CNC Machining Tolerances: Standards, Achievable Limits, and How to Specify Them
ISO 2768 classes, GD&T basics, achievable tolerances by process, the tolerance-cost curve, and how parts are measured.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 9 min read
On this page
Why Tolerance Is a Design Decision, Not a Machine Spec
Every machined dimension has variation — the question a drawing answers is how much variation the part can tolerate and still function. CNC machining tolerances sit at the intersection of three things: what the process can hold, what the part actually needs, and what inspection can verify. Get the intersection wrong in either direction and you pay for it — in scrap if too loose, in machining and measurement cost if too tight.
This guide covers the standards (ISO 2768 and GD&T), what each machining process can realistically hold, how tolerance drives cost, and how the numbers get verified. For our shop's default standards and quoting approach, see the tolerances capability page — this article is the deeper engineering reference.
ISO 2768: The Default You Already Have
ISO 2768 is the international general-tolerance standard. When a drawing says "ISO 2768-m" in the title block, every dimension without an explicit tolerance inherits a defined limit — no ambiguity, no phone calls. It has two parts:
- ISO 2768-1 covers linear and angular dimensions, in four classes: f (fine), m (medium), c (coarse), v (very coarse).
- ISO 2768-2 covers geometric tolerances (straightness, flatness, perpendicularity, symmetry, runout) in classes H, K, L.
Typical ISO 2768-1 limits for linear dimensions, medium class:
| Capability | Specification |
|---|---|
| 0.5–6 mm nominal | ±0.1 mm |
| 6–30 mm nominal | ±0.2 mm |
| 30–120 mm nominal | ±0.3 mm |
| 120–400 mm nominal | ±0.5 mm |
| 400–1000 mm nominal | ±0.8 mm |
Most precision machine shops work comfortably at ISO 2768-m or -f as a default. Specifying the class in your title block costs nothing and eliminates the most common source of RFQ confusion. The ASME world equivalent is a title-block note like "UNLESS OTHERWISE SPECIFIED ±0.005 in" — same idea, different habit.
GD&T Basics: Controlling Geometry, Not Just Size
Plus-minus tolerances control size. GD&T (ASME Y14.5 / ISO GPS) controls geometry — where features are and how they relate. The symbols that matter most on machined parts:
- Position (true position) — how far a hole axis may drift from its theoretical location, referenced to datums. A position callout with MMC (maximum material condition) gives you bonus tolerance as the hole gets larger — usually more manufacturable than a tight ± on coordinates.
- Flatness — how much a surface may deviate from a perfect plane, no datum needed. Critical for sealing faces and mounting surfaces.
- Perpendicularity and parallelism — orientation of one feature relative to a datum.
- Runout / concentricity — control of rotational surfaces relative to a datum axis; the turned-part equivalents of position.
- Profile of a surface — the catch-all for contoured 5-axis geometry.
Two rules make GD&T inspectable. First, every geometric callout needs a datum structure — a position tolerance without datums A, B, C is a number nobody can measure. Second, datums should be functional: choose the surfaces the part actually locates on in the assembly, because that is how the CMM will fixture it.
Typical Achievable Tolerances by Process
What each process holds under normal production conditions, and what is achievable with extra care and cost:
| Process | Standard production | Achievable (quoted) |
|---|---|---|
| CNC milling (3-axis) | ±0.005 in (±0.13 mm) | ±0.001 in (±0.025 mm) |
| CNC turning | ±0.005 in (±0.13 mm) | ±0.001 in (±0.025 mm) |
| Drilling (as-drilled) | ±0.005 in (±0.13 mm) | ±0.002 in (±0.05 mm) |
| Reaming | ±0.001 in (±0.025 mm) | ±0.0005 in (±0.013 mm) |
| Boring (precision) | ±0.001 in (±0.025 mm) | ±0.0003 in (±0.008 mm) |
| Surface grinding | ±0.0005 in (±0.013 mm) | ±0.0001 in (±0.003 mm) |
| Wire EDM | ±0.001 in (±0.025 mm) | ±0.0002 in (±0.005 mm) |
Below roughly ±0.0002 in (±0.005 mm), you leave conventional machining territory: grinding, honing, lapping, and temperature-controlled metrology enter the picture. A good shop will route the feature to the right process rather than promise a milling tolerance it cannot repeat.
