CNC Machining Aluminum Tolerances: A Practical Guide

If you source aluminum parts, "what tolerance can you hold?" is usually the first question you ask a machine shop — and the answer is often vague. The reality is that aluminum behaves differently from steel, and the tolerance you need is rarely the tolerance you should ask for. Over-specifying is the single most common reason a simple aluminum part arrives with a surprising price tag.

This guide covers how CNC machining tolerances work for aluminum in practice: what a normal shop can hold, which callouts actually drive cost, and how to specify tolerances so your supplier quotes — and delivers — exactly what you need.

Why aluminum behaves differently from steel

Aluminum is roughly one third the density of steel and about three times more thermally conductive. Those properties, not the machine, are what shape a realistic tolerance window.

• Thermal expansion. Aluminum grows by about 23 µm per metre per °C — roughly twice as much as steel. A 300 mm part inspected at 32 °C in an unconditioned workshop is measurably smaller at the 20 °C reference temperature used on most drawings. On long parts or precision bores, that difference can consume the whole tolerance budget.
• Low cutting resistance. Free-cutting alloys such as 6061-T6 machine quickly and take a good finish, but they also let the tool pull thin sections out of position. A 1 mm wall will deflect long before the cutter reaches its limit.
• Built-up edge and burrs. Aluminum tends to weld to the cutting edge and to burr heavily. A 0.05 mm burr is invisible on a drawing and fatal on a mating face, so edge quality belongs in the specification.

General tolerances: what a tolerance block really means

Most drawings carry a general tolerance block such as ISO 2768-m. It applies to every dimension that does not carry its own limit, and it is the cheapest tolerance you can buy — because the shop is free to choose the most economical process that lands inside it.

Nominal size (mm)	ISO 2768-f (fine)	ISO 2768-m (medium)	ISO 2768-c (coarse)
0.5 – 3	±0.05	±0.10	±0.20
over 3 – 6	±0.05	±0.10	±0.30
over 6 – 30	±0.10	±0.20	±0.50
over 30 – 120	±0.15	±0.30	±0.80
over 120 – 400	±0.20	±0.50	±1.20
over 400 – 1000	±0.30	±0.80	±2.00

Two practical points: class m is the sensible default for machined aluminum parts, and CNC machining is usually capable of f at no extra cost on small parts. Anything tighter than ±0.05 mm needs to be justified feature by feature — and it should never be applied to a non-functional dimension such as a chamfer or an outside profile.

What a CNC shop can actually hold in aluminum

The values below are what a well-equipped shop holds routinely, with normal fixturing and a controlled workshop. They are not laboratory best-case numbers — they are what you should expect on a production order.

Feature	Typical achievable tolerance	Notes
General milled profile	±0.05 mm (±0.002")	Down to ±0.025 mm on small, rigid parts
Turned diameter	±0.025 mm (±0.001")	Better on short, well-supported parts
Reamed hole	H7	Standard for dowel and bearing seats
Drilled hole position	±0.10 mm	±0.025 mm if bored on a jig
Flatness (small face)	0.02 mm	Requires a supported setup or face milling
Perpendicularity	0.02 mm per 100 mm	Worsens as part length increases
Surface roughness	Ra 1.6 µm	Ra 0.8 µm with fine finishing passes
Thin wall (<1 mm)	+0.1 / −0 mm	Deflection, not machine accuracy, is the limit

Which callouts actually drive cost

Tolerance cost is not linear. Three things move a quote far more than the rest:

1. Tolerances below ±0.02 mm. These usually force a second operation, in-process temperature control, or a coordinate measuring machine report. Expect a step change in price, not a few percent.
2. Geometric callouts without a datum. Position and profile tolerances that reference a theoretical datum force the shop to build a fixture instead of holding the part in a vice.
3. Surface finish tighter than Ra 0.8 µm. Requires slower passes, a dedicated finishing tool and often a polishing step — and it is easily damaged in handling.

By contrast, a general tolerance of ±0.1 mm, a generous fillet, and a note permitting "edges deburred" all reduce cost while rarely affecting function.

How to specify aluminum tolerances correctly

• Start from a general block (ISO 2768-m is a safe default) and tighten only what the assembly demands.
• Tie every tight tolerance to a function. If you cannot explain why a dimension is ±0.01 mm, it probably should not be.
• Use GD&T for interfaces, and always define datums. Position tolerances with a proper datum reference are cheaper to inspect and easier for the shop to satisfy.
• State the reference temperature (20 °C) and the inspection method for critical dimensions.
• Specify finish and edge condition separately. "Deburr all edges, Ra 1.6 µm on sealing faces" is unambiguous; "good finish" is not.
• Say what happens after machining. Anodizing, powder coating and heat treatment all move dimensions slightly, and the shop needs to know whether tolerances are pre- or post-finish.

Five mistakes buyers make every week

1. Applying one tight tolerance to the whole drawing. A single ±0.01 mm callout in the title block can multiply the price of an otherwise simple part.

2. Omitting datums. Without datums, a position callout is open to interpretation, and you will receive parts that meet the drawing on paper and still do not assemble.

3. Ignoring thermal effects on long parts. Anything over about 300 mm deserves a note on temperature, and sometimes a design margin.

4. Forgetting the finish. A hard anodized bore grows; a powder coated face gains 60–100 µm of thickness. If those surfaces are functional, the tolerance must account for it.

5. Treating a prototype tolerance as a production tolerance. A tolerance that was just achievable in the tool room is often not repeatable at 5,000 pieces. Design for the process you will actually use.

Frequently asked questions

What is the standard tolerance for CNC machined aluminum?
Most shops default to ISO 2768-m — roughly ±0.1 mm on small features and ±0.3 mm between 30 and 120 mm. It is the best value for money on non-critical dimensions.

Can you hold ±0.01 mm in aluminum?
It is possible on small, rigid, well-fixtured features, but it requires temperature control and metrology, and the cost rises sharply. For most aluminum parts, ±0.025 mm is the practical floor for a competitive price.

Does anodizing change the tolerance?
Yes. Type II anodizing adds roughly 5–15 µm per surface and Type III hard anodizing adds 25–50 µm. Specify whether tolerances apply before or after finishing.

Why is my 600 mm aluminum part out of tolerance when it measured fine at the shop?
Almost always thermal. The part was measured warm and inspected cold, or the reverse. Agree a reference temperature and, where it matters, an inspection procedure.

Get aluminum parts quoted against a realistic tolerance

Renjiu Machinery machines aluminum prototypes and production parts to tolerances from general ISO 2768-m down to ±0.01 mm where the function requires it. Send us your drawing and intended use, and we will tell you which tolerances are driving cost — and which you can safely relax.

Explore our CNC machining service, check aluminum and other metal materials, review surface treatment options, or request a quote.

Related Reading

• 6061 vs 7075 Aluminium: Choosing the Right Grade for Machined Parts