CNC Machining Tolerance Chart & GD&T Reference

Why Tolerances Decide Your Quote

Here's the thing most drawings get wrong: a designer marks ±0.01mm on every dimension "to be safe," and the quote comes back three times higher than expected. Then the buyer asks us to cut the price, and we have to explain that the drawing is asking for something the part does not functionally need.

Tolerance is the single biggest lever on machining cost — bigger than material choice in most cases. This page gives you the numbers to make that call yourself.

We machine to ISO 2768-mH by default. Anything tighter needs to be called out explicitly on the drawing, and anything tighter than ±0.01mm needs a conversation before we quote.

Table 1

ISO 2768 Linear Tolerances (mm)

Deviation allowed on linear dimensions, by nominal size range. This is the table to check when a drawing says "ISO 2768-m" with no other callout.

Nominal size (mm)	f (fine)	m (medium)	c (coarse)	v (very coarse)
0.5 – 3	±0.05	±0.1	±0.2	—
over 3 – 6	±0.05	±0.1	±0.3	±0.5
over 6 – 30	±0.1	±0.2	±0.5	±1.0
over 30 – 120	±0.15	±0.3	±0.8	±1.5
over 120 – 400	±0.2	±0.5	±1.2	±2.5
over 400 – 1000	±0.3	±0.8	±2.0	±4.0
over 1000 – 2000	±0.5	±1.2	±3.0	±6.0
over 2000 – 4000	—	±2.0	±4.0	±8.0

Source: ISO 2768-1:1989. For nominal sizes below 0.5mm, tolerances shall be indicated directly on the drawing.

Table 2

ISO 2768 Geometric Tolerances (Part 2)

The "H", "K" and "L" suffix in a callout like ISO 2768-mH refers to these classes for form and position — not the same as the linear table above.

Tolerance type	H	K	L
Straightness & flatness	0.1	0.2	0.4
Perpendicularity (per 100mm)	0.2	0.4	0.6
Symmetry	0.5	0.6	0.6
Circular runout	0.1	0.2	0.5
Cylindricity	Not covered by ISO 2768-2	—	—
Concentricity	Not covered by ISO 2768-2	—	—

Values in mm. Note: cylindricity, concentricity, profile and angularity are NOT covered by ISO 2768-2 — they must be explicitly toleranced on the drawing or the shop has no defined requirement.

Table 3

What Each Process Can Actually Hold

Realistic, repeatable tolerances on a production run — not laboratory best-case numbers.

Process	Standard	Achievable with effort	Surface Ra typical	Cost multiplier
3-axis CNC milling	±0.05mm	±0.01mm	Ra 1.6 μm	1.0×
5-axis CNC milling	±0.05mm	±0.01mm (better on compound angles)	Ra 0.8 μm	1.8×
CNC turning	±0.05mm	±0.01mm on diameter	Ra 0.8 μm	1.0×
Turning + grinding	±0.01mm	±0.002mm	Ra 0.4 μm	2.5×
Wire EDM	±0.01mm	±0.005mm	Ra 0.4 μm	2.0×
Jig boring	±0.005mm	±0.002mm	Ra 0.8 μm	3.0×
Surface grinding	±0.01mm	±0.002mm flatness	Ra 0.2 μm	2.2×

Cost multiplier is relative to standard 3-axis milling on the same part geometry. "Achievable with effort" assumes climate-controlled inspection, sharp tooling and in-process measurement.

Table 4

GD&T Symbol Quick Reference

Category	Symbol name	What it controls	Needs a datum?
Form	Straightness ⏤	How straight a line element is	No
	Flatness ▱	How flat a surface is	No
	Circularity ○	Roundness of a cross-section	No
	Cylindricity ⌭	Combined roundness + straightness of a cylinder	No
Profile	Profile of a line ⌒	Deviation of a cross-section from true profile	Sometimes
Profile	Profile of a surface ⌓	Deviation of a 3D surface from true profile	Sometimes
Orientation	Angularity ∠	Angle of a feature relative to a datum	Yes
	Perpendicularity ⟂	90° relationship to a datum	Yes
	Parallelism ∥	Equal distance from a datum	Yes
Location	Position ⌖	Where a feature sits relative to datums	Yes
	Concentricity ◎	Coaxiality of median points (rarely used — prefer runout)	Yes
	Symmetry ⌯	Mid-plane alignment to a datum	Yes
Runout	Circular runout ↗	Variation at any single cross-section	Yes
Runout	Total runout ⌰	Variation across the entire surface	Yes

Datum = a reference feature the tolerance is measured from. Symbols render differently across fonts; your drawing software will generate the correct glyphs per ASME Y14.5 or ISO 1101.

The Cost Curve

What Tightening Tolerance Actually Costs

This is the table we wish every designer saw before marking a drawing:

Tolerance band	What changes on the shop floor	Typical cost vs. ±0.1mm
±0.1mm	Standard speeds, single