ISO 2768 Tolerances Explained (and When to Use GD&T Instead)

Every mechanical drawing carries a title block, and most title blocks contain a line that decides the price of the part: "General tolerances: ISO 2768-m". It is one of the few specifications on a drawing that applies to every dimension nobody labeled, which means it is also the one most often copied from a template without being read.

This article explains how the ISO 2768 tolerance system actually works, how the four classes differ, where the standard stops being sufficient, and how to decide between general tolerances and GD&T without adding cost you do not need.

What ISO 2768 does

ISO 2768 exists so that a drawing does not need a tolerance printed next to every dimension. It defines default tolerances for linear and angular dimensions that carry no individual tolerance, based on the nominal size and a chosen class. The practical effect is that a 120 mm dimension and a 6 mm dimension can share the same title block and still receive appropriate tolerances.

The standard has two parts. Part 1 covers linear and angular dimensions. Part 2 covers geometric tolerances, which is where the K, H and L classes come from. A title block that reads "ISO 2768-mK" is calling up both: class m for dimensions, class K for geometry.

The four linear classes

The class is a statement about how much variation you are willing to accept, and the cost of the part rises as the class tightens. Linear tolerances for nominal size ranges, in millimetres:

Angular dimensions are treated separately, with the tolerance depending on the length of the shorter side of the angle:

Note that classes f and m share the same angular tolerances. That is not a typo in the standard; it reflects the practical limits of angular measurement and of the tooling that produces angles.

Which ISO 2768 tolerance class to choose

For most machined metal parts, class m is the right default. On a 30 to 120 mm dimension it allows ±0.3 mm, which is comfortably within the capability of a CNC machining center without any special attention, and it leaves the supplier free to plan the process around the dimensions you actually care about.

Class f is appropriate when the part interacts with others across many dimensions and you do not want to mark each one: instrument components, multi-part assemblies, parts that stack. It is achievable on a modern machine, but it removes the supplier's freedom to let non-critical features drift, which adds inspection time.

Class c and v are for welded structures, castings, flame-cut plate and other parts where the process itself is coarse. Specifying class c on a machined part is usually a sign that the drawing was copied from a fabrication drawing, and it can cause a different problem: the supplier may assume the part is rough work.

How over-tolerancing inflates price

A cost model of a machined part has three main lines: setup, machine time and inspection. General tolerances affect all three.

• A tight default tolerance can force an extra finishing pass, because the roughing cut no longer leaves enough margin to stay inside the band after stress relief or heat treatment.
• It can force additional inspection, because every unmarked dimension now needs to be verified rather than sampled.
• It can eliminate the cheapest process route. A part that could be sawn and milled may need grinding because the default flatness will not pass.

Where the cost really compounds is when a tight general tolerance meets a large part. A ±0.05 mm default on a 500 mm aluminum plate is a different proposition from the same tolerance on a 20 mm bracket, because thermal expansion over that length exceeds the tolerance band with a few degrees of shop temperature change. The part becomes inspectable only in a controlled room, and the price reflects it.

The habit worth adopting: keep the default tolerance realistic, and tolerate individual features explicitly where function demands it. A drawing with a medium default and four marked critical dimensions is cheaper to make and easier to inspect than a drawing with a fine default and no marked dimensions, even though the second one technically looks more precise.

Where ISO 2768 stops being enough

General tolerances control size and angle. They do not control the relationship between features, and that relationship is usually what determines whether an assembly works.

Three specific gaps:

1. Position of holes in a pattern. A hole pattern dimensioned with coordinate dimensions and a general tolerance accumulates error from datum to each hole. A position callout controls the pattern as a group.
2. Form and orientation. Straightness, flatness, perpendicularity and parallelism are not covered by Part 1. Part 2 provides classes, but they are crude instruments compared with a proper callout.
3. Functional fits across a stack. A mating pair can have every dimension in tolerance and still fail to assemble, because the tolerances were applied independently rather than to the datum that matters.

When to switch to GD&T

Move from general tolerances to geometric dimensioning and tolerancing when any of the following is true:

• The part must assemble with another part, and the fit has a functional consequence: a seal, a bearing, a locating pin, an optical axis.
• A feature must be located relative to a datum that is established by the function, not by the machining setup.
• You need to allow bonus tolerance: with position tolerance at maximum material condition, a hole that comes in large gains extra positional tolerance, which lets the supplier use the natural capability of the process instead of fighting it.
• The part is inspected on a CMM and you want the inspection to match the design intent.
• You are transferring the part between suppliers and need the requirement to be unambiguous.

For US drawings the reference is ASME Y14.5; for European drawings it may be ISO 1101 with ISO 2768-2 as a fallback. Mixing the two on one drawing is a reliable way to get a quote with a clarification request.

The four callouts buyers most often need

A drawing that uses these four well is usually shorter than the coordinate-dimensioned equivalent, and considerably cheaper to make.

What to check before you send an RFQ

1. Standard and revision stated in the title block: ISO 2768-m, ASME Y14.5-2018, or a customer standard.
2. Projection convention: first angle versus third angle. A European drawing read as third angle produces mirror-image parts.
3. Units, if the drawing is not consistent.
4. Default tolerance applied to unmarked dimensions, and whether it also applies to the 3D model.
5. Surface finish specified as Ra values with the surfaces identified.
6. Threads called out by standard, and whether they are formed or cut.
7. Critical dimensions marked, so the supplier knows what will be inspected.

Frequently asked questions

What does ISO 2768-m mean on a drawing? It means dimensions without an individual tolerance are held to class m of ISO 2768-1: for example ±0.2 mm on a dimension between 6 and 30 mm, and ±0.3 mm between 30 and 120 mm. It is the most common default for machined parts.

Is ISO 2768 the same as a general tolerance note like ±0.1 mm? No. A single ±0.1 mm note applies the same tolerance to every dimension regardless of size, which is unrealistic for large parts and unnecessarily loose for small ones. ISO 2768 scales the tolerance with nominal size.

Do I need GD&T for a simple bracket? Usually not. A bracket with a medium general tolerance and one or two marked hole positions is sufficient. GD&T earns its keep where features must relate to datums functionally or where assemblies stack.

Can a supplier hold ±0.01 mm everywhere? Physically possible on a small part with careful process control, economically unwise. Precision is applied to features, not to whole drawings. Marking a handful of critical dimensions and relaxing the rest is both cheaper and more likely to be delivered.

Next step

If a drawing is producing quotes that vary widely between suppliers, the cause is often an ambiguous default tolerance or a missing datum. Send the drawing and we will return it marked up with the features we would control, the tolerances we can hold without cost penalty, and where a callout is creating work that the function does not require.