CNC Machining Tolerances for Aluminum Parts: What’s Realistic

Realistic CNC machining tolerances for aluminum are ±0.005 in (±0.127 mm) for standard features and ±0.001 in (±0.025 mm) for high-precision features on a well-set-up mill. Tighter is possible on turned diameters and reamed holes, but temperature, part size, thin walls, and anodizing decide what you can actually hold and inspect.

Quick answer: Use ±0.005 in as your default and a general tolerance note such as ISO 2768-m for everything else. Apply ±0.001 in only to fits, bores, and sealing faces. Remember that aluminum grows about 23 µm per meter for every 1 °C, and that anodizing adds material to every surface, including bores and threads.

What Does a Machining Tolerance Mean?

A tolerance is the amount a dimension is allowed to vary from its nominal size. A 20.000 mm hole with ±0.025 mm is acceptable anywhere from 19.975 to 20.025 mm.

Drawings use three kinds:

• Dimensional tolerances: limits on sizes and distances, written as ±, as limits, or as an ISO fit such as H7.
• General tolerances: one note in the title block that covers every dimension without its own tolerance.
• Geometric tolerances: GD&T controls for flatness, position, perpendicularity, and similar features. The US standard is ASME Y14.5.

A tolerance is not the same as a machine’s accuracy, and that difference matters when judging realistic tolerances for aluminum parts. A machine that positions to a few microns still produces parts that vary with tool wear, heat, clamping, and material movement.

Realistic Tolerances for Aluminum Parts

These are the aluminum machining tolerances Tuowei publishes for CNC milled parts. They reflect what a production shop can hold repeatably, not a one-off best case.

Feature type	Realistic tolerance
Standard machined features	±0.005 in (±0.127 mm)
High-precision features	±0.001 in (±0.025 mm)
Small components	±0.002 in (±0.051 mm)
Large components	±0.010 in (±0.254 mm)
Threaded features	±0.005 in (±0.127 mm)

Turned diameters and reamed or bored holes can usually go tighter than milled features, because the process controls a single axis of size. Long parts and large plates go the other way. The bigger the part, the more heat and internal stress move it.

Our position: if you do not know what tolerance a feature needs, it probably needs the standard one. Tight tolerances belong on features that locate, seal, or carry a bearing.

Tolerances for Common Aluminum Features

Different features need different tolerances on aluminum parts. A practical starting point:

Feature	Common callout	Why
Bearing bore	H7 fit	Controls the fit with a standard bearing
Dowel pin hole	H7, reamed	Locates mating parts repeatably
Clearance hole for a bolt	Loose, general tolerance	Only needs to let the bolt pass
Tapped hole	Thread class 6H (metric) or 2B (inch)	Standard thread gauges check it
O-ring groove	Tight on depth, looser on width	Depth controls the seal squeeze
Cosmetic outer faces	General tolerance	Appearance, not fit, matters

Most aluminum machining tolerances on a drawing should fall in the loose rows. If more than a handful of features sit in the tight rows, review whether each one really locates, seals, or carries load.

What Is ISO 2768, and Which Class Should You Use?

ISO 2768-1 sets general tolerances for linear dimensions that have no individual tolerance on the drawing. You pick a class and write it once, for example “General tolerances ISO 2768-m.”

Nominal size (mm)	Fine (f)	Medium (m)
0.5 to 3	±0.05	±0.1
Over 3 to 6	±0.05	±0.1
Over 6 to 30	±0.1	±0.2
Over 30 to 120	±0.15	±0.3
Over 120 to 400	±0.2	±0.5
Over 400 to 1000	±0.3	±0.8

For most aluminum parts, ISO 2768-m is the right general class for untoleranced aluminum machining tolerances. It is loose enough to machine quickly and tight enough for non-critical features. Use ISO 2768-f only when the whole part needs to be accurate, such as a precision fixture, because it tightens every untoleranced dimension at once.

A general tolerance is not a capability statement. It is a default. Critical features still need their own tolerance.

Why Temperature Matters More With Aluminum

Aluminum expands roughly twice as much as steel for the same temperature change, at about 23 µm per meter per °C, so temperature eats into aluminum tolerances quickly. That sounds small until you run the numbers:

• A 200 mm part that warms by 5 °C grows about 0.023 mm. That is almost the entire ±0.025 mm high-precision band.
• A 400 mm plate that cools by 10 °C shrinks about 0.092 mm.

