Reference & calculator Design ~7 min read
What your title block really says

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.

mK The most common note
4 Linear classes f, m, c, v
± 0.3 mm for 50 mm in class m

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.

Permissible deviation
—
Min size
—
Max size
—

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.

Full Excel version, for checking a drawing or a part: all 50 untoleranced dimensions on one sheet (lengths, radii, chamfers and angles), the title-block class or a class per dimension, min and max sizes, and a pass / out-of-tolerance verdict on measured values. Includes H, K, L geometrical tolerances and ISO 286 fits. Offline, no macros, English and French workbooks.

Get the workbook · $9 or the bundle with the tolerance stack-up calculator, $15

Secure checkout by Gumroad · instant download · standard Excel formulas, also checked in LibreOffice Calc · all Excel templates

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.

Class0.5 – 33 – 66 – 3030 – 120120 – 400400 – 10001000 – 20002000 – 4000
f (fine)± 0.05± 0.05± 0.1± 0.15± 0.2± 0.3± 0.5—
m (medium)± 0.1± 0.1± 0.2± 0.3± 0.5± 0.8± 1.2± 2
c (coarse)± 0.2± 0.3± 0.5± 0.8± 1.2± 2± 3± 4
v (very coarse)—± 0.5± 1± 1.5± 2.5± 4± 6± 8

Below 0.5 mm, the standard doesn't apply: such dimensions must always carry their own tolerance.

Printable version: the ISO 2768 tables (f, m, c, v and H, K, L) as a PDF (A4, no sign-up), to pin up in the workshop or keep in a binder.

2. Radii, chamfers and angles

External radii and chamfer heights (± mm):

Class0.5 – 33 – 6> 6
f (fine)± 0.2± 0.5± 1
m (medium)± 0.2± 0.5± 1
c (coarse)± 0.4± 1± 2
v (very coarse)± 0.4± 1± 2

Angles, by length of the shorter side of the angle (mm):

Class≤ 1010 – 5050 – 120120 – 400> 400
f (fine)±1°±0°30′±0°20′±0°10′±0°5′
m (medium)±1°±0°30′±0°20′±0°10′±0°5′
c (coarse)±1°30′±1°±0°30′±0°15′±0°10′
v (very coarse)±3°±2°±1°±0°30′±0°20′

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:

Class≤ 1010 – 3030 – 100100 – 300300 – 10001000 – 3000
H0.020.050.10.20.30.4
K0.050.10.20.40.60.8
L0.10.20.40.81.21.6

Perpendicularity, by length of the shorter side:

Class≤ 100100 – 300300 – 10001000 – 3000
H0.20.30.40.5
K0.40.60.81
L0.611.52

Symmetry, by length:

Class≤ 100100 – 300300 – 10001000 – 3000
H0.50.50.50.5
K0.60.60.81
L0.611.52

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. ISO 2768 tolerance table in Excel

To look up a dimension's tolerance in a spreadsheet, copy the table from section 1 with the upper limit of each range in column D and the deviations of classes f, m, c and v in columns E to H (without the ± sign):

RowD: up to (mm)E : fF : mG : cH : v
230.050.10.2
360.050.10.30.5
4300.10.20.51
51200.150.30.81.5
64000.20.51.22.5
71,0000.30.824
82,0000.51.236
94,000248

Row 1 holds the headings f, m, c and v in E1:H1. With the nominal dimension in A2 and the class in B2, the tolerance is:

=INDEX($E$2:$H$9,COUNTIF($D$2:$D$9,"<"&A2)+1,MATCH(B2,$E$1:$H$1,0))

COUNTIF counts the upper limits strictly below the dimension: a 6 mm dimension stays in the 3 – 6 range, 6.5 mm moves to the 6 – 30 range, as the standard says ("over 6 up to 30"). The formula works in every Excel version, with no array formula. Example: 45 mm in class m gives 0.3, i.e. 44.7 to 45.3 mm. Minimum size =A2-C2, maximum size =A2+C2 with the tolerance in C2. An empty cell (f above 2,000 mm, v up to 3 mm) returns 0: it means "not defined", not "zero tolerance".

For a whole drawing, the ISO 2768 and ISO 286 tolerance calculator for Excel ($9) handles 50 dimensions with a pass/fail verdict on the measured value, radii, chamfers and angles, 30 ISO 2768-2 lines (H, K, L) and 30 ISO 286 fits.

6. 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.

Read next