CNC Machining Tolerances: A Practical Guide to Lower Part Costs
Tightening every dimension does not make a part better, only more expensive. Learn how ISO 2768 general tolerances work, where tight tolerances really matter, and the mistakes that inflate quotes.
Table of contents 11 sections
- What is a tolerance and why does it matter?
- ISO 2768 general tolerances
- When are tight tolerances really needed?
- Fit tolerances (ISO 286)
- Geometric tolerances (GD&T)
- How tolerances affect cost
- Pre-quote checklist
- Frequently asked questions
- What happens if I don’t put tolerances on my drawing?
- Is ±0.01 mm achievable with CNC machining?
- If I send a 3D model, do I still need a drawing?
Applying tight tolerances to every dimension does not make a part better, it only makes it more expensive. This guide explains how general tolerances work, where tight tolerances are genuinely needed and which drawing mistakes quietly inflate your quotes.
In short: For dimensions without a specific tolerance, a general tolerance class (usually ISO 2768-m) is enough. Reserve tight tolerances for fits, bearing seats and sealing surfaces. Every tight tolerance adds machining and inspection time.
What is a tolerance and why does it matter?
No manufacturing process can hit a dimension perfectly. Tool wear, thermal expansion, machine accuracy and measurement uncertainty all cause small variations from part to part. A tolerance defines how much a dimension is allowed to vary: when you write 50 ±0.1 mm, any part between 49.9 and 50.1 mm is acceptable.
A well-chosen tolerance guarantees that the part works. An unnecessarily tight tolerance does not improve the part; it simply makes it slower to machine, longer to inspect and more likely to be rejected.
ISO 2768 general tolerances
Writing a tolerance next to every dimension makes a drawing hard to read and is rarely necessary. Instead, the title block states something like “General tolerances: ISO 2768-m”. Every linear dimension without its own tolerance is then judged against that class. The standard defines four classes: f (fine), m (medium), c (coarse) and v (very coarse).
| Nominal size (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 – 3 | ±0.05 | ±0.1 | ±0.2 | — |
| 3 – 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| 6 – 30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| 30 – 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| 120 – 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| 400 – 1000 | ±0.3 | ±0.8 | ±2 | ±4 |
Class “m” is the most common choice for CNC machining; modern machines hold these values without extra effort. Class “f” suits more precise parts, but applying it as the general tolerance for a whole part can increase cost.
Common mistake: drawings where the CAD default has put ±0.01 mm on every dimension. The manufacturer either has to measure every feature or add a risk margin to the quote. Either way, the price goes up.
When are tight tolerances really needed?
Before tightening a dimension, ask: would the part stop working if this were 0.2 mm off? If not, the general tolerance is enough. Tight tolerances are usually needed on:
- Mating surfaces: bearing seats, shaft–hub connections, pin and bushing holes.
- Sealing surfaces: O-ring grooves and gasket faces.
- Assembly datums: holes and faces that must align with other parts.
- Moving mechanisms: slides, guides and fits where clearance is critical.
Fit tolerances (ISO 286)
For parts that fit together, such as shafts and holes, ISO 286 fit classes are used instead of ± values. Ø20 H7 defines the tolerance zone for a hole and Ø20 g6 for a shaft. The letter sets the position of the zone and the number its width. H7/g6 is a common sliding fit and H7/p6 a common press fit. If you are unsure which fit you need, describe the function in the notes and the manufacturer can suggest one.
Geometric tolerances (GD&T)
Size tolerances control how big a feature is; geometric tolerances control its form and position. Flatness, perpendicularity, parallelism, concentricity and position are typical examples. They are defined relative to datum features.
- Choose the surfaces the part rests on in the assembly as datums (A, B, C).
- Apply geometric tolerances only to features that affect function.
- If inspection requires special equipment (e.g. a CMM), mention it when requesting a quote.
How tolerances affect cost
As tolerances tighten, cost rises exponentially rather than linearly. The main reasons:
- Lower cutting speeds and additional finishing passes are required.
- The part may need to stabilise thermally on the machine.
- Every part must be measured, sometimes with a formal inspection report.
- The share of out-of-tolerance parts increases.
Listing your critical dimensions separately in the quote notes helps the manufacturer understand where to focus and leads to more accurate prices.
Pre-quote checklist
- General tolerance class (e.g. ISO 2768-m) stated in the title block
- Tight tolerances only on functional surfaces
- Fits specified with ISO 286 classes (H7, g6, etc.)
- Datums and geometric tolerances defined
- Surface roughness (Ra) specified where needed
- STEP model and PDF drawing ready together
Frequently asked questions
What happens if I don’t put tolerances on my drawing?
The manufacturer will usually assume their own shop standard or ISO 2768-m. To make your expectations clear, always state the general tolerance class in the title block.
Is ±0.01 mm achievable with CNC machining?
Yes, with suitable machines, tooling, environment and inspection equipment, but it significantly increases machining and inspection time. Request it only on surfaces that functionally need it.
If I send a 3D model, do I still need a drawing?
Yes. A STEP file carries geometry but not tolerances, threads, surface roughness or critical dimensions. Add a PDF drawing for this information.
Upload your STEP model and PDF drawing; manufacturers will review your tolerances and send offers.