This is why dimensions are defined at a reference temperature. ISO 1 sets the standard reference temperature for dimensional specification at 20 °C. A part measured warm, straight off the machine, can pass at the mill and fail in a cool inspection room.

In practice, tight-tolerance aluminum parts are allowed to cool to room temperature before final passes and before measurement, and they are checked in a temperature-controlled room.

Which Alloys Hold Tolerances on Aluminum Parts Best?

The alloy and temper change how easily a shop can hold tolerances on aluminum parts, even before the drawing does.

Alloy and temper	How it behaves	Tolerance tip
6061-T651	Stress-relieved, stable, cuts cleanly	The safest default for tight features
7075-T651	Harder, cuts crisply, less smearing	Holds fine features well, costs more
2024-T351	Machines well, stable	Coat it; corrosion can affect fits over time
5052	Soft and gummy, burrs heavily	Avoid tight tolerances on machined 5052
MIC6 cast plate	Very flat and stable after machining	Best choice when flatness is the critical tolerance

If a part has a tight flatness or position callout and the stock is plain T6 or an extrusion, expect movement after roughing. Switching to T651 plate or MIC6 is often cheaper than fighting the distortion with extra operations.

What Makes Aluminum Parts Drift Out of Tolerance?

Most problems holding aluminum tolerances come from five sources.

1. Heat from cutting. Heavy roughing warms the part. Finishing it hot and measuring it cold shifts every dimension.
2. Internal stress in the stock. Removing a lot of material releases stress, and the part bows. Stress-relieved plate such as 6061-T651 moves far less than plain T6.
3. Thin walls. A thin wall deflects under cutting force, then springs back. The wall measures thicker than programmed, and flatness suffers.
4. Clamping. Aluminum is soft. Clamp too hard and the part distorts while held, then relaxes when released.
5. Tool wear and deflection. Long, thin tools bend. Worn tools push instead of cut.

The usual fixes are symmetrical roughing, leaving a finishing allowance, releasing and re-clamping lightly before final passes, and keeping walls as thick as the design allows.

How Does Anodizing Change Your Tolerances?

Anodizing converts the aluminum surface into oxide. Part of the coating grows into the metal and part builds outward. The outward part changes your dimensions.

For tolerances on aluminum parts, the effect doubles on features you measure across. A bore shrinks by twice the outward buildup, because both walls grow. External diameters get bigger by the same amount. Threads can tighten enough that a screw will not start.

Hard anodizing (Type III) is much thicker than decorative Type II, so it has a bigger effect on tight features. Three ways to handle the anodizing allowance:

• Mask bores, threads, and press-fit features so they stay bare.
• Machine undersize or oversize to allow for the coating, based on the thickness your finisher actually runs.
• State on the drawing whether each tolerance applies before or after anodizing.

Ask your supplier for their typical coating thickness on the alloy you are using, and build that anodizing allowance into the design. Guessing is how anodized parts stop fitting. Tuowei’s Type II anodizing page describes the standard finish.

Tolerance Stack-Up: Where Good Parts Make a Bad Assembly

Every part can pass inspection and the assembly can still fail. That is tolerance stack-up.

Stack-ups are where individual tolerances for aluminum parts add together. Take three machined spacers stacked in a housing, each 10.00 mm ±0.05 mm.

Method	Total variation of the stack	When to use it
Worst case	±0.15 mm (0.05 + 0.05 + 0.05)	Safety-critical fits, low volumes
Statistical (root sum square)	about ±0.087 mm (0.05 × √3)	High volumes where extremes rarely combine

If the housing only allows ±0.10 mm, the worst case says the design can fail even though every spacer is in tolerance. The fix is usually not tighter tolerances on every part. It is tightening one part, or adding an adjustment feature such as a shim or a slot.

Run a quick tolerance stack-up on any chain of three or more parts before you release the drawing.

How Tight Tolerances Affect Cost

Tight tolerance machining costs more for several reasons at once, and aluminum tolerances are no exception:

• Slower feeds and more finishing passes.
• More frequent tool changes to avoid wear.
• Extra steps to control heat and stress, such as rough, rest, and finish.
• Longer inspection, often on a CMM (coordinate measuring machine).
• Higher scrap risk.

The cost does not rise in a straight line. Moving from standard to high precision on one feature is manageable. Moving the whole part to high precision can multiply the price. That is why the cheapest improvement on most drawings is removing tight tolerances that do not do anything.

