CNC machining
Milling, turning, 3- to 5-axis machining centres
Free calculator
ISO 2768-1 general tolerances: free calculator
Enter a dimension and a class (f, m, c or v): you get the permissible deviation, along with broken edges and angles. The standard’s full tables are just below.
- Free, no sign-up
- Calculated in your browser
- Formulas and tables shown
ISO 2768-1 general tolerance calculator
Linear dimension · class m (medium)
±0.3 mm
Permitted actual dimension: from 49.7 to 50.3 mm
Table 1, row “over 30 up to and including 120 mm”
Broken edge of 2 mm
±0.2 mm
External radius or chamfer · table 2, row “over 0.5 up to and including 3 mm”
Angle, shorter side of 40 mm
±0°30′
Table 3, row “over 10 up to and including 50 mm” · i.e. approximately ±0.35 mm at the end of the side
Title block note: General tolerances ISO 2768-m
The calculation is done in your browser: the values you enter are neither sent nor saved.
The ISO 2768-1 tables
The row and column that match your input are highlighted. “Over 30 up to and including 120” means that 30 mm belongs to the previous row and 120 mm to this one.
Table 1: linear dimensions (deviations in mm)
| Nominal dimension (mm) | ffine | mmedium | ccoarse | vvery coarse |
|---|---|---|---|---|
| from 0.5up to and including 3 | ±0.05 | ±0.1 | ±0.2 | — |
| over 3up to and including 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| over 6up to and including 30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| over 30up to and including 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| over 120up to and including 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| over 400up to and including 1,000 | ±0.3 | ±0.8 | ±2 | ±4 |
| over 1,000up to and including 2,000 | ±0.5 | ±1.2 | ±3 | ±6 |
| over 2,000up to and including 4,000 | — | ±2 | ±4 | ±8 |
Table 2: broken edges (mm)
| Radius or chamfer (mm) | ffine | mmedium | ccoarse | vvery coarse |
|---|---|---|---|---|
| from 0.5up to and including 3 | ±0.2 | ±0.2 | ±0.4 | ±0.4 |
| over 3up to and including 6 | ±0.5 | ±0.5 | ±1 | ±1 |
| over 6 | ±1 | ±1 | ±2 | ±2 |
Table 3: angular dimensions
| Shorter side (mm) | ffine | mmedium | ccoarse | vvery coarse |
|---|---|---|---|---|
| up to and including 10 | ±1° | ±1° | ±1°30′ | ±3° |
| over 10up to and including 50 | ±0°30′ | ±0°30′ | ±1° | ±2° |
| over 50up to and including 120 | ±0°20′ | ±0°20′ | ±0°30′ | ±1° |
| over 120up to and including 400 | ±0°10′ | ±0°10′ | ±0°15′ | ±0°30′ |
| over 400 | ±0°5′ | ±0°5′ | ±0°10′ | ±0°20′ |
A dash means the standard gives no value: the tolerance is then stated next to the dimension. Below 0.5 mm there is no value either. The deviations are symmetrical. Part 2 of the standard (ISO 2768-2, classes H, K and L) deals with general geometrical tolerances: it exists, but this tool does not cover it. See the guide on machining tolerances and ISO 2768.
How to read the result
ISO 2768-1 sets general tolerances: they apply to all linear and angular dimensions on a drawing that carry no individual tolerance. The calculator reads the standard’s table for you: the nominal dimension selects the row, the class selects the column. The result is a symmetrical “±” deviation, in millimetres. For 50 mm in class m, the actual dimension of the part may vary from 49.7 to 50.3 mm.
The four classes run from tightest to widest: f (fine), m (medium), c (coarse) and v (very coarse). Class m is the most common on mechanical part drawings. The finer the class, the more care the workshop must take over machining and inspection, which affects the price.
The calculator’s three results
- Linear dimensions (table 1): lengths, widths, thicknesses, diameters, distances, external and internal dimensions, from 0.5 to 4,000 mm.
- Broken edges (table 2): external radii and chamfer heights. The deviation depends on the size of the radius or chamfer itself, not on the size of the part. Other radii follow table 1.
- Angles (table 3): the deviation depends on the length of the shorter side of the angle, not on the angle itself. The standard also covers right angles that are not dimensioned.
The equivalent deviation of an angle
Below the angular result, the calculator shows an equivalent deviation in millimetres. This is a geometrical calculation, not a value from the standard: at the end of a side of length L, an angular deviation α shifts the point by L × tan α. For a 100 mm side and ±0°30′, that is approximately ±0.87 mm. It helps you picture the deviation; the tolerance itself remains expressed in degrees and minutes.
Pitfalls to avoid
- With no note in the title block, nothing applies. General tolerances only apply if the drawing cites them (“ISO 2768-m”, for example). Otherwise the workshop applies its own practice, which is a classic source of disputes.
