A tolerance callout tells the person cutting the part how far a feature can drift before the part stops working. ±0.1mm on a 20mm dimension means anything from 19.9mm to 20.1mm passes inspection. Leave the callout off and the shop applies its own general standard. Mark everything ±0.01mm and you pay for precision on faces that never touch anything. The job is to put the tight number on the two or three features that mate with something, and leave the rest at the shop's default.
What the number promises, and what it doesn't
The callout is not a claim about how good the machine is. Protolabs quotes linear dimensions to the ISO 2768 fine grade and holes to ±0.127mm as standard, and ±0.0127mm on a hole or bore called out on the drawing. Same machines, ten times the precision, because the drawing asked for it. Hubs gives a similar spread for its network: ±0.1mm typical, ±0.02mm feasible, with the caveat that achievable tolerances vary with the base dimension and the geometry of the part.
If a drawing says nothing, the shop still has to pick a number. Both suppliers point to ISO 2768, the general-tolerance standard, and Protolabs names the grades it applies by default: fine for metals, medium for plastics. An unmarked drawing is not untoleranced. It is toleranced by a standard you did not read, to a grade you did not choose.
| Process | Stated tolerance | Where it comes from |
|---|---|---|
| CNC milling, standard hole | ±0.127mm | Protolabs, CNC machining page (linear dimensions go to ISO 2768 fine) |
| CNC milling, hole or bore called out on the drawing | ±0.0127mm | Protolabs, CNC machining page |
| SLA (stereolithography, resin) printing | ±0.05mm | Protolabs, 3D printing page |
| SLS (selective laser sintering, nylon) printing | ±0.254mm | Protolabs, 3D printing page |
| FDM (fused deposition, filament) printing | ±0.5mm | Protolabs, 3D printing page |
These are one supplier's numbers for its own equipment. Your shop or your printer will differ, so ask before you design to them. Protolabs' 3D printing page adds a line worth keeping for any process: design away from minimum limits and leave extra room for variation.
Fits: the part of the callout that gets skipped
A plain ± number says how much a feature can vary. It does not say which way it should lean, and for anything that mates with a shaft or a pin, the direction is the whole point. That is what ISO 286 fit classes are for. The hole gets a letter and a grade, H7 being the common hole basis, and the shaft gets its own, and the pairing names the fit.
| Shaft class | Shaft measures (mm) | What it means in the hand |
|---|---|---|
| g6, sliding fit | 19.980 to 19.993 | Precise, but still slides by hand |
| h6, location clearance | 19.987 to 20.000 | Located accurately, no significant play |
| k6, slight interference | 20.002 to 20.015 | Light interference, may need slight force |
| p6, press fit | 20.022 to 20.035 | Needs pressing or force to assemble |
Read the two ends of that table together. The whole distance from a hand-slide fit to a press fit on a 20mm pin is 0.055mm. FDM printing's published tolerance is ±0.5mm, nine times that spread in each direction. That is why a printed press fit is a matter of trial prints, and a machined one is a matter of writing down the right letter.
Three questions before you tighten a number
- What does this feature touch? A running fit needs clearance and a moderate tolerance. A press fit needs a tighter tolerance on a much smaller target, a few hundredths of a millimetre of interference.
- Does it stack? If four faces each have to land in tolerance for a fifth part to bolt on, the errors add. A tolerance that is fine on one feature can produce an assembly that will not go together.
- Does temperature matter here? Aluminum and PETG both move with heat. A press fit checked on a cold bench can measure differently once the part has sat in direct sun on deck.
When not to tighten it
Chamfers, clearance holes for bolts, outside faces that touch nothing, and pockets that hold wiring do not need a callout beyond the general standard. Tightening them adds a slower pass and an inspection step to features nobody will measure in use.
Do not put a machining tolerance on a printed part. If the supplier's own figure for FDM is ±0.5mm, a ±0.05mm callout on that part is a wish. Print it, measure it, and adjust the model, or read choosing between CNC and 3D printing and move the fit into metal. And do not tolerance a part against a mating piece you have not measured. A boat fitting that matches no catalogue number needs a caliper on it first, or the callout is a guess dressed as a number.
Before you send the drawing
The check I run before a drawing leaves my bench:
- Name the two or three features that mate with something, and tolerance only those.
- Use a fit class, not a bare ± number, on any bore or pin that has a partner.
- Measure the mating part with a caliper before you write the number down.
- Ask the shop what general standard it applies when a feature is unmarked.
- Check whether the process you chose can hold the number at all.
Tolerance describes what the part has to do. Work out which features mate, tolerance those on purpose, and let the general standard cover the rest. If your machined parts drift between runs, the cause is in the setup as much as the callout, and work-holding for a small shop covers the repeatable side of that. On the printer, dimensions move with the first layer and with the filament, so auto bed leveling and wet filament both belong on the checklist before you blame the model.
Checked against Protolabs, Hubs and Simply Bearings source pages on 2026-09-21: Protolabs CNC machining, Protolabs 3D printing, Hubs, how to design parts for CNC machining, Simply Bearings, ISO 286 limits and fits.
