughly half of L at the smaller sizes. The spread between H and L grows as the part gets larger.

Two characteristics handled by rule

Not every control had its own table. Circularity was tied to the diameter tolerance: the circularity value equalled the size tolerance, but could not exceed the circular runout value for the class. Parallelism was tied to the size tolerance or to the flatness or straightness value, whichever was greater.

Those rules are easy to miss when a drawing is read quickly. A note that says ISO 2768-mK is not only invoking the tables. It is also invoking the clauses that derive circularity and parallelism from other tolerances.

What the standard never covered

General geometrical tolerances did not apply to every characteristic. Cylindricity, profile of any line, profile of any surface, angularity, coaxiality, position and total runout were outside the scope. Those features needed an individual control if they needed control at all.

The exclusion list is the practical limit of the standard. A shaft that must run true needs a runout or coaxiality callout. A sealing face needs flatness or profile. A hole pattern needs position with basic dimensions and datums. A title block class cannot supply any of those.

The standard also did not create a datum reference frame. Perpendicularity and symmetry need a datum, and the drawing still has to say which feature is the datum. A general tolerance can reduce drawing text, but it cannot remove the need to define the reference.

The status change that matters

ISO 2768-2:1989 is withdrawn. ISO 22081:2021 replaced it and was confirmed in 2026. The replacement is not a new set of H, K and L tables. It sets out how to write general geometrical specifications and general size specifications under the ISO GPS framework.

The practical consequence is that H, K and L should not be presented as a current accuracy class on a new drawing. A title block that says ISO 2768-mK is a legacy callout. It may still be contractually binding if the drawing and purchase order say so, but it is not the current way to specify general geometry.

ISO 2768-1:1989 remains published at the time of writing, although a replacement edition is in development. That is why drawings still use ISO 2768-m for linear dimensions while the geometrical half has moved on.

The old designation could also carry an E suffix, as in ISO 2768-mK-E. That invoked the envelope requirement: the surface of a feature of size could not cross the envelope of perfect form at maximum material size. ISO does not apply the envelope by default, so the suffix changed the inspection. If a legacy drawing carries the E, do not drop it when the drawing is reissued.

Reading a legacy drawing

Start by identifying which standard and which class the title block actually invokes. ISO 2768-m invokes part 1 only. ISO 2768-mK invokes both parts. ISO 2768-K invokes part 2 only, which is rare but valid on old drawings.

Then list the features that the general class covers and the features that need an individual control. Check that the drawing has datums for perpendicularity and symmetry. Check whether the part is machined. If it is moulded or formed, question whether the general geometrical values were ever appropriate.

Finally, confirm the revision and the contract. A withdrawn standard can still govern a legacy part if both sides agree. The risk is a new supplier reading the note as a current specification and applying it without the original assumptions.

• Identify the standard parts invoked by the title block.
• Separate features covered by the class from features outside it.
• Confirm the datum features and their order.
• Check that the process matches the scope of the standard.
• Record the interpretation in the inspection plan.

How to specify general geometry today

For a new drawing, the cleaner route is to use ISO 22081 for general geometrical and size specifications, or to apply individual ISO 1101 controls where the function needs them. ISO 22081 is built for the current GPS system and does not rely on a letter class to carry the intent.

In practice, many drawings still use a small set of individual controls: flatness on a sealing face, perpendicularity on a mounting face, position on a hole pattern, profile on a curved cover. That is more text than a title block note, but it is unambiguous and it survives a change of supplier.

If a customer insists on ISO 2768-mK for an existing part, keep the callout and add a note that names the withdrawn standard. Do not silently translate it into ISO 22081. The two are not numerically equivalent, and the translation needs a design decision, not a clerical one.

1. 01

   Identify the function

   Decide which surfaces locate, seal, rotate or carry load.

2. 02

   Choose individual controls

   Use flatness, perpendicularity, position or profile where the function needs a defined zone.

3. 03

   Set the datums

   Pick datum features that match the assembly and the fixture, then state the order.

4. 04

   Check the inspection

   Confirm that each control can be measured with the equipment and access available.

Inspection consequences

A general geometrical class is easy to write and hard to audit. The inspector has to know which features the class covers, which are excluded and which have individual controls. On a complex part, that is a reading exercise before any measurement starts.

For legacy parts, put the interpretation in the first article report. Record the datum alignment, the features checked against the general class and any feature that was referred to an individual control. If a feature sits outside the class, say so before the batch ships rather than after.

For new parts, the inspection plan should follow the individual controls. That is the point of writing them. A drawing with clear zones and datums produces a shorter argument at first article, even if the title block is less tidy.