Tolerance is not one number a machine can hold. It is a property of a specific feature on a specific part, measured with a specific instrument in a specific room. Stated that way, the question becomes answerable.
The short answer
General milled and turned features: ±0.05 mm. Reamed bores, ground faces and features that get their own operation: ±0.01 mm. Features ground or verified on a CMM under controlled conditions: ±0.005 mm. Surface finish to Ra 0.4 µm on a ground or polished face.
Those three numbers are not a hierarchy of skill. They are three different processes, and the middle and bottom ones exist because the top one cannot reach them. A shop that quotes ±0.005 mm on every dimension on the drawing is either grinding everything, or not being precise about what it promised.
Tolerance by feature
Buyers compare quotes on a single tolerance figure. Suppliers quote on features. This is the table that reconciles the two.
| Feature | Process | Typical tolerance |
|---|---|---|
| Pocket depth | 3-axis milling | ±0.05 mm |
| Pocket wall position | 3-axis milling | ±0.02 mm |
| Contoured surface | 3+2 or 5-axis milling | ±0.01 mm profile |
| Drilled hole | Drilling | ±0.1 mm |
| Reamed bore | Reaming | ±0.01 mm |
| Bore roundness | Reaming or boring | 0.005 mm |
| Turned diameter | CNC turning | ±0.02 mm |
| Ground flat face | Surface grinding | Flatness 0.01 mm |
| Hole position | Milling, from one datum | True position ∅0.02 mm |
| Surface finish | Grinding or polishing | Ra 0.4 µm |
| Feature measured on CMM | Grinding plus CMM | ±0.005 mm |
Size changes the answer
A tolerance is a band, and the band competes with physics. On a small rigid part, ±0.005 mm is a machining question. On a half-metre aluminium frame it is a thermal question: aluminium expands roughly 23 micrometres per metre per degree Celsius, so a two-degree swing between machining and inspection consumes most of the band before a cutter touches anything.
| Part size | Practical floor | Limiting factor |
|---|---|---|
| Under 100 mm | ±0.005 mm | Machine and cutter |
| 100–300 mm | ±0.01 mm | Fixture rigidity |
| 300–600 mm | ±0.02 mm | Thermal growth, fixturing |
| Over 600 mm | ±0.05 mm | Thermal growth dominates |
What widens it
When a feature misses its tolerance, the cause is usually on this list rather than in the control loop.
- Part rigidity. A thin wall deflects under cutting force. Two passes with a light finish cut beat one heavy pass, and no control system can compensate for a part that moves while being cut.
- Fixture and re-clamping. Every re-clamp invites a new error. Features that must be related should be machined in one setup where the geometry allows it.
- Temperature. The part, the machine and the gauge all expand. A part measured hot reads small; a part measured in a cold shop reads large.
- Cutter wear and deflection. A worn end mill cuts oversize; a long, slender cutter deflects into the wall. Tool life monitoring matters more on tight work than on loose work.
- Material stress. Machining releases residual stress in rolled plate, and the part moves after the last cut. Rough, stress-relieve, then finish.
- Measurement itself. Caliper, micrometer, bore gauge and CMM do not agree to the micron. The drawing should say how a critical dimension is verified, because the method is part of the specification.
The question to ask a supplier. Not “what tolerance can you hold”, but “what tolerance will you hold on this feature, and how will you prove it”. The second question produces a process and an instrument; the first produces a marketing number.
How to draw it
Most tolerance arguments are drawing problems, not machining problems.
- One loose general tolerance block, then tight callouts only on functional features. Blanket fine tolerances multiply cost across the whole part.
- Datum features marked explicitly, and critical dimensions referenced to a single datum rather than chained across several.
- Geometric callouts where function demands them: flatness, parallelism, true position, perpendicularity. A plus-or-minus band on a bolt pattern does not control position.
- Surface finish specified per face, with the process implied by the value. Ra 0.4 µm means ground or polished, and the price reflects that.
- Inspection method noted for the critical few — CMM, bore gauge, profilometer — so both sides measure the same way.
- Material condition and grain direction stated where it affects stability, especially on thin plates.
The economical drawing is not the one with the tightest numbers. It is the one where every tight number has a reason, and everything else is left loose enough to be made quickly and checked cheaply.
On these values. The figures above describe what our equipment and inspection setup routinely achieve on typical work, and they are the basis of our quotations. A specific part may do better or worse depending on geometry, material and quantity — which is why the tolerance we commit to is stated per feature in the quotation, not as a shop-wide claim.
What tolerance can CNC machining hold in general?
As a working figure, plus or minus 0.05 mm on a general milled or turned feature, plus or minus 0.01 mm on a reamed bore or ground face, and plus or minus 0.005 mm on a feature that is ground or measured on a CMM under controlled conditions. The number is meaningless without the feature it applies to, which is why a drawing with one global tolerance block invites arguments.
Does a tighter tolerance cost more?
Always. Tightening one dimension from plus or minus 0.05 to 0.01 mm usually adds an operation, a slower pass, a dedicated fixture, or an in-process measurement, and it raises the rejection rate. The economical drawing states a loose general tolerance and tightens only the features that function depends on.
Can you hold plus or minus 0.005 mm on a large part?
It depends on size and on the measurement environment as much as on the machine. A 0.005 mm callout on a small, rigid part measured in a temperature-controlled room is achievable. The same callout on a 500 mm aluminium frame becomes a fight against thermal expansion: aluminium moves roughly 23 micrometres per metre per degree Celsius, so a two-degree shop swing consumes most of the band.
What surface finish comes with a tight tolerance?
They are separate specifications. A dimension can be within 0.01 mm while the face is still Ra 1.6 micrometres, because tolerance controls size and finish controls roughness. Where a seal or a sliding fit needs both, specify both — and expect a grinding or polishing operation in the route.
Ask what we will hold, per feature
Send the drawing and we return the tolerance we commit to on each critical feature, the process that reaches it, and how it is verified.
Request a quote