Blog / How to choose CNC machining tolerances without overpaying
How to choose CNC machining tolerances without overpaying
Which dimensions actually need ±0.01 mm, and where a general tolerance is good enough
KaiMi Engineering Team · · 7 min read
Tolerance is the single largest cost driver a designer controls. A drawing that specifies ±0.005 mm everywhere can cost 30–60% more than one that reserves tight tolerance for the four features that matter — and it does not perform better. This guide explains how to decide, feature by feature, and how ISO 2768 general tolerances can carry the rest of the drawing.
Start from function, not from habit
Before adding a tolerance, ask what the dimension has to do. A mounting hole that locates a bearing needs a precise position and diameter; a clearance hole for an M6 screw needs about ±0.2 mm and nothing more. A cosmetic edge needs no tolerance at all.
The practical rule: tolerance only the features that touch another part, seal, transmit load, or define an interface. Everything else can rely on the general tolerance block.
What each process can actually hold
These are process capabilities on rigid parts in aluminium or steel, measured with a CMM rated to about ±0.003 mm. Thin walls, long parts, plastics and titanium all move the practical limit.
| Process | Everyday tolerance | Best achievable |
|---|---|---|
| CNC milling (3/4/5-axis) | ±0.01 mm | ±0.005 mm with CMM verification |
| CNC turning | ±0.01 mm | ±0.005 mm on precision fits |
| Surface / cylindrical grinding | ±0.002 mm | ±0.001 mm with tight process control |
| Wire EDM | ±0.002 mm | ±0.001 mm on precision features |
| Die-sinking EDM | ±0.01 mm | ±0.005 mm with electrode correction |
Use ISO 2768-m as your default
If the drawing states ISO 2768-m, every dimension without an individual tolerance follows the medium general-tolerance table: about ±0.1 mm up to 6 mm, ±0.2 mm from 6 to 30 mm, and ±0.3 mm from 30 to 120 mm. That is right for most non-critical features and it is the cheapest option for both of us.
ISO 2768-f (fine) roughly halves those values and adds inspection time. Use it when a whole group of dimensions needs tighter control, rather than tolerancing each one individually.
Where tight tolerance earns its cost
- Bearing seats and shaft fits — a wrong fit is an immediate failure, not a cosmetic issue.
- Sealing surfaces — flatness and roughness drive leak performance more than size.
- Mating interfaces on multi-part assemblies — position tolerance accumulates across parts.
- Sliding and locating features — clearance determines whether the part binds.
- Any dimension that a customer measures on incoming inspection.
How tolerance changes price
The same logic applies to surface finish. Going from Ra 1.6 µm to Ra 0.4 µm usually means an extra operation; going to Ra 0.1 µm means grinding or polishing. If the surface is not sealing or sliding, Ra 3.2 µm is often acceptable.
| Tolerance band | Typical cost effect | Why |
|---|---|---|
| ±0.1 mm and looser | Baseline | Single roughing + finishing pass, sample inspection |
| ±0.02 to ±0.05 mm | +10–20% | Finishing passes, more frequent in-process checks |
| ±0.01 mm | +20–40% | Controlled cutting parameters, coolant, CMM sampling |
| Below ±0.01 mm | +40–100% | Grinding or EDM step, temperature control, 100% inspection |
GD&T: be explicit about datums
Geometric tolerances only work if the datums are defined. A position callout without clear A-B-C datums cannot be measured consistently, and two suppliers will quote different processes to guarantee it.
Keep the datum scheme simple: three planes that the part actually sits on in assembly. Avoid referencing a datum feature that is itself machined late in the process.
A checklist before you send the drawing
- Is every individually toleranced dimension tied to a function?
- Does the title block state a general tolerance (ISO 2768-m is a good default)?
- Are datums defined for every GD&T callout?
- Is the surface finish specified only where it matters?
- Did you mark critical-to-quality features so inspection can focus there?
About the author
KaiMi Engineering Team — 30+ mechanical engineers and quality inspectors at our Dongguan plant, writing about machining capability, tolerances and sourcing for OEM buyers. More about KaiMi.
Frequently asked questions
Is ±0.01 mm a reasonable general tolerance for CNC parts?
Yes for critical features, but not as a blanket tolerance. ±0.01 mm adds 20–40% to machining cost versus ISO 2768-m, so it is better applied to mating and locating features while the rest of the drawing uses the general tolerance block.
Can I get ±0.001 mm from a CNC machine?
Wire EDM reaches ±0.001 mm on precision features and grinding holds ±0.002 mm, but measurement uncertainty matters: our CMM is rated to about ±0.003 mm. For anything below ±0.005 mm we agree the measurement method before production.
Does a tighter tolerance always mean a better part?
No. Tolerances exist to control how parts fit and function. Over-tolerancing increases cost and inspection time without improving performance, and it can force processes that introduce other risks such as heat distortion or surface damage.
Send your drawing for a free quote
Free DFM feedback and a drawing-based quotation within 24 hours. No minimum order quantity.