# CNC Machining Tolerances Explained: What Tight Tolerances Cost

Published 2026-06-03 by the Axisform engineering team. URL: https://www.machined-parts-factory.com/blog/cnc-machining-tolerances-cost-guide/

## Key takeaways
- ±0.05 mm is standard CNC capability on most metal parts and usually adds little or no cost.
- ±0.01 mm typically needs light finish passes, reamed or bored holes, thermal control and CMM or gauge inspection.
- ±0.005 mm is realistic only on short, stiff features in stable metals, often with boring, grinding or honing and 100% inspection.
- Use a general tolerance note such as ISO 2768-mK and apply tight tolerances only to features that mate, seal, locate or rotate.
- GD&T position, flatness and runout controls often allow a cheaper part than stacked plus/minus tolerances while keeping function.

A tolerance of ±0.05 mm is standard CNC capability and adds little or no cost on most metal parts; ±0.01 mm usually requires slower finishing passes, temperature-stable conditions and CMM verification; ±0.005 mm typically means grinding, honing or very controlled finish machining plus 100% inspection of that feature. Cost does not rise in a straight line as tolerances tighten — it rises in steps, each time a tighter number forces a different process, a different inspection method or a higher scrap risk. The practical rule: apply tight tolerances only to features that mate, seal, locate or rotate, and let a general tolerance standard such as ISO 2768 cover everything else.

## What does a CNC machining tolerance actually mean?

A tolerance is the total permitted variation of a dimension. A 20.00 mm bore toleranced ±0.01 mm may measure anywhere from 19.99 to 20.01 mm, a tolerance band of 0.02 mm. The band, not the nominal number, is what drives process choice and cost.

Common ways to state a band:

- **Bilateral:** 20.00 ±0.01 mm (variation in both directions).
- **Unilateral:** 20.00 +0.02/0 mm (variation in one direction only, common for holes that must accept a pin).
- **Limit dimensions:** 20.00 / 20.02 mm (the upper and lower limits written directly).

For shafts and holes, ISO 286 fit codes such as H7 or g6 are often clearer than plus/minus values. An H7 hole between 10 and 18 mm, for example, is +0.018/0 mm.

## How much do ±0.05, ±0.01 and ±0.005 mm really cost?

There is no universal price multiplier, because the cost depends on the feature, material, size and quantity. What changes predictably is the work required. The table below shows what each tolerance level usually means on the shop floor for a typical aluminum or steel part.

| Tolerance (on a ~10–50 mm feature) | Typical process | Typical inspection | Cost impact |
|---|---|---|---|
| ±0.1 mm or ISO 2768-m | Standard roughing and finishing | Calipers, sampling | Baseline |
| ±0.05 mm | Standard CNC milling/turning with a finish pass | Calipers, micrometers, sampling | Usually negligible |
| ±0.02 mm | Dedicated finish pass, tool wear compensation | Micrometers, bore gauges, CMM | Moderate increase |
| ±0.01 mm | Light finish cuts, reamed or bored holes, thermal stability, possibly separate setups | CMM or air gauging, high inspection frequency | Significant increase |
| ±0.005 mm | Precision boring, grinding, honing or lapping; controlled temperature | CMM, 100% inspection of the feature | High; process-dependent |

What drives the jumps:

- **Machine time.** Tighter features need lighter cuts, slower feeds and sometimes a spring pass (a repeat pass at the same depth to remove tool deflection).
- **Tooling.** Reamers, fine boring heads and fresh finishing tools replace general-purpose end mills.
- **Thermal effects.** Aluminum expands about 23 µm per meter per °C. A 100 mm aluminum part warming by 5 °C grows roughly 0.012 mm — larger than an entire ±0.005 mm band.
- **Inspection.** Calipers resolve to about 0.01 mm and are not appropriate for verifying ±0.01 mm. Micrometers, bore gauges and CMMs take longer and cost more.
- **Scrap and rework.** The tighter the band, the more parts fall outside it during setup and tool wear.

### Is ±0.005 mm achievable on any material?

Not reliably on every material or feature. Thin-walled aluminum moves when clamping forces are released. Plastics such as POM, nylon and PTFE absorb moisture, creep and expand far more than metals, so ±0.005 mm on a plastic part is rarely meaningful once it leaves the machine. Long, slender features deflect under the tool. Precision down to ±0.005 mm is realistic on short, stiff features in stable metals — a bearing bore in steel, a locating diameter on a turned stainless shaft — not across a whole part.

## What is ISO 2768 and how do you use it?

ISO 2768 is the general tolerance standard most CNC shops worldwide work to. It applies to every dimension on a drawing that has no individual tolerance, so you only call out tolerances on the features that matter.

ISO 2768-1 covers linear and angular dimensions in four classes: **f** (fine), **m** (medium), **c** (coarse) and **v** (very coarse). Its geometric counterpart, ISO 2768-2 (classes H, K, L), covers flatness, straightness, perpendicularity, symmetry and runout. ISO 2768-2 has formally been replaced by ISO 22081, but "ISO 2768-mK" remains the most common title-block note on machined part drawings.

| Nominal length (mm) | f (fine) | m (medium) | c (coarse) |
|---|---|---|---|
| 0.5 – 3 | ±0.05 | ±0.1 | ±0.2 |
| over 3 – 6 | ±0.05 | ±0.1 | ±0.3 |
| over 6 – 30 | ±0.1 | ±0.2 | ±0.5 |
| over 30 – 120 | ±0.15 | ±0.3 | ±0.8 |
| over 120 – 400 | ±0.2 | ±0.5 | ±1.2 |
| over 400 – 1000 | ±0.3 | ±0.8 | ±2.0 |

For most machined parts, **ISO 2768-m** (or -mK with geometry) is the sensible default. Class f is easy for a CNC shop on small parts but adds inspection effort across every dimension. If you want ±0.05 mm everywhere, say so in the title block instead of tightening each dimension individually.

