Why tolerances are needed
No dimension can be made exactly. A tolerance states how far the dimension may deviate and still be accepted. If the drawing says 20 ±0.1 mm, anything between 19.9 and 20.1 mm is correct.
Tolerances cost money. A tolerance twice as tight can require an extra operation, slower machining or more measuring. The aim is therefore not to specify tolerances as tight as possible, but to specify the right tolerance on the right dimension: tight where parts fit together, generous everywhere else.
Tolerances are given in millimetres for linear dimensions and in degrees and minutes for angles. The table values in the ISO standards apply at 20 °C, the reference temperature for measurement under ISO 1.
General tolerances to ISO 2768-1
ISO 2768-1 gives general tolerances for linear and angular dimensions that have no tolerance of their own on the drawing. The standard has four tolerance classes: f (fine), m (medium), c (coarse) and v (very coarse). The class is written in or near the title block, for example “ISO 2768-m”.
The tolerance depends on the size of the dimension. In class m, ±0.1 mm applies to dimensions from 0.5 to 6 mm, ±0.2 mm above 6 up to 30 mm, ±0.3 mm above 30 up to 120 mm and ±0.5 mm above 120 up to 400 mm. The full table is further down the page.
Class m is the most common choice for milling and turning. Class f is used for precision engineering and costs more. Class c suits welded structures, rough machining and many plastic parts.
Geometric general tolerances – straightness, flatness, perpendicularity – used to be specified with ISO 2768-2 and the classes H, K and L, for example “ISO 2768-mK”. ISO 2768-2 has been replaced by ISO 22081, but the old designation still appears on many drawings.
Radii, chamfers and angles
ISO 2768-1 has its own tolerances for radii and chamfer heights. In classes f and m, ±0.2 mm applies for 0.5–3 mm, ±0.5 mm above 3 up to 6 mm and ±1 mm above 6 mm. In classes c and v the values are twice as large.
The angular tolerance depends on the length of the shorter leg. In class m, ±1° applies up to 10 mm, ±0°30′ above 10 up to 50 mm and ±0°20′ above 50 up to 120 mm. The longer the leg, the tighter the angular tolerance – because a small angular deviation gives a large positional deviation at the end.
Fits to ISO 286 – the hole-basis system
When a shaft has to go into a hole, ± tolerances are not enough. That is where ISO 286-1 and ISO 286-2 come in, giving the tolerance position as a letter and the tolerance grade as a number. A capital letter refers to a hole, a lower-case letter to a shaft.
In Europe the hole-basis system is almost always used. The hole gets tolerance H, where the lower limit is exactly the nominal size. A Ø20 H7 hole may be between 20.000 and 20.021 mm. The shaft tolerance is then chosen according to the fit you want. The advantage is that the workshop can use standard tools such as reamers and plug gauges for the hole.
The number is the IT tolerance grade. A higher number means a larger tolerance. For Ø20, IT6 is 0.013 mm, IT7 0.021 mm and IT9 0.052 mm. The size of the tolerance also grows with the diameter.
Clearance, transition and interference fits
A clearance fit always has a gap between shaft and hole. H7/g6 gives a small but reliable clearance and is used for sliding and rotating parts with good guidance, such as a piston or a pivot pin. H7/h6 is a sliding fit with clearance from zero upwards, for parts that are assembled by hand and must be accurately located.
A transition fit can end up with either slight clearance or slight interference, depending on where in the tolerances the parts land. H7/k6 is used for gears, pulleys and bearing inner rings that must stay in place but can be dismantled.
An interference fit always has interference. H7/p6 is used, for example, for bushings and pins in hubs that are pressed in and stay put without adhesive or screws. With interference fits, material matters a lot: aluminium, steel and plastic tolerate different amounts of interference.
The table below shows the limits for Ø20 mm. Other diameters have other values according to ISO 286-2.
Example: a milled plate with dowel pins
Imagine a milled aluminium plate measuring 120 × 80 mm with four screw holes and two holes for dowel pins. The drawing specifies ISO 2768-m as the general tolerance. The 120 mm length may then deviate by ±0.3 mm and the 80 mm width also by ±0.3 mm. That is more than enough for outer dimensions that do not mate with anything.
The clearance holes for M6 are drilled Ø6.6 mm, giving 0.6 mm clearance. The hole positions can therefore often stay on the general tolerance, as long as the other part has the same clearance.
The dowel pins, however, must locate the plate exactly. A parallel pin to ISO 8734 has tolerance m6. In a Ø8 H7 hole this gives a transition fit: the pin stays in place but can be knocked out. The hole spacing gets its own, tighter tolerance, for example ±0.02 mm, or a position tolerance to ISO 1101. The result is a drawing where only two dimensions are expensive – the rest is made to standard accuracy.
Tolerances for 3D printing compared with CNC
CNC milling typically gives ±0.05–0.1 mm without special measures, and tighter tolerances with finishing passes. Fits such as H7 often require reaming or boring.
FDM printing is coarser. A guide value for a well-tuned print is ±0.1–0.2 mm on dimensions in the XY plane and roughly one layer height in Z. Holes often come out 0.1–0.3 mm undersize. Fits such as H7/g6 cannot be printed directly – instead a clearance is designed in, typically 0.2–0.4 mm, or the hole is drilled and reamed afterwards.
So state on the drawing which method the part will be made with, and give 3D-printed parts realistic tolerances. More on this in the guide [[g_3dutskrift|3D printing materials and design rules]].
Common mistakes with tolerances
The most common mistake is putting ±0.01 mm on every dimension. That makes the part expensive without making it work better. Another is chain dimensioning so that the errors add up – dimension from a common datum instead.
Other mistakes are forgetting the general tolerance class, specifying a fit without considering the material and mixing up hole and shaft tolerances. Want help with tolerancing? Read about technical drawings or send your drawing for review.
ISO 2768-1: general tolerances for linear dimensions (mm)
| Size range (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5–3 | ±0.05 | ±0.1 | ±0.2 | – |
| over 3–6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| over 6–30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| over 30–120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| over 120–400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| over 400–1000 | ±0.3 | ±0.8 | ±2 | ±4 |
| over 1000–2000 | ±0.5 | ±1.2 | ±3 | ±6 |
Fits for Ø20 mm to ISO 286-2: hole H7 = 20.000–20.021. Shaft g6 = 19.980–19.993 (clearance 0.007–0.041). Shaft h6 = 19.987–20.000 (clearance 0–0.034). Shaft k6 = 20.002–20.015 (clearance 0.019 to interference 0.015). Shaft p6 = 20.022–20.035 (interference 0.001–0.035). Always check against the current edition of the standard.
Checklist for tolerancing
- General tolerance class stated, for example ISO 2768-m
- Tight tolerances only on dimensions that affect function and fit
- Dimensioning from common datums, not in chains
- Fits given with an ISO 286 designation, e.g. Ø20 H7/g6
- Hole-basis system (H holes) unless something else is required
- Material considered for interference fits
- Realistic tolerances for 3D-printed parts (guide value ±0.1–0.2 mm)
- Manufacturing method stated on the drawing
Frequently asked questions
What does ISO 2768-m mean on a drawing?
It means that all dimensions without their own tolerance are made to tolerance class m in ISO 2768-1. A 50 mm dimension may then deviate by ±0.3 mm and a 10 mm dimension by ±0.2 mm. Class m is the most common for milling and turning.
What is the difference between H7/g6 and H7/h6?
H7/g6 is a clearance fit that always has a little play, for parts that rotate or slide. H7/h6 has clearance from zero upwards and is used when parts are assembled by hand but must be accurately located. Both are clearance fits under ISO 286.
Which fit should I choose to press in a bushing?
An interference fit such as H7/p6 is a common choice for steel or bronze bushings. The interference depends on the diameter and the materials, so always check that the hub can take the stress. In plastic and aluminium, less interference is often needed.
What tolerances can 3D printing achieve?
A guide value for FDM is ±0.1–0.2 mm in the XY plane. Holes often come out slightly undersize. For fits, a clearance of 0.2–0.4 mm is designed in, or the hole is finished afterwards.