The numbers, by operation
Published capability figures from machining references and platforms such as Protolabs and Fractory cluster around the same values, and they match what UK shops quote in practice.
| Operation | Standard capability | Precision capability | Typical use |
|---|---|---|---|
| CNC milling | ±0.13 mm | ±0.025 mm | Pockets, slots, faces, brackets |
| CNC turning | ±0.13 mm | ±0.02 to 0.025 mm | Shafts, bushes, concentric diameters |
| Drilling | ±0.13 mm | ±0.05 mm | Clearance and pilot holes |
| Reaming | ±0.025 mm | ±0.010 mm | Dowel holes, bearing fits |
| Grinding (secondary) | ±0.005 mm | A few microns | Sealing faces, precision journals |
Read the table the way a machinist does: the part is not made to one tolerance. Different features on the same part carry different numbers, and the process route follows the tightest feature. A bracket with one reamed dowel hole is a milling job with one precise operation, not a precision part.
ISO 2768: the two letters that prevent most tolerance arguments
Most dimensions on most drawings carry no individual tolerance. ISO 2768 exists for exactly those: it defines general tolerances in four grades, f for fine, m for medium, c for coarse and v for very coarse, covering linear dimensions, angles and chamfers by size band.
Writing "ISO 2768-m" in the title block tells the shop precisely how to treat every uncontrolled dimension, and medium is the sensible default for general engineering work. Leave it off and the shop must ask or assume. Assumed general tolerances are one of the quiet causes of goods-inward disputes: the part measures 100.2 mm, the buyer expected 100.0, and nobody wrote down who was right.
For form and position, flatness, position of hole patterns, concentricity, the tool is GD&T rather than a plus-minus band. Use it where the function is genuinely geometric, and remember every GD&T callout is also an inspection instruction someone must carry out and document.
Bar stock has a tolerance too, and it can save a turning operation
Bright steel bar is sold to an ISO 286 tolerance class. The letter h means the bar is never over its nominal size, only under. The number sets how far under. A 25 mm bar to h9 measures between 24.948 and 25.000 mm.
Each figure below is how far under nominal the bar may be, in millimetres. The upper limit is always zero.
| Bar diameter | h9 | h10 | h11 |
|---|---|---|---|
| Over 3 to 6 mm | 0.030 | 0.048 | 0.075 |
| Over 6 to 10 mm | 0.036 | 0.058 | 0.090 |
| Over 10 to 18 mm | 0.043 | 0.070 | 0.110 |
| Over 18 to 30 mm | 0.052 | 0.084 | 0.130 |
| Over 30 to 50 mm | 0.062 | 0.100 | 0.160 |
| Over 50 to 80 mm | 0.074 | 0.120 | 0.190 |
| Over 80 to 120 mm | 0.087 | 0.140 | 0.220 |
Under BS EN 10278, cold drawn round bar is normally supplied to h10, drawn hexagon and square to h11, and precision ground bar to h9, with tighter classes to order. Black bar is hot rolled, looser, and needs machining all over.
This matters on the drawing. If a shaft diameter can live with the bar's own tolerance, draw it at a stock bar size and leave that diameter as supplied. The turning operation disappears from the price. Ask for h7 on the same diameter and it becomes a ground bar or a grinding operation. Confirm the class on the stockholder's quote, because it varies with the grade and the finish. The engineering steel bar guide lists who stocks bright and ground bar, and the bright bar tolerances page has the full table from h6 to h12.
What a tightened digit actually buys
Tolerance is the strongest price dial on a drawing, a point our cost guide makes from the buying side. From the shop floor it looks like this. To hold ±0.127 mm, a machinist cuts the feature and moves on. To hold ±0.025 mm the cuts get lighter, tools get checked and offset more often, the fixture gets stiffer, temperature starts to matter, and the feature gets measured rather than spot-checked. Go finer and the process route changes: the hole gets reamed, the face gets ground, and a second operation with its own setup enters the price.
None of that is padding. It is real work that repeats on every part in every batch. Which is why the expensive habit is not one tight tolerance, it is the blanket-tight drawing: a title block set to ±0.05 mm "to be safe", quietly turning forty ordinary dimensions into precision work nobody will ever measure a benefit from.
How to tolerance a drawing that machines cheaply
- State ISO 2768-m in the title block. Every uncontrolled dimension now has an agreed home.
- Tighten only what seals, locates, rotates or mates. Each tight feature gets its own number, justified by what it touches.
- Tolerance the fit, not the habit. A 25.00 mm shaft in a bearing needs its tolerance; the bracket face nobody touches does not. Standard fits (H7/g6 and friends) say it cleaner than invented numbers.
- Say what the part does. One sentence of function in the RFQ pack tells the machinist which numbers are real, and makes the DFM review sharper.
- Expect to be queried. A supplier who asks "does this face really need ±0.02?" is saving you money. Ours does it at the DFM review, before the quote, which is the only time the saving is free.
Tolerances also decide inspection: the tighter the number, the more the part must be measured to prove it. Whatever the drawing demands, TrueNorth orders ship with dimensional inspection before dispatch, and the documentation to show it.