CNC Machining Tolerance Guide
How tight is tight enough — and where tolerance specifications start inflating cost without improving the part.
A drawing that marks every dimension ±0.01 mm is not a high-quality drawing. It is an expensive one. Tight tolerances require slower cutting, more stable fixturing, temperature control, finer tooling and more inspection time. Applied to non-functional faces, they add cost without changing how the part performs.
This guide sets out what is realistically achievable by process, how general tolerances work, and how to write a drawing that a supplier can quote accurately on the first pass.
Achievable Tolerances by Process
These are practical production ranges for metal parts, not one-off laboratory results. A feature can be held tighter, but usually with a dedicated process and a measurable price premium.
| Process | Typical tolerance | Tight but feasible | Notes |
|---|---|---|---|
| CNC milling, 3-axis | ±0.05 mm | ±0.01 mm | Depends on feature size, tool reach and thermal stability |
| CNC turning | ±0.02 mm | ±0.005 mm | Diameters are easier to hold than lengths |
| 5-axis machining | ±0.05 mm | ±0.02 mm | Fewer setups reduces datum stack-up |
| Grinding | ±0.01 mm | ±0.002 mm | Used for bearing seats and sealing faces |
| Investment casting (as-cast) | ISO 8062 CT4–CT7 | — | Machining needed for tight features |
| Sheet metal, formed | ±0.2 mm | ±0.1 mm | Bend allowance dominates |
Note the gap between milling and turning. A shaft diameter of ±0.01 mm is routine on a lathe; a deep pocket width of ±0.01 mm on a milling centre is not, because tool deflection and heat build-up scale with depth of cut.
General Tolerances: ISO 2768
Rather than dimensioning every edge, most drawings declare a general tolerance class in the title block — for example ISO 2768-m for medium, ISO 2768-f for fine. Untoleranced linear dimensions then inherit a value based on their size band. This keeps the drawing readable and lets the machinist focus on the few dimensions that actually matter.
If your drawing has no general tolerance note at all, suppliers will either ask for clarification or quietly assume their own standard. That is a common source of a quotation that looks cheap and a first article that does not fit.
Fits: H7/g6, H7/p6 and What They Mean
For a shaft in a bore, the fit is defined by the hole basis letter and number, not by a single ± value. H7/g6 is a sliding clearance fit; H7/k6 is a transition fit; H7/p6 is a press fit. Specifying the fit system is more robust than writing two independent tolerances, because it guarantees the clearance or interference regardless of where each part lands within its own tolerance zone.
GD&T in One Paragraph
Geometric dimensioning controls form and relationship, not just size. A flatness callout on a sealing face, a perpendicularity callout between a bore and a mounting face, or a true position callout on a bolt pattern often matters more than tightening every linear dimension. If your assembly has a mating face, identify it as a datum and relate the critical features to it.
Finishing Changes Dimensions
Anodizing adds roughly 5–25 µm per surface depending on type and thickness; zinc and nickel plating add 5–20 µm; powder coating adds 60–120 µm. On a press-fit bore or a threaded hole, that is enough to matter. State whether dimensions apply before or after finishing, and specify masking for threads and grounding surfaces. Our surface finish guide covers this in detail.
A Practical Drawing Checklist
- Declare a general tolerance class in the title block.
- Mark only functional features with tight tolerances, and say why they are functional.
- Use fit designations for mating shafts and bores.
- Assign datums on mating faces and add GD&T where orientation matters.
- State material grade, heat treatment and hardness if they affect machining.
- State surface finish and whether dimensions are pre- or post-finish.
- State thread standards and any masking requirements.
Our RFQ checklist shows how to package this information into a single request that gets an accurate quote.
Related Questions
Is ±0.01 mm achievable on every feature?
No. It is realistic on turned diameters, ground surfaces and short milled features with controlled setups, but not economical on deep pockets, thin walls or large flat areas. Apply it only where function requires it.
Should I use ISO 2768 or dimension everything?
Use a general tolerance class for non-critical dimensions and explicit tolerances for functional features. This is clearer for the machinist and cheaper to produce.
Do you check tolerances after anodizing or plating?
We machine to the post-finish dimension when the drawing specifies it. State this explicitly, and tell us which threads or faces must be masked.
Ready to source custom metal parts?
Send your drawing or sample. Engineering review and quotation within 24 hours.