General tolerance: what ISO 2768 says and leaves out

What is a general tolerance?

A general tolerance is the tolerance that applies to any dimension without one of its own. It sits in or beside the title block, either as a plain value such as ±0.1 or as a reference to a standard and a class. Often that standard is ISO 2768-1 (opens in a new tab), which sets four classes for linear and angular dimensions, from fine to very coarse.

The class applies to the whole drawing. On a milled frame with forty untoleranced dimensions, that one letter decides how tight all forty have to be. So read the class before you work through the individual tolerances: it sits beside no dimension, yet it governs every free one.

How far can a dimension deviate in each ISO 2768 class?

The larger the dimension, the wider the permitted deviation. An 80 mm dimension falls in the range over 30 up to 120 mm, so it may deviate by ±0.3 mm in class m, ±0.15 mm in class f and ±0.8 mm in class c. Machined parts usually carry class m. Drawings that need more accuracy call for f, while c and v turn up mainly on fabricated and sheet metal work.

Values in the table are for linear dimensions from 0.5 mm upward. Where the table says ‘none’, the standard sets no value for that range in that class. Ask the customer which deviation applies.

Angular dimensions take their deviation from the length of the shorter leg. In class m that is ±1° up to 10 mm, ±0°30′ over 10 up to 50 mm and ±0°20′ over 50 up to 120 mm; class f uses the same angular values as m. Chamfer heights and external radii have their own, wider series: in f and m, ±0.2 mm from 0.5 up to 3 mm, ±0.5 mm over 3 up to 6 mm and ±1 mm above that.

What does the K in ISO 2768-mK mean?

In ISO 2768-mK the lower-case letter is the class from part 1, for linear and angular dimensions. The capital comes from part 2, which sets general geometrical tolerances in three classes, H, K and L, mainly for machined parts. It covers features without a feature control frame of their own, such as the flatness of a face or the squareness between two faces.

Class K allows 0.05 mm of flatness and straightness on a line or face up to 10 mm long, 0.1 mm over 10 up to 30 mm, 0.2 mm over 30 up to 100 mm and 0.4 mm over 100 up to 300 mm. Squareness in K is 0.4 mm as long as the shorter leg is no longer than 100 mm. Run-out has one value per class, whatever the size: 0.1 mm in H, 0.2 mm in K and 0.5 mm in L.

Part 2 was replaced in February 2021 by ISO 22081, the standard for general geometrical specifications and general size specifications, and NEN withdrew it on 1 March 2021. A drawing that cites mK therefore points to a withdrawn part for form and position. Part 1 was confirmed again in 2022 and remains current.

So check for a year after the reference. A reference with a year, such as ISO 2768-2:1989, pins the drawing to that edition, whatever has replaced it since. Without one, the edition currently in force applies, and a new edition or a withdrawal can change what the drawing asks for while the drawing itself stays the same. If it does not say which edition or agreement applies, ask the customer before you estimate.

Which requirements override the general tolerance?

Any requirement written against a dimension or feature itself. A dimensional tolerance such as 20 ±0.05 takes precedence, and so does a fit such as Ø12 H7; a fit takes its limits from ISO 286 and sits outside ISO 2768. A feature control frame with a geometric tolerance also takes precedence, and it says something the general class does not: where a feature sits relative to a datum.

Two kinds of dimension fall outside the general tolerance altogether: auxiliary dimensions in brackets and theoretically exact dimensions in a box. So leave them out of the free dimensions when you size the inspection load.

General roughness is another requirement again. Ra 3.2 beside the title block is about the surface, ISO 2768 about size, form and position. Keep them apart in the estimate: surface roughness decides the final pass and sometimes a finishing operation, the general class decides the inspection load on every free dimension.

Does a general ±0.1 decide whether you need 5 axes?

No. A general ±0.1 says how accurate every free dimension has to be, not which machine you need or how many axes. Whether a frame calls for 5-axis milling follows from its geometry and accessibility: can you reach every face and bore with standard tooling from the main directions, or are there angled faces and bores in between.

What does change the route is the requirements between features. Two bores with a tight position tolerance relative to each other usually belong in the same setup, and that can decide the machine. How that plays out is in position tolerance and route.

That is why Subduxion describes manufacturability as a relationship between part, requirements, process and factory, not a property of the geometry alone. The general tolerance is one of those requirements, and rarely the one that decides the route.

Where does the general tolerance sit in your cost?

Mostly in inspection. A fine class on a part with many untoleranced dimensions means tighter machining and more measuring, with an instrument that resolves well below the permitted deviation. A coarse class leaves room to cut faster and measure less.

A spreadsheet with a line for every toleranced dimension has no line for the title block. What the cost engineer knows about the class lives in their head, not in the sheet, so the inspection time on forty free dimensions in class f sits in no line at all. That time then comes out of your margin, or you cover it with a flat surcharge on every part and price a simple frame in class m too high.

Agree up front what you will measure. Under ISO 2768-1 a free dimension outside the general tolerance need not lead to rejection as long as the part still does its job, but settle that with the customer rather than rely on it. Dimensions that matter to function should carry a tolerance of their own.

Sometimes it also sits in the setup. A tight class for form and position can keep two faces in a single setup that you would otherwise machine in two. How setups add up in the cost is covered in counting setups.

In what order do you read a drawing's tolerances?

A fixed order stops you missing a requirement or counting it twice. Start with what applies to the whole part and work down to the requirements per feature.

1. Read the standard, class and edition in the title block, such as ISO 2768-mK, or the plain value, such as ±0.1.
2. Mark the dimensions with their own tolerance, the fits and the feature control frames. They override the general class.
3. Find the requirements between features, such as position, squareness and coaxiality. They decide the setup and the route.
4. Treat every value taken from the drawing as a proposal until someone has found it on the drawing and confirmed it.
5. If the general tolerance is missing, ask the customer which class applies, as with any other gap in a complete request. Choosing one yourself is a guess that comes back at final inspection.