- Below 0.5 mm, the standard is silent. The tolerance must then be written next to the dimension. The dashes in the table (class v from 0.5 to 3 mm, class f above 2,000 mm) mean the same thing: no value is defined.
- The limits are “over … up to and including …”. In class m, a 30 mm dimension gives ±0.2 mm and a 30.1 mm dimension gives ±0.3 mm. Check which side of the limit your dimension falls on.
- The deviations concern dimensions, not form. ISO 2768-1 limits neither flatness, nor perpendicularity, nor run-out. These general geometrical tolerances fall under part 2 of the standard (classes H, K and L, hence the note “ISO 2768-mK”), which this tool does not cover. On recent drawings, ISO 22081 sometimes replaces it: check the reference adopted by your design office.
- Each standard has its own scope. ISO 2768 covers machined parts and parts formed from sheet metal. Welded assemblies fall under ISO 13920, cast parts under ISO 8062 and functional fits (shaft and bore, such as H7/g6) under ISO 286.
- Before or after treatment. State whether dimensions apply before or after a surface treatment: a hard anodising or electroless nickel layer adds a few microns, sometimes several tens.
In a drawing and in a request for quote
Put the note in the drawing’s title block: “General tolerances ISO 2768-m”, or “ISO 2768-mK” if you also want to cover geometry. Then dimension individually only the functional features (bearing surfaces, fit bores, mounting centre distances). All other dimensions inherit the general tolerance, with no extra reading or inspection effort.
In a request for quote, the class is a pricing factor. A workshop does not price a class f part and a class c part in the same way: state it in the request, alongside the drawing, and flag separately any dimensions tighter than the class. If in doubt, ask the workshops which dimensions on your drawing are the hardest to hold: they are quickly spotted when examining the drawing, and it is often possible to relax them without affecting function.
The guide on machining tolerances explains how to dimension without over-specifying. The specification generator helps you present your whole requirement, and the roughness converter helps you choose the surface finish that goes with your tolerances.
Frequently asked questions
A question not answered here? Visit the help centre or write to us.
What does ISO 2768-m mean on a drawing?
It is a general tolerance note placed in the title block. The letter m designates the “medium” class of ISO 2768-1 for linear and angular dimensions with no individual tolerance. With a second letter (H, K or L, as in “ISO 2768-mK”), the geometrical tolerance class from part 2 of the standard is added.
Which class should I choose: f, m, c or v?
Class m suits the majority of machined mechanical parts. Choose f if the whole part requires precision and your workshop can hold it, and c or v for rough or less demanding parts. Tightening the class increases cost: it is better to keep class m and dimension the few functional features individually.
What should I do with a dimension below 0.5 mm?
ISO 2768-1 gives no deviation below 0.5 mm: the tolerance must be written directly next to the dimension. The same applies to class v from 0.5 to 3 mm and to class f above 2,000 mm, where the table has a dash.
Are the ISO 2768-1 deviations symmetrical?
Yes: the standard gives symmetrical “±” deviations. For a 50 mm dimension in class m, the actual dimension may vary by ±0.3 mm. If you want an asymmetrical or tighter deviation, you need to dimension the feature individually on the drawing.
Does ISO 2768 cover flatness and perpendicularity?
Not part 1, which is used here. Part 2 (classes H, K and L) deals with general geometrical tolerances: straightness, flatness, perpendicularity, symmetry, run-out. This tool only covers part 1, but the guide on machining tolerances presents both.
Related expertise
Workshops to manufacture, treat or inspect the part you are calculating.
Inspection & metrology
Dimensional inspection, NDT, reports
Sheet metalwork & cutting
Laser, plasma and waterjet cutting, bending
Guides to go further
Machining tolerances: ISO 2768, fits and dimensioning
ISO 2768 general tolerances, ISO 286 fits, ISO 1101 geometric tolerancing, Ra roughness: read a drawing and dimension sensibly to control the cost of a machined part.
Writing a manufacturing specification: method and template
What a workshop needs to know to quote and make your part: a method in a few points, a ready-to-copy template and common mistakes to avoid.
CNC machining prices: how is a quote calculated?
Programming, setup, cycle time, material, finishing, inspection: what a CNC machining quote contains, why quantity changes everything and how to reduce the cost.
Other free tools
Converter
Roughness converter
Ra in micrometres, ISO 1302 N grades and microinches, with the processes that achieve each range.
Calculator
Part mass calculation
Plate, round bar, tube, hexagon: volume and mass of the raw stock by material, quantity and density.
Generator
Specification generator
Write a clear specification in 10 minutes, then print it or publish it on Meaflow.
Need this part manufactured?
Describe your part, attach your drawing and compare the workshops’ price quotes. It’s free.