Tolerances on a machined part, explained for the person buying it
August 4, 2026
Tolerance is the single biggest cost lever on most machined parts and the one buyers control most directly. You do not need to be a machinist to control it well. You need to know what is routine, what is expensive and how to say which features matter.
What shops hold without being asked
These are typical figures on the right machine in reasonable material. They are what to plan with, not promises on your part.
| Feature | Typical | Achievable with care |
|---|---|---|
| Milled linear dimension | ±0.05 mm | ±0.02 mm |
| Turned diameter | ±0.02 mm | ±0.01 mm |
| Reamed hole | ±0.01 mm | ±0.005 mm |
| Ground surface or diameter | ±0.005 mm | ±0.002 mm |
| Flatness over 100 mm | 0.05 mm | 0.01 mm, ground |
| Surface roughness, milled | Ra 1.6 to 3.2 | Ra 0.8 |
Material matters as much as the machine. Aluminium and brass behave. Stainless work hardens and moves. Plastics expand with heat and creep over time, so a ±0.01 mm feature in nylon is not a realistic request regardless of the machine.
General tolerance standards
Rather than tolerancing every dimension, drawings carry a general note and then call out the exceptions. The common standards:
ISO 2768 has classes f (fine), m (medium), c (coarse) and v (very coarse) for linear dimensions, and H, K, L for geometric ones. ISO 2768-mK is a sensible default on general engineering parts.
ASME Y14.5 is the American system, more often used together with a full GD&T scheme rather than as a simple block note.
Pick one, put it in the title block and make sure the drawing does not contradict it.
The blanket tolerance trap
The most expensive line on a drawing is usually a template default that nobody revisited: every dimension at ±0.01 mm because that is what the CAD system inherited from an earlier part.
That single choice forces the shop to:
- Finish every surface slowly rather than only the ones that matter
- Measure every dimension rather than the critical few
- Carry scrap risk on features where nothing would ever have noticed a deviation
The fix takes ten minutes. Set a sensible general tolerance, then call out the two to five features that actually control function: the bore that takes the bearing, the face that seals, the distance between two mounting holes.
How to decide what is critical
Ask what the feature touches.
- Does it mate with another part? Then it needs a real tolerance, and usually a fit rather than a symmetric band.
- Does it seal? Surface finish matters as much as size.
- Does it carry a bearing or a shaft? Roundness and runout matter, not just diameter.
- Is it a clearance feature? A clearance hole for an M6 bolt does not need ±0.05 mm. It needs to be big enough.
- Is it cosmetic? Then specify appearance, not a dimension.
If a feature touches nothing, it does not need a tight tolerance no matter how important the part is.
Fits are clearer than bands
For holes and shafts that go together, a fit designation says what you mean better than a plus and minus. H7/g6 is a sliding fit, H7/k6 a light interference, H7/p6 a press fit. Shops read these instantly and they carry the intent, which a bare ±0.01 mm does not.
If you are unsure which fit, describe the function in the request: “this bore takes a 20 mm bearing outer race, press fit, no rotation in the housing”. A shop that knows the function can pick a fit and tell you what it picked.
Temperature, measurement and honesty
Tolerances tighter than about ±0.01 mm are only meaningful with a stated measurement condition. Metal grows roughly 0.000023 per degree for aluminium, which over a 200 mm part is around 0.005 mm for every degree of difference between your inspection room and theirs.
If your part is at that level, say what temperature the inspection assumes and what instrument you expect to be used. Otherwise you and the shop will measure honestly and disagree.
What to write in a request
Three lines usually cover it:
General tolerance ISO 2768-mK. Critical: bore A 25 H7, parallelism of face B to face C within 0.02 mm, true position of the four M6 holes 0.1 mm to datum A-B. Everything else general.
That is enough for any shop to price the part properly, and it is short enough that nobody skips reading it.
A worked markup
Take a simple aluminium housing. Here is the difference between a drawing that quotes badly and one that quotes well.
Before. Every dimension carries ±0.01 mm because the template said so. Surface finish Ra 0.8 all over. No datums. Result: every shop prices full inspection, a finishing pass on surfaces nobody cares about and a scrap allowance for features that were never functional.
After.
General tolerance ISO 2768-mK. Surface finish Ra 3.2 unless noted. Datum A: mounting face. Datum B: 12 mm dowel hole. Datum C: second dowel hole. Bore D: 25 H7, Ra 1.6. Position of the four M6 holes: 0.2 mm to A, B, C at maximum material condition. Parallelism of face E to datum A: 0.03 mm.
Same part, same function, and typically a double digit percentage off the price. Nothing was loosened that mattered.
Where tolerances get lost
Even a good drawing can be undermined by the process behind it. Three things to ask about on tight work:
- How many setups? Every setup adds a stack between features cut before and after.
- Where is the part measured? A workshop at 33 C measures differently from an air conditioned room.
- When is it measured? Stainless and large aluminium parts move for hours after machining as stress relaxes.
The GD&T basics guide covers the second half of this in more detail, and the DFM checklist shows where tolerance sits among the other cost drivers. When your drawing is marked up, send it for quotes.
Questions we get on this
What is a standard CNC machining tolerance?
Where nothing is called out, most shops work to a general standard such as ISO 2768 medium, which allows roughly ±0.1 to ±0.3 mm depending on the size of the feature. Called-out features are usually held between ±0.05 and ±0.01 mm depending on geometry and material.
Why does a tight tolerance cost so much more?
It changes three things at once: slower finishing passes, more frequent measurement and a higher scrap risk. The last one is the expensive part, because the shop prices the parts it expects to throw away.
Should I put ISO 2768 on my drawing?
Yes, or another general tolerance note. Without it the shop chooses, and what it chooses may be tighter or looser than you expect. One line in the title block removes a whole class of disputes.
Have a part like this?
Send the drawing. We shortlist the shop we place it with that run the process and material, and answer within 24 business hours.
Send a drawing