ISO 2768-mK is on every second drawing. Usually the wrong one
What a general tolerance actually settles
Every dimension on a drawing needs a tolerance. For those that do not get one of their own, the entry in the title block applies. That is not sloppiness but a deliberate agreement: it defines when a part may be rejected, and with it how much inspection effort the supplier has to spend.
The usual entry reads ISO 2768-mK. The lower-case letter covers linear and angular dimensions from part 1, the capital letter form and position from part 2. Four characters that are binding for most of the dimensioning, and that are still often copied from the last drawing without a second look.
| Nominal size range | ISO 2768-f (fine) | ISO 2768-m (medium) |
|---|---|---|
| 0.5 … 6 mm | ± 0.05 mm | ± 0.1 mm |
| 6 … 30 mm | ± 0.1 mm | ± 0.2 mm |
| 30 … 120 mm | ± 0.15 mm | ± 0.3 mm |
| 120 … 400 mm | ± 0.2 mm | ± 0.5 mm |
| 400 … 1000 mm | ± 0.3 mm | ± 0.8 mm |
| 1000 … 2000 mm | ± 0.5 mm | ± 1.2 mm |
There are also classes c (coarse) and v (very coarse), rare in machine building and better suited to welded and flame-cut parts.
Going from m to f halves the tolerance. On a milled part that is usually free, because modern machines work more accurately anyway. On a weldment or a casting it is a statement that means rework.
The classic: the wrong standard for the process
ISO 2768 was written for machined parts. Put it on an injection moulding, a die casting or a printed part and you are asking for something the process cannot deliver. The supplier notices at the quotation stage if you are lucky, and at first article inspection if you are not.
The same 100 mm dimension, four processes:
| Process and standard | Tolerance at 100 mm |
|---|---|
| Milling, ISO 2768-f | ± 0.15 mm |
| Milling, ISO 2768-m | ± 0.3 mm |
| Injection moulding, ISO 20457 TG4 | ± 0.4 mm |
| Injection moulding, ISO 20457 TG6 | ± 0.9 mm |
| FDM printing, industrial | ± 0.2 mm |
| FDM printing, desktop | ± 0.5 mm |
Values from the general tolerance assistant. The 3D printing figures follow published process limits of common service providers, not a standard.
The ISO 20457 TG6 row is worth noting: almost three times the machined tolerance, and not out of negligence but because shrinkage, mould temperature and holding pressure move the part by that much.
ISO 20457: the distinction you have to know
Plastic mouldings fall under ISO 20457. It does not just assign tolerance groups TG1 to TG7, it also distinguishes two kinds of dimension.
- Tool-related dimensions (W) are formed entirely within one half of the mould. They are more accurate, because only shrinkage comes between design and part.
- Non-tool-related dimensions (NW) cross the parting line or involve moving mould elements. On top of shrinkage they carry the positional accuracy of the mould halves and the deflection under clamping force.
The difference is substantial: at 100 mm in tolerance group TG4 it is ± 0.25 mm for a tool-related dimension against ± 0.40 mm for a non-tool-related one. It is still routinely overlooked in design. If you need a tight dimension, place it on the part so that it lies within one half of the mould. That is a design decision, not a tolerancing decision, and it is made long before anyone dimensions the drawing.
Castings follow ISO 8062 with its casting tolerance grades, stampings and bent parts DIN 6930. Those have their own quirks too: with bent parts the achievable accuracy hangs on springback, and springback is a function of material batch and sheet thickness.
General tolerances add up
The most expensive mistake with general tolerances is not the wrong class but the forgotten chain. A part with four steps, all toleranced to ISO 2768-m at ± 0.2 mm each, carries ± 0.8 mm across its length in the worst case. If the mating part brings the same, you are past a millimetre without a single unusual tolerance anywhere.
The way out is rarely a finer general tolerance. Usually it is enough to dimension the critical chain deliberately: one dimension from the datum face to the functional face with a tolerance of its own, instead of a chain of individual steps. How much that matters is shown in the comparison of stack-up methods.
Conversely, chain dimensioning helps where the spacings matter more than the position relative to a datum, for example a row of holes for a connector strip. The dimensioning decides which dimensions are toleranced and which ones fall out of the others. It is one of the few places where the drawing genuinely determines the function.
What has changed on the standards side
ISO 2768 with its two parts dates from the 1980s. Since 2021 there has been a successor for the geometrical part in ISO 22081, which takes a different route: instead of fixed class values it requires an explicit statement of the general geometrical tolerance and a datum in the title block.
In existing drawings that has barely caught on. In practice you will be reading ISO 2768-mK for a long time yet, and as long as both sides mean the same thing by it, that works. It gets awkward in international supply chains where the inspection department no longer has the withdrawn edition to hand.
Whichever edition applies, the practical advice stays the same: choose the general tolerance once, deliberately, instead of inheriting it, and tolerance the three to five dimensions the function depends on individually. Everything else is negotiable.
Frequently asked questions
Do general tolerances apply to radii and chamfers as well?
Yes, ISO 2768-1 has its own columns for radii and chamfer heights, with considerably coarser values than for linear dimensions. There is a separate table for angular dimensions too, whose tolerance decreases with the length of the shorter leg.
What happens if a dimension exceeds the general tolerance?
Under ISO 2768-1 a part is not automatically scrap as long as its function is not impaired. That is a weak point in every complaint, because function is eminently arguable. Where you want to avoid that discussion, the dimension belongs in an individual tolerance.
Can I simply always use ISO 2768-f?
Technically yes, economically rarely. On machined parts it often costs little. As soon as weldments, tubes, sheet metal bends or bought-in blanks are involved, the fine class creates inspection effort and rework for dimensions that carry no function.
How do general tolerances and fits relate?
They do not. A fit designation such as H7 is an individual tolerance and always takes precedence. The general tolerance applies only to dimensions without one of their own. Problems arise where a fitted feature is dimensioned from a face whose own position is only covered by the general tolerance.