What Tolerance Can CNC Machining Actually Hold?

Buyers often send a drawing marked ±0.01 mm on every dimension and expect it to be routine. Sometimes it is. Often it is not — and the difference has little to do with whether the shop owns a “precision” machine.

Tolerance capability is not a single number. It is the result of the machine, the fixture, the tool, the material, the feature geometry, the temperature, and the measurement method, all acting on one specific dimension. Understanding which of those is limiting your part is the difference between a quote you can use and a quote that quietly doubles.

Machine accuracy is not part tolerance

A machining center may position to ±0.005 mm in a temperature-controlled room. That figure describes the machine, not your part. By the time a feature is cut, tolerance has already been consumed by fixture location, tool deflection, spindle growth, material movement after stock removal, and the uncertainty of the measurement used to accept it.

A practical rule: the tolerance on the drawing should be at least three times the combined uncertainty of the process used to verify it. If you cannot measure it reliably, you cannot claim it.

Typical tolerance ranges

The figures below are rules of thumb for common part sizes, feature types, and materials. They assume a competent shop with proper fixturing — not a specific machine or a specific supplier.

Level	Typical tolerance	How it is usually achieved
General machining	±0.10 mm (±0.004″)	Standard 3-axis milling and turning, no special measures
Moderate precision	±0.05 mm (±0.002″)	Rigid setup, sharp tooling, in-process checks
Precision	±0.025 mm (±0.001″)	Controlled finish passes, temperature awareness, CMM verification
High precision	±0.010 mm (±0.0004″)	Dedicated fixturing, small depth of cut, skilled operator, defined inspection
Beyond normal milling	below ±0.010 mm	Grinding, lapping, honing, jig boring — a different process, not a tighter parameter

Note the last row. When a feature needs better than about ±0.01 mm, the answer is usually a second operation on a different machine, not a slower pass on the same one. That is why cost rises steeply at the tight end.

Size changes everything

Aluminum expands roughly 23 µm per metre per degree Celsius. A 500 mm frame that warms by 5 °C during machining grows about 0.06 mm — six times a ±0.01 mm tolerance. On a part that size, temperature control is not a luxury; it is the tolerance.

The same logic applies to geometry. A ±0.01 mm bore on a 20 mm part is a different problem from ±0.01 mm across a 600 mm mounting pattern. Whenever possible, specify tight tolerance on the small, functional feature and let the overall envelope stay general.

GD&T is usually the real cost driver

Linear dimensions are rarely what makes a part expensive. Position, concentricity, perpendicularity, and flatness usually are, because they depend on how the part is held and referenced, not just on how accurately the tool moves.

Two habits make a real difference:

• Use datums. A feature located from a defined datum is inspectable and repeatable. The same feature located by a chain of dimensions accumulates error from every link.
• Do not blanket the drawing. A note saying “all dimensions ±0.01” forces the shop to treat a clearance hole like a bearing seat. It raises cost and tells the shop the drawing was not thought through.

Features that are genuinely difficult

• Thin walls below about 1 mm — deflection and chatter during finishing
• Deep pockets where depth exceeds roughly four times the width — tool reach and chip evacuation
• Small deep holes with a length-to-diameter ratio above five — drill wander and breakage
• Sharp internal corners — a rotating tool always leaves its radius, so a true sharp corner needs EDM
• Interrupted cuts and cross-holes — impact load on the insert, surface finish suffers
• Flexible parts — the part moves away from the tool, so holding size is a fixturing problem

Surface finish is a separate requirement

Ra 3.2 µm is a normal milled finish. Ra 1.6 µm is achievable with careful parameters. Ra 0.8 µm usually means a finishing pass with a small stepover, and Ra 0.4 µm generally means grinding. Tight tolerance and fine finish often travel together, but they are not the same requirement — specify both only where the function needs both.

Specify tolerance without overpaying

• Tighten only the dimensions that affect fit, function, or assembly
• Reference features to datums instead of chaining dimensions
• State the inspection method where acceptance is critical
• Leave clearance holes, covers, and non-mating surfaces at general tolerance
• Ask for a DFM review before the drawing is frozen

A shop that reviews the drawing before quoting will tell you which tolerances are driving the price. A shop that simply quotes the number is guessing — and the guess is usually padded.

Inspection is part of the cost

Holding ±0.01 mm is only half the job; proving it is the other half. First-article inspection on a CMM, gauge setup, and documentation all take time, and 100% inspection on a tight feature can exceed the machining time itself. If your quality plan allows sampling, say so on the drawing — it is often the cheapest saving available.

FAQ

Is ±0.01 mm achievable in CNC machining?
Yes, on specific features, in a controlled setup, with defined inspection. It is not a blanket capability across an entire part, and it is not economical on every dimension.

What is a normal CNC machining tolerance?
Around ±0.1 mm for general work. Most functional features land between ±0.05 and ±0.025 mm. Tighter than ±0.01 mm usually means a secondary process.

Why does tightening tolerance raise cost so sharply?
Because it consumes setup time, slows the cut, increases scrap risk, and requires more inspection. The relationship is not linear — each step tighter removes more of the process margin.