Dimensional tolerances: forgings, machining (ISO 286, H7) and ISO 2768
A drawing without tolerances turns into an argument at delivery. A forging has wide tolerances and machining allowance; a machined part has general tolerances (ISO 2768) and, on mating dimensions, an ISO 286 fit (such as H7).
From forging to machined part
- Open-die forging: leaves with machining allowance and wide tolerances, defined in the order or in a forging standard (e.g. DIN 7527 for open-die forgings*). State the final machined dimensions and let the forger define the allowance.
- Closed-die forging: tolerances per EN 10243-1, according to mass, shape and precision class.
- Machined part: dimensions without tolerance follow the general tolerance stated on the drawing (usually ISO 2768-m); mating dimensions receive an ISO 286 fit (e.g. Ø50 H7).
- ASME B16.5 flanges: the standard itself gives the tolerances for diameter, thickness and bolt pattern. See the B16.5 flanges.
ISO 2768-1 general tolerances (linear dimensions)
| Range (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 to 3 | ±0.05 | ±0.1 | ±0.2 | – |
| over 3 to 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| over 6 to 30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| over 30 to 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| over 120 to 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| over 400 to 1,000 | ±0.3 | ±0.8 | ±2 | ±4 |
| over 1,000 to 2,000 | ±0.5 | ±1.2 | ±3 | ±6 |
| over 2,000 to 4,000 | – | ±2 | ±4 | ±8 |
On the drawing it appears as "ISO 2768-m" (or -mK, with part 2 for form and position). Class m is the most used in general machining.
IT tolerance grades (ISO 286-1)
| Diameter (mm) | IT6 | IT7 | IT8 | IT9 | IT11 |
|---|---|---|---|---|---|
| over 6 to 10 | 9 | 15 | 22 | 36 | 90 |
| over 10 to 18 | 11 | 18 | 27 | 43 | 110 |
| over 18 to 30 | 13 | 21 | 33 | 52 | 130 |
| over 30 to 50 | 16 | 25 | 39 | 62 | 160 |
| over 50 to 80 | 19 | 30 | 46 | 74 | 190 |
| over 80 to 120 | 22 | 35 | 54 | 87 | 220 |
| over 120 to 180 | 25 | 40 | 63 | 100 | 250 |
| over 180 to 250 | 29 | 46 | 72 | 115 | 290 |
| over 250 to 315 | 32 | 52 | 81 | 130 | 320 |
An H hole has zero lower deviation: Ø50 H7 = 50.000 to 50.025 mm. An h shaft has zero upper deviation: Ø50 h6 = 49.984 to 50.000 mm.
Most used fits (hole-basis system H7)
| Fit | Type | Typical use |
|---|---|---|
| H7/g6 | Clearance (sliding) | Parts that rotate or slide with precision: guides, pivot pins |
| H7/h6 | Minimum clearance (locational) | Centering of removable parts |
| H7/k6 | Transition | Bearings, pulleys and couplings assembled with light pressure |
| H7/p6 | Interference | Pressed-in bushings and gears, without key |
Surface roughness (Ra)
| Process | Typical Ra (µm) |
|---|---|
| Forging without machining | 12.5 to 25 or more* |
| Rough turning and milling | 6.3 to 12.5* |
| Finish turning and milling | 1.6 to 3.2* |
| Grinding | 0.4 to 1.6* |
| Raised face (RF) flange facing, ASME B16.5 | 3.2 to 6.3 (125 to 250 µin), serrated |
* Typical shop values. The drawing must state the required Ra on sealing and mating faces.
In practice
- Tolerance only what needs it: tight tolerances over the whole part make machining more expensive with no gain.
- In nickel alloys, duplex and titanium machining is slower: tolerance and roughness define much of the lead time and cost.
- Send the drawing with material, tolerances and roughness. See machining.
Frequently asked questions
What does H7 on the drawing mean?
It is the tolerance of a hole per ISO 286: H means the hole may be equal to or larger than the nominal size (zero lower deviation) and 7 is the IT7 tolerance grade. For Ø50 H7 the hole ranges from 50.000 to 50.025 mm.
Which tolerance applies to a dimension without tolerance on the drawing?
The general tolerance stated in the title block, usually ISO 2768-m. On a 100 mm dimension, that gives ±0.3 mm. If the drawing states none, agree on it before fabrication.
What is the machining allowance of a forging?
It depends on size, shape and process. State the final dimensions of the machined part and the forger defines the allowance; in the forging calculator you can simulate it with the allowance per face.
