No part is ever made exactly to size. A shaft drawn at 25 mm might come out at 24.993 or 25.004. A tolerance tells the workshop how far from the drawn size a feature may be and still work. Too loose and parts rattle, leak or don’t line up; too tight and every part costs more than it needs to. Choosing tolerances is where design meets manufacturing cost.
Size tolerances
A tolerance can be written in several ways:
- Limits: 25.021 / 25.000
- Plus and minus: 50 ±0.1, or 50 +0.2/−0 for a one-sided tolerance
- ISO fit code: ⌀25 H7, which the reader looks up in ISO 286
- General tolerance: a note such as “ISO 2768-m” in the title block covers every dimension without its own tolerance
IT grades
ISO 286 defines international tolerance (IT) grades: the smaller the number, the tighter the tolerance. The width of the tolerance also grows with size, so a 25 mm IT7 tolerance is 21 µm but a 100 mm IT7 tolerance is 35 µm.
| IT grade | Typical process | Typical use |
|---|---|---|
| IT5–IT6 | Grinding, honing | Bearing seats, precision spindles |
| IT7 | Fine turning, reaming, boring | Fits for bearings, dowels and gears |
| IT8–IT9 | Normal turning and milling | Running fits, general machined features |
| IT10–IT11 | Drilling, rough machining | Clearance holes, non-critical features |
| IT12–IT14 | Sheet metal, casting, rough work | Features with no fit |
Fits
A fit is the relationship between a hole and the shaft that goes in it. ISO 286 describes each with a letter (the position of the tolerance zone) and a number (the IT grade). Capital letters are holes, lower case are shafts. In the hole-basis system, used almost everywhere, the hole is always H (its lower limit is the nominal size) and the shaft letter is chosen to give the fit.
| Fit | Type | Typical use |
|---|---|---|
| H11/c11 | Loose running | Agricultural machines, dirty conditions |
| H9/d9 | Free running | Large temperature changes, idler gears |
| H8/f7 | Close running | Shafts in plain bearings, gearbox spindles |
| H7/g6 | Sliding | Locating pins, sliding gears, parts that must move without play |
| H7/h6 | Locational clearance | Parts that are assembled and taken apart by hand |
| H7/k6 | Transition | Gears and pulleys on shafts, located accurately, light press |
| H7/p6 | Light interference | Bushes, permanent location, press fit |
| H7/s6 | Medium drive | Bronze bushes, couplings, fits that carry torque |
Worked example: clearance and interference in three fits
Find the limits for a 25 mm hole H7 with shafts g6, k6 and p6 (ISO 286 values for 18–30 mm: H7 = 0 to +21 µm; g6 = −7 to −20 µm; k6 = +2 to +15 µm; p6 = +22 to +35 µm).
Hole H7: 25.000 to 25.021 mm.
H7/g6: shaft 24.980 to 24.993 mm.
H7/k6: shaft 25.002 to 25.015 mm.
H7/p6: shaft 25.022 to 25.035 mm.
Tolerance stack-up
When several parts sit in a row, their tolerances add up. The gap or overall length at the end of the chain varies by the sum of all the individual tolerances in the worst case.
Worked example: three parts in a row
Three spacers measure 20 ±0.1, 30 ±0.1 and 15 ±0.05 mm. What range of overall length can occur?
Worst case: add the tolerances.
Statistical (root sum square): parts are rarely all at their limits at once, so for large batches:
Stack-ups explain why good designs keep chains short, dimension critical features from one datum, and use an adjustable part (a shim or slotted hole) where the stack can’t be controlled.
GD&T basics
A size tolerance controls how big a feature is, but not its shape, angle or position. A ⌀25 shaft can be within size and still bent like a banana; a hole can be the right size but in the wrong place. Geometric dimensioning and tolerancing (GD&T) controls those things, using symbols defined in ASME Y14.5 (USA) and ISO 1101 (ISO GPS).
Datums
A datum is a reference feature, usually a flat face, a hole or a shaft axis, from which other features are measured. Datums are marked with a letter in a box attached to a triangle. Their order (A, then B, then C) says how the part is placed in the inspection fixture: on A first, then against B, then against C.
The feature control frame
Each geometric tolerance is written in a frame, read from left to right: the characteristic symbol, the tolerance zone (⌀ means a cylindrical zone) with any modifiers, then the datums in order.
| Group | Characteristics | Datum needed? |
|---|---|---|
| Form | Straightness, flatness, circularity, cylindricity | No |
| Orientation | Perpendicularity, parallelism, angularity | Yes |
| Location | Position (plus concentricity and symmetry in ISO) | Yes |
| Profile | Profile of a line, profile of a surface | Optional |
| Runout | Circular runout, total runout | Yes |
The modifier Ⓜ (maximum material condition) after the tolerance lets the position tolerance grow as the hole gets bigger than its smallest size, which still guarantees assembly with a bolt but allows more parts to pass.
Worked example: why position beats ± coordinates
A hole’s position is toleranced as ±0.05 mm in X and in Y. That gives a 0.1 mm square zone. Find the position tolerance (a round zone) that accepts every hole the square accepts.
The furthest a hole can be in the square is its corner:
A ⌀0.141 circle contains the whole square, and its area is
Choosing tolerances sensibly
- Start from function: which features locate, seal, slide or carry load? Tolerance those tightly; leave the rest to the general tolerance.
- Use standard fits rather than inventing limits.
- Ask what the process can hold. Tighter than about IT7 on a turned part usually means grinding.
- Dimension from datums that match how the part is located in use and in inspection.
- Check the stack-up for every critical gap in the assembly.
Key points
- Every dimension needs a tolerance, either its own or the general tolerance.
- IT grade sets the width of the zone; the fit letter sets its position. H7/g6 slides, H7/k6 locates, H7/p6 presses.
- Worst-case stack-up adds tolerances; RSS gives a realistic range for large batches.
- GD&T controls form, orientation, location, profile and runout, measured from datums.