Process capability also shifts with material (titanium and thin stainless deflect under the tool; plastics creep with temperature and moisture), part size (thermal growth over a 1 m part is not trivial), and feature depth (long tools deflect). These are the reasons "achievable" is quoted per drawing, not guaranteed by a table.
The Tolerance–Cost Relationship
Tolerance cost is a step function, not a line. Each tightening step crosses a process boundary:
- ±0.005 → ±0.002 in: still standard machining, but slower feeds, more tool wear allowance, and in-process checks. Expect a modest premium on the affected features.
- ±0.002 → ±0.001 in: finishing passes, stable fixturing, CMM verification. The feature now carries meaningful machining and inspection time.
- ±0.001 → ±0.0005 in and below: often a different machine, a secondary grinding or honing operation, and controlled measurement conditions. Cost can double per feature.
The cheapest drawing strategy is asymmetric: loose general tolerances in the title block, tight callouts only on functional features. A housing with three tight bores and everything else at ISO 2768-m costs a fraction of the same part with a blanket ±0.002 in — and it machines faster because the shop spends precision only where the drawing asks for it.
When to Tighten, When to Relax
Tighten when the dimension: mates with another part in a stack-up; locates bearings, seals, or precision bores; controls interchangeability across suppliers; or affects safety or regulation. Bearing fits (like an H7 bore for a standard bearing) are the classic case — the fit is the function.
Relax when the dimension: clears other parts; is a cosmetic or external profile; spans a large distance (accumulated error makes long tight dimensions disproportionately expensive); or is on a flexible or thin-walled feature that will not hold the number anyway. If two parts mate, budget the tolerance across both drawings rather than tightening one into grinding territory.
One sentence of application context on the drawing — "sealing face," "bearing seat," "clearance for M8 bolt" — lets a machinist sanity-check your callouts. At IsoCNC, that review is part of every quote.
How Tolerances Get Measured
| Method | Best for | Practical resolution |
|---|---|---|
| Calipers / micrometers | General linear dimensions, production checks | ±0.001 in (±0.025 mm) |
| Pin and plug gauges | Hole sizes, go/no-go verification | Class-dependent, very fast |
| Height gauge / surface plate | Flatness, parallelism, step dimensions | ±0.0005 in (±0.013 mm) |
| Optical comparator | 2D profiles, small turned parts, threads | ±0.0002 in (±0.005 mm) |
| CMM (coordinate measuring machine) | GD&T position, profile, complex datums | ±0.0001 in (±0.003 mm) or better |
The method has to match the callout: you cannot verify a 0.002 in position tolerance with calipers. This is why tight GD&T carries inspection cost — it books CMM programming and measurement time. Every IsoCNC order passes dimensional inspection before shipment, with CMM verification for tight and geometric callouts; the full workflow is on the quality inspection page.
FAQ
What are standard CNC machining tolerances?
Without explicit callouts, most shops hold ±0.005 in (±0.13 mm) or ISO 2768-m as a general standard, with ±0.001 in (±0.025 mm) achievable on specified features. The drawing always governs.
What is ISO 2768-m?
The "medium" class of the international general-tolerance standard. It assigns default limits to every untoleranced dimension — for example ±0.2 mm on features between 6 and 30 mm — so the drawing stays unambiguous without tolerancing every number.
Do tighter tolerances always cost more?
Per feature, yes — tightening crosses process and inspection boundaries. But a drawing with three tight functional dimensions and loose everything-else costs far less than a blanket tight tolerance, and usually machines better too.
How are tight GD&T callouts verified?
On a CMM, fixtured to the drawing's datum structure. Position, profile, and runout callouts require CMM or equivalent metrology — handheld tools cannot resolve them.
Have a Drawing to Check?
Send your STEP file and PDF — DFM review is part of every quote, and if a tolerance is fighting the geometry or the budget, we will tell you before you order.
Need these tolerances held — and proven — on real parts? Our quality inspection workflow covers first article and final dimensional checks against the drawing, and the China CNC machining
Related Resources
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
Passivation of Stainless Steel: Process, Specs, and When Parts Need It
Passivation of stainless steel explained for machined parts: the chemistry, ASTM A967 and AMS 2700 methods, nitric…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Send Your Drawing for a DFM Review
Upload your STEP file and drawing. We'll flag tolerance and manufacturability issues with your quote, typically within 1–2 business days.
Get an Instant Quote →