Machining tolerances: ISO 2768, fits and dimensioning

No machined part is exactly at its nominal dimension: the tolerance sets the permissible deviation. Rather than writing a tolerance on every dimension, the drawing can refer, in its title block, to a general tolerance standard. ISO 2768-1 covers linear and angular dimensions that have no individual tolerance, and defines four classes: f (fine), m (medium), c (coarse) and v (very coarse).

Permissible deviations for linear dimensions, in millimetres (symmetrical deviations, plus or minus). “Over 3 up to 6” means beyond 3 mm and up to and including 6 mm:

Example: a 50 mm dimension with no individual tolerance, on a drawing in class m, can vary by ±0.3 mm (between 49.7 and 50.3 mm); in class f, by ±0.15 mm. The standard also provides separate tables for radii, chamfers and angles, not reproduced here. Class m is very common on mechanical part drawings.

A dimension within its tolerance does not guarantee a perfect shape: a part can meet all its dimensions and still be warped. Part 2 of the standard sets general geometrical tolerances, notably for straightness, flatness, perpendicularity, symmetry and run-out, in three classes: H (the finest), K and L (the widest).

The designation combines the two parts. The note “General tolerances ISO 2768-mK” in the title block means: class m for linear and angular dimensions, class K for geometry. Without a note of this kind, no general tolerance applies normatively: the workshop then falls back on its own practice, which is a source of disputes.

In the more recent GPS (Geometrical Product Specifications) approach, ISO 22081 (2021) covers general geometrical specifications and replaces ISO 2768-2. The ISO 2768-mK note nevertheless remains very widespread on existing drawings, and most workshops understand it. Check with your design office which reference your company uses.

When two parts are assembled (a shaft in a bore, for example), the tolerance of each determines the clearance or interference obtained. The ISO fit system (ISO 286) standardises these tolerances through two pieces of information: the IT grade (the number, from IT01 to IT18; the smaller it is, the tighter the tolerance) and the position of the tolerance zone relative to the nominal dimension (the letter, upper case for a bore, lower case for a shaft).

The notation H7/g6 reads: H7 bore and g6 shaft. The basic hole system (H) is the most common: the bore keeps the same position and the shaft letter is varied to obtain clearance (g, h, f), a transition fit (k, js) or interference (p, s). Example for a nominal diameter of 25 mm:

These values apply to the 18 to 30 mm diameter range: they change with diameter. Consult the ISO 286-2 tables or ask your workshop for them. On the manufacturing side, an H7 bore is commonly produced by fine boring or reaming; finer grades such as IT6 often call for grinding.

Geometrical tolerancing expresses the function of the part better than an accumulation of plus-or-minus dimensions. It is defined by ISO 1101, within the framework of Geometrical Product Specifications (GPS). A requirement is written in a tolerance frame: the characteristic symbol, the value of the tolerance zone (preceded by Ø for a cylindrical zone), then one or more datums (A, B, C), defined by ISO 5459. The characteristics are grouped into families:

• Form (no datum): straightness, flatness, circularity, cylindricity.
• Orientation: parallelism, perpendicularity, angularity.
• Location: position, coaxiality, concentricity, symmetry.
• Run-out: circular run-out and total run-out.
• Profile: profile of a line or of any surface.

Why use it? To locate two fixing holes, coordinate dimensioning of ±a gives a square tolerance zone of side a. Positional tolerancing defines a circular zone: if you take the circle circumscribing that square (diameter of about 1.41 a), the permissible area increases by about 57%. For an assembly that depends on radial deviation (a screw in a hole, a dowel in a bore), this zone better matches the function and leaves the workshop more margin. In return, the datums must reflect how the part is actually mounted.

Drawings of North American origin often follow the ASME Y14.5 standard, close to ISO 1101 but different in some respects: tell the workshop. Checking these requirements generally requires a coordinate measuring machine.

Ra roughness is the arithmetic mean deviation of the profile, expressed in micrometres. It was long defined by ISO 4287 and shown on drawings according to ISO 1302; the ISO 21920 series is gradually replacing them. The following orders of magnitude are indicative and depend on the material, the tool and the cutting parameters:

Ra does not tell the whole story: two surfaces with the same Ra can have different textures. For most parts, a general note (“Ra 3.2 unless otherwise stated”, for example) completed by a few flagged surfaces is enough. Each step up in fineness adds passes, or even a grinding operation.

Tightening a tolerance does not cost proportionally. As long as the requirement stays within the machine’s normal capabilities, the effect is moderate. Beyond that, the workshop changes method, and every change costs money:

• slower finishing passes, more carefully chosen tools replaced earlier;
• thermal stabilisation of the part and the machine, the reference temperature for measurement being set at 20 °C;
• additional operations (grinding, rework on another machine);
• finer inspection, often on every part, with a measuring method whose uncertainty remains well below the tolerance; the one-tenth rule of thumb is often cited;
• a higher risk of scrap, passed on in the price.

1. Start from the function. For each surface, ask yourself what happens if the dimension varies: if nothing changes, the general tolerance is enough.
2. Put general tolerances in the title block (ISO 2768-mK, for example), then dimension individually only the functional features.
3. Use standardised fits (H7/g6, H7/h6…) rather than custom values.
4. Prefer geometrical tolerancing for positions to make use of a circular zone, with datums that reflect how the part is mounted.
5. Avoid redundant or chain dimensioning. Each dimension appears only once; an auxiliary dimension goes in brackets and is not inspected.
6. State whether dimensions apply before or after treatment. A thick coating such as hard anodising or electroless nickel changes dimensions by a few microns to several tens of microns.
7. Distinguish machine accuracy from functional tolerance. What the machine can do is not what your part requires.

Once your drawing is dimensioned, attach it to a complete specification. On Meaflow, posting a request is free: you can ask the suppliers who reply to flag the dimensions that make the part more expensive. For materials, see materials for machined parts.