Engineering reference

CNC tolerance chart: metric to inch conversion

Tolerance is the single largest cost driver in a machined part. A drawing that says ±0.05 mm in imperial units confuses factories, and confusion on a drawing becomes scrap on the floor.

A tolerance misread by a factor of 25 does not fail at the quoting stage. It fails at incoming inspection, three weeks later, on parts that are correct to the drawing as the factory read it and wrong to the drawing as you wrote it. In outsourced CNC work this is one of the most avoidable disputes, and it almost always traces back to units rather than machining capability.

Metric to inch tolerance conversion chart

The factor is exact: 1 inch = 25.4 mm. Imperial tolerances are quoted in thousandths of an inch, which is why the metric values below do not round to tidy numbers.

Metric tolerance	Inch equivalent (exact)	Customary callout	Typical interpretation
±0.005 mm	±0.000197 in	±0.0002 in	Grinding or jig boring; not milling
±0.010 mm	±0.000394 in	±0.0004 in	Precision turning or grinding
±0.020 mm	±0.000787 in	±0.0008 in	High-end CNC milling
±0.025 mm	±0.000984 in	±0.001 in	Standard precision CNC work
±0.050 mm	±0.001969 in	±0.002 in	General CNC; the most common callout
±0.075 mm	±0.002953 in	±0.003 in	Comfortable CNC work
±0.100 mm	±0.003937 in	±0.004 in	Loose CNC, fabrication-level fit
±0.125 mm	±0.004921 in	±0.005 in	Rough machining, non-critical
±0.250 mm	±0.009843 in	±0.010 in	Reference geometry only

Read it in reverse too. A drawing that says ±0.001 in is asking for ±0.0254 mm, not ±0.025 mm. Round the quotation, never the requirement.

What IT grades actually mean

ISO 286 defines the IT (International Tolerance) grade system. For a given nominal size, each grade corresponds to a tolerance width that grows with the feature size. IT5 to IT7 cover precision fits and belong to grinding and fine boring. IT8 to IT11 cover the vast majority of machined components. IT12 and looser is reference geometry.

Two facts matter more than the full table. Grades scale with nominal size, so IT7 on a 10 mm diameter is far tighter in absolute terms than IT7 on a 200 mm diameter. And for the sizes most CNC parts fall into, the bands match familiar conventions:

• IT7 is around ±0.015 mm on small features, near ±0.03 mm at 50 mm. Precision work.
• IT8 is roughly ±0.02 mm to ±0.046 mm by size. Routine on a maintained machining centre.
• IT9 is roughly ±0.03 mm to ±0.074 mm. The home of general CNC milling.
• IT11 is roughly ±0.07 mm to ±0.19 mm. Comfortable for any shop.

Treat these as bands, not exact values, because the standard steps by size range. What is reliable is the ordering: each grade is roughly 1.6 times the width of the one below, which is also why tolerance cost is not linear.

What is standard, and what costs more

On a typical 3-axis vertical machining centre, ±0.05 mm is routine and the price does not move. Below that, cost climbs faster than most buyers expect.

Tolerance band	Cost impact	What changes at the shop
±0.10 mm and looser	Baseline	Standard programming and inspection
±0.05 mm	Baseline	Normal practice; caliper check per batch
±0.02 mm to ±0.03 mm	Slight increase	Slower feeds, more finishing passes, CMM checks per part
±0.01 mm to ±0.02 mm	Noticeable increase	Temperature control, in-process gauging, trial-cut scrap
Below ±0.01 mm	Large increase	Grinding or lapping after machining, dedicated fixtures

Geometry is more sensitive than size: flatness or parallelism below about 0.02 mm on a large part usually needs a single-operation set-up to avoid re-fixturing error. Position tolerance on hole patterns is cheap by comparison. Surface finish is priced separately: Ra 3.2 µm is standard, Ra 1.6 µm carries a light premium, and Ra 0.8 µm or finer generally means a finishing pass or an external process.

The most common mistake: ±0.05 mm read as ±0.002 in

The buyer specifies ±0.05 mm because the design is metric. The operator sees a value with three decimals and thinks in imperial, because machine offsets and shop calipers are often set in thousandths. The value is transcribed as ±0.002 in.

Do the arithmetic. ±0.05 mm is ±0.001969 in. ±0.002 in is ±0.0508 mm, about 1.6 percent wider than required. On a part running near nominal that is trivial. But inspection is a bet on worst case, and the part at the extreme of the factory's accepted band falls outside yours.

The error is worse in reverse. A drawing calling ±0.002 in, read by a metric shop as ±0.002 mm, demands a tolerance 25 times tighter than intended. The quote comes back absurd or the parts fail on dimensions the factory believed were perfect. Neither party was careless; the ambiguity was built into the document.

How to specify tolerances so they cannot be misread

1. State the unit in the title block and every general note. "All dimensions in millimetres unless otherwise stated."
2. Suffix every tolerance with its unit. ±0.05 mm is unambiguous. ±0.05 is not, however obvious it seems to the author.
3. Show the conversion in brackets. For example 25.40 ±0.05 mm [1.000 ±0.002 in]. Intent becomes visible without changing the requirement.
4. Never mix units in one general tolerance block. "X.X = ±0.1, X.XX = ±0.02, X.XXX = ±0.002" is a trap: imperial in intent, metric in form.
5. Convert toward tighter, not looser. ±0.002 in is ±0.0508 mm; ask for ±0.05 mm, not ±0.051 mm.
6. Confirm interpretation at PO stage. One line asking the supplier to state inspection units and gauges closes the loop in minutes.

Apply the same discipline to the inspection report: measured values with units, not pass marks, and a reporting resolution finer than the tolerance being verified.

The practical takeaway

Tolerances are requirements, and units are part of the requirement. A chart converts values, but what prevents disputes is a drawing that states units in the title block, suffixes every tolerance, and converts in the tightening direction when one reference serves both metric and imperial readers. The factory machines exactly what it reads, and it cannot read your intent.