CNC Machining Tolerances: What ±0.005 mm Really Means

Home / Blog / CNC Machining Tolerances

Tolerance is the number that decides whether a part works — and how much it costs. The same part marked ±0.05 mm and marked ±0.005 mm can differ by two or three times in price, even though the geometry is identical.

This guide explains what ±0.005 mm actually covers on a CNC mill and a CNC lathe, where standard tolerances are good enough, and how to write tolerances on a drawing so every supplier quotes the same thing you intended.

What a tolerance really controls

A tolerance is the allowed range for a dimension. A shaft dimension of Ø20.00 ±0.01 mm can be 19.99 or 20.01 mm. The tolerance says nothing about how round, straight or well-positioned that diameter is — those are separate geometric controls.

It also says nothing about the surface. A part can sit inside ±0.005 mm and still have a torn finish that fails inspection. Dimension, geometry and surface finish are three different conversations, and all three show up on the quote.

The tolerance ranges we work to

On our 3-axis and 4-axis machining centers we hold ±0.005 mm on critical milled features; on the CNC lathes we hold ±0.01 mm on diameters. Those are the tight ends of the range, not the default. The table below shows what is practical for common features — and what changes when a general job becomes a precision job.

Feature	General machining	Precision (tightest)	What sets the limit
Milled profile and pocket walls	±0.05 mm	±0.005 mm	Tool deflection, wall height
Milled hole diameter	±0.05 mm	±0.01 mm	End mill vs. reamer
Hole position	±0.1 mm	±0.01 mm	Fixture and machine repeatability
Turned diameter	±0.05 mm	±0.01 mm	Thermal growth, tool wear
Turned length	±0.1 mm	±0.025 mm	Setup and stop position
Flatness / parallelism	0.02 mm	0.005 mm	Material stress, clamping
Surface finish (Ra)	1.6 µm	0.8 µm	Feed rate, tool, material

Why tighter tolerance costs more

A tighter tolerance is not a machine setting; it is a different process. Four things drive the extra cost:

• More setups and more checking. A ±0.005 mm feature usually means a dedicated setup, a test cut and in-process measurement. That time is in the quote.
• Slower cutting. To hold a tight diameter you take lighter passes and leave material for a finish pass, which adds cycle time.
• Scrap risk. When the window is 10 µm wide, a worn tool or a warm machine can push a part outside it. The supplier prices that risk.
• Inspection time. Tight tolerances need measurement, not a visual check — micrometers, height gauges or a vision system, with a record for each part.

That is why the useful question is not “how tight can you machine?” but “which features actually matter?”

GD&T changes the price more than a ± does

Geometric dimensioning and tolerancing (GD&T) describes relationships between features: how flat a face must be, how far a hole may drift from its true position, how perpendicular a bore is to a shoulder. Two drawings with identical ± dimensions can quote very differently once one adds a position tolerance at maximum material condition.

• Position (⌖) controls hole location relative to datums. A position tolerance of Ø0.05 mm is routine; Ø0.01 mm on a production part needs a controlled process and full inspection.
• Profile (⌓) controls a surface against a basic shape. It is common on contoured pockets and housings, and it is expensive to verify without a CMM or vision system.
• Flatness and parallelism show up on sealing faces and mounting pads, where a few micrometres decide whether a gasket seals.

Good GD&T makes a part easier to make, not harder: it tells the shop which features are functional and which are free. Bad GD&T stacks tight controls on features that do nothing.

Tolerance and surface finish are different specs

A turned surface can be Ra 0.8 µm and still be out of round. A milled floor can be flat within 0.01 mm and still show tool marks. If the part is a seal face or a sliding surface, specify all three: the dimensional tolerance, the geometric control and the Ra value. See how we measure these on the quality control page.

Five features that push the limit

• Deep pockets. Anything deeper than about three times the tool diameter needs a longer, more flexible tool. It deflects, so the wall tapers and the floor is not flat. The fix is usually design, not a tighter tolerance.
• Thin walls. Walls under 1 mm move when they are machined and again when they are clamped. Expect a stress-relief step or a light finish pass — both add cost.
• Small, deep holes. A Ø2 mm hole 20 mm deep is a drilling problem before it is a tolerance problem. Peck drilling or reaming adds operations.
• Threads and concentricity. A thread that must run true to a bore needs one setup, or a fixture that keeps both features aligned. Two setups double the error.
• Large flat faces. Flatness across a 300 mm face depends on the material’s internal stress as much as on the machine. Stress-relieved stock is worth asking for.

How we verify a tight tolerance

Every precision job is checked against the drawing before it ships. On the shop floor that means Mitutoyo micrometers and height gauges for diameters, lengths and step heights; gauge blocks and plug gauges for reference; and a 2.5D vision measuring system (VMS400T, 400 × 300 mm stage, ±0.0015 mm) for hole positions, profiles and features that are hard to reach with a hand tool.

For a first article we record the measured values, not just a pass/fail tick. If you need a dimensional report with the shipment, say so in the RFQ — it is a line item, not a surprise.

How to specify tolerances on a drawing

You do not need to dimension every feature to ±0.005 mm. A practical drawing does three things:

1. Puts a general tolerance in the title block, e.g. ISO 2768-mK, so untoleranced dimensions have a defined default.
2. Calls out only the features that affect fit, function or assembly, with the tightest value that still works.
3. States the finish and any heat treatment or coating, because those change the final size.

If a feature is critical, say why. A note like “seal face — flatness 0.01, Ra 0.8” gets a better part than a blanket ±0.01 mm across the drawing.

Frequently asked questions

What is the standard tolerance for CNC machining?

General machining is usually quoted at ±0.05 mm to ±0.1 mm, or to a title-block standard such as ISO 2768-m. Precision work — what we hold on critical features — is ±0.005 mm for milling and ±0.01 mm for turning. The default should come from the drawing’s title block, not from the shop.

What does ±0.005 mm mean in practice?

It means the feature may sit 5 micrometres above or below the nominal size. For reference, a human hair is roughly 70 µm. Holding that band takes a controlled cut, a stable machine and real measurement — which is why it belongs on critical features, not on every dimension.

Can you machine tighter than ±0.005 mm?

Not as a general milling tolerance. Some features can be brought closer with reaming, grinding or a dedicated process, but that has to be discussed feature by feature before quoting. A drawing that asks for ±0.002 mm everywhere usually signals a mismatch between design intent and process.

Does a tighter tolerance also give a better surface finish?

No. Tolerance controls size and geometry; surface finish controls roughness. A part can be dimensionally perfect and still have a rough finish. Specify the Ra value separately when the surface matters.