## When should you use GD&T instead of plus/minus tolerances?

Plus/minus tolerances control size. They do not control form, orientation or location very well. Geometric dimensioning and tolerancing (GD&T, defined in ASME Y14.5 and the ISO GPS standards) controls those directly and often allows a looser, cheaper part that still functions.

The controls you will use most often on machined parts:

- **Position** — where a hole or pin sits relative to datums. Position defines a circular zone. A hole that functions within a ±0.025 mm square zone also functions anywhere within the circle that encloses that square (Ø0.071 mm), which is about 57% more area — parts that would fail a plus/minus check pass a position check without affecting fit.
- **Flatness** — for sealing faces and mounting surfaces.
- **Perpendicularity and parallelism** — for faces and bores that must align with each other.
- **Runout and total runout** — for rotating parts: shafts, pulleys, knobs.
- **Profile of a surface** — for complex 3D shapes where coordinate dimensions are awkward.

### How do datums affect cost?

Datums tell the machinist and the inspector how the part is held and measured. Choose datums that reflect how the part is assembled: the mounting face first, then a locating bore or edge. When datums match the functional mounting, the machinist can often finish all critical features in one setup, which is the single most effective way to hold tight positional tolerances at reasonable cost.

### What does MMC mean and why does it save money?

Maximum material condition (MMC, the circled M symbol) allows a position tolerance to grow as a hole gets larger than its smallest size. Clearance holes for bolts rarely need exact positioning when they are oversized, so adding MMC lets more parts pass without affecting assembly.

## How should you call out tolerances on a drawing?

A clear drawing prevents both over-processing and disputes at inspection. A good tolerance callout typically includes:

1. **A general tolerance note** in the title block, for example "Untoleranced dimensions per ISO 2768-mK."
2. **Individual tolerances only on functional features** — fits, sealing faces, bearing seats, locating holes.
3. **Fit codes for shafts and holes** (H7, h6, g6) where parts mate.
4. **GD&T for orientation and location** rather than stacking linear dimensions.
5. **Surface roughness** where it matters (Ra 3.2 µm is standard as-machined; Ra 1.6 or 0.8 µm costs extra passes).
6. **Whether tolerances apply before or after finishing.** Anodizing, plating and powder coating all add thickness. State "dimensions apply after anodize" or specify masking — see our [anodizing guide](/blog/anodizing-guide-machined-aluminum/).
7. **Critical-to-function marks** (for example a "CTF" flag or a balloon list) so the supplier knows which dimensions to report on the inspection sheet.

### Common tolerance mistakes that raise cost

- Copying ±0.01 mm onto every dimension from a template.
- Tolerancing a chamfer, a cosmetic pocket or an outer edge as tightly as a bearing bore.
- Chaining dimensions so tolerances stack, instead of dimensioning from a datum.
- Specifying tight tolerances on plastic parts without considering moisture and temperature.
- Forgetting coating thickness on threads and fits.

## How do tolerances interact with material and part geometry?

The same number is easy on one part and hard on another. A ±0.01 mm diameter on a 10 mm stainless steel turned pin is routine for a capable lathe. The same ±0.01 mm across 300 mm on a thin aluminum plate is difficult, because residual stress in the plate makes it move after material is removed. For large or thin parts, specify flatness and position relative to datums rather than tight linear dimensions, and consider stress-relieved plate stock.

Our [DFM rules for CNC parts](/blog/dfm-rules-reduce-cnc-machining-cost/) cover wall thickness and geometry choices that make tolerances easier to hold.

## How does Axisform handle tolerances?

Our standard machining tolerance is ±0.05 mm, with precision down to ±0.005 mm on critical features depending on material and geometry. Critical dimensions are 100% inspected before shipment, using CMM, height gauges, thread gauges and roughness testers, and inspection reports are available on request. If you are unsure which features really need a tight tolerance, send the drawing through our [contact page](/contact/) and we will flag the ones that drive cost.

## Frequently asked questions

### What is the standard tolerance for CNC machining?

Most CNC shops work to about ±0.1 mm or ISO 2768-m when no tolerance is stated, and ±0.05 mm is a widely achievable standard for metal parts. Tighter tolerances such as ±0.01 mm are possible but should be applied only to functional features.

### Is ISO 2768-f or ISO 2768-m better for CNC parts?

ISO 2768-m is the usual default because it keeps inspection effort reasonable while matching normal CNC capability. ISO 2768-f is appropriate for small precision parts, but applying it to every dimension of a large part adds inspection cost without functional benefit.

### Can CNC machining hold ±0.005 mm?

Yes, on short, stiff features in stable metals, often with boring, reaming, grinding or honing and controlled temperature. It is not realistic across an entire part, on thin walls or on most plastics, so reserve it for bearing seats, precision bores and similar features.

### Do tolerances apply before or after anodizing?

That depends on what the drawing says, which is why you should state it. Anodizing adds thickness, so either specify that dimensions apply after finishing, mask the critical features, or give the machinist a pre-finish dimension.