ISO 2768 general tolerances: f, m, c, v and H, K, L tables
Published September 28, 2026 — permissible deviations for lengths, radii, chamfers and angles, general geometrical tolerances, a min/max size calculator, and the right way to write “ISO 2768-mK” on your drawings.
ISO 2768 general tolerance calculator
Enter a dimension and the class from your title block: you get the ISO 2768-1 permissible deviation and the min/max sizes. For an angle, enter the length of the shorter side of the angle.
Example: an 85 mm length in class m is ± 0.3 mm (30 to 120 range): between 84.7 and 85.3 mm. In class f, ± 0.15 mm.
1. Linear dimensions (ISO 2768-1)
Permissible deviations in millimetres, by nominal size range (over … up to and including …). A dash means the standard gives no value: the dimension must carry its own tolerance.
Below 0.5 mm, the standard doesn't apply: such dimensions must always carry their own tolerance.
2. Radii, chamfers and angles
External radii and chamfer heights (± mm):
Angles, by length of the shorter side of the angle (mm):
3. General geometrical tolerances H, K, L (ISO 2768-2)
The second letter in the title block (the “K” in “mK”) sets unstated form and orientation tolerances. Values in millimetres. For tolerances stated on the drawing in a frame, see the 14 ISO 1101 geometrical tolerance symbols.
Straightness and flatness, by nominal length:
Perpendicularity, by length of the shorter side:
Symmetry, by length:
Circular run-out (radial, axial): 0.1 mm in H, 0.2 mm in K, 0.5 mm in L.
Standards status: ISO 2768-2 was withdrawn and replaced by ISO 22081:2021, which sets rules for using general tolerances within the GPS system but no longer gives values. ISO 2768-1 remains in force. In practice, “ISO 2768-mK” is still very common on drawings: if you put it on a new drawing, make sure your suppliers and inspection read it the same way.
4. In the title block, and in SOLIDWORKS
The note goes in or near the title block: “General tolerances ISO 2768-mK”. The first letter (f, m, c, v) applies to dimensions, the second (H, K, L) to geometry. m matches ordinary machining; f careful machining; c and v sheet metal, weldments or rough parts. On a weldment drawing, welds are read with the ISO 2553 welding symbols.
- Put the note in the sheet format, not by hand on each drawing: in SOLIDWORKS, a custom property (for example “TolGen”) linked to a note in the sheet format lets you change it per part without touching the title-block template.
- Only put individual tolerances on functional dimensions. Everything else is covered by the general tolerance: a readable drawing is one that shows where the precision is. Surface finish follows the same logic: one general roughness near the title block, then only the exceptions (see Ra roughness: N grades and the value to specify by function).
- Fits are not covered by ISO 2768: a Ø 20 H7 is toleranced with ISO 286, see the H7/g6 fit calculator.
Standardising this note across a whole drawing base is typically a SOLIDWORKS codification and properties job: one property, one rule, one sheet format.
5. FAQ
What does ISO 2768-mK mean on a drawing?
That every dimension without a stated tolerance follows class m (medium) of ISO 2768-1, and every unstated form and orientation tolerance follows class K of ISO 2768-2. For example, a 50 mm length is then ± 0.3 mm.
What is the ISO 2768-m tolerance for 100 mm?
± 0.3 mm. 100 mm falls in the over 30 up to 120 mm range. In class f it would be ± 0.15 mm, in class c ± 0.8 mm.
Is ISO 2768 still valid?
ISO 2768-1 (linear and angular dimensions) is still in force. ISO 2768-2 (geometrical tolerances) was replaced by ISO 22081:2021, which no longer sets values. The ISO 2768-mK note remains widely used in industry.
Which class should I choose between f, m, c and v?
m for ordinary machining, f for precision machining, c for sheet metal and weldments, v for rough or very large parts. Choosing finer than needed raises manufacturing and inspection cost for no benefit.
Does the general tolerance apply to fit diameters?
No. A functional dimension, such as a fit diameter, must carry its own tolerance (for example Ø 20 H7 per ISO 286). The general tolerance only covers non-functional dimensions.