Can the Tolerance Actually Be Measured?

A tolerance is only real if it can be checked. As a common shop rule of thumb, the measuring tool should be about ten times more precise than the tolerance it checks.

Tolerance	Typical measuring method
±0.005 in (±0.127 mm)	Calipers, height gauge
±0.001 in (±0.025 mm)	Micrometers, bore gauges, pin gauges
Position, flatness, profile	CMM
Thread fit	Go/no-go thread gauges

For a new part, ask for a first article inspection report so the aluminum tolerances on your drawing are verified, not assumed. It should list measured values for every dimension, not just pass or fail. Tuowei outlines its approach on the quality assurance page.

When your incoming inspection disagrees with the supplier’s report, the cause is usually one of three things: a different temperature, a different datum setup, or a different measuring method. Agree on all three before production.

Questions to Ask a Supplier About Aluminum Machining Tolerances

A quote that says “tolerances to ±0.0002 in” tells you what a machine can do on a good day, not what your part will measure. Before placing an order that depends on tight tolerance machining, ask:

1. Which features will you inspect, and with what? You want the method for each critical feature, not a general promise.
2. At what temperature do you measure? The answer should be a controlled room near 20 °C.
3. Will I get a first article inspection report with measured values? A first article inspection with real numbers is the only proof a new part is right.
4. Which datums will you measure from? They should match the datums on your drawing.
5. What anodizing allowance do you plan for? They should know their finisher’s typical coating thickness.

A supplier who answers these clearly is more trustworthy than one quoting the tightest number.

How to Write Tolerances on Your Drawing

A clear drawing gets you realistic quotes and fewer rejections:

1. Add a general tolerance note, such as ISO 2768-m, so untoleranced dimensions are defined.
2. Tolerance only the critical features individually, and mark them for inspection.
3. Use GD&T for relationships, such as hole position to a datum, instead of tight ± tolerances on every coordinate.
4. Call out alloy and temper, for example 6061-T651 plate, because it affects stability.
5. State anodize type and whether dimensions apply before or after finishing.
6. Use standard fits like H7 for bearing and dowel holes, so any shop reads them the same way.

Frequently Asked Questions

What is the standard tolerance for CNC machined aluminum?

A standard tolerance of ±0.005 in (±0.127 mm) is typical for machined aluminum features. Many drawings pair it with a general tolerance note such as ISO 2768-m for untoleranced dimensions. Tighter tolerances are available for critical features but cost more because they need slower cutting and more inspection.

Can CNC machining hold ±0.001 in on aluminum?

Yes, on suitable features. A well-set-up mill can hold ±0.001 in (±0.025 mm) on bores, fits, and sealing faces. It becomes harder on large parts, thin walls, or after anodizing, because heat, stress, and coating growth move the dimension. Apply it only where the function needs it.

Should I use ISO 2768-m or ISO 2768-f for aluminum parts?

Use ISO 2768-m for most aluminum parts. It suits general features and keeps machining fast. Choose ISO 2768-f only when the entire part must be accurate, such as a precision fixture, because it tightens every untoleranced dimension. Critical features should still carry their own individual tolerances.

Does anodizing affect tolerances?

Yes. Anodizing adds a coating that partly builds outward, so bores get smaller, outside diameters get larger, and threads can tighten. Hard anodizing has a bigger effect than Type II. Mask critical features, machine to allow for the coating, or state whether dimensions apply before or after anodizing.

Why do thin aluminum walls go out of tolerance?

Thin walls deflect under cutting forces and spring back after the tool passes, so they measure thicker than programmed. Stress released from the stock and clamping pressure add distortion. Thicker walls, stress-relieved T651 plate, lighter clamping, and symmetrical roughing all help thin features hold tolerance.

Setting Realistic CNC Machining Tolerances for Aluminum

Good CNC machining tolerances for aluminum start with a default that is easy to hold, then add precision only where the part needs it. Plan for temperature, stress, and anodizing, check your stack-ups, and agree with your supplier on how each critical feature will be measured.

Tuowei Precision works to these tolerances on its CNC milling, CNC turning, and precision machining lines. Every drawing gets a DFM (design for manufacturing) review before cutting starts. Send your drawing through the Tuowei Precision homepage and our engineers will flag any tolerance that adds cost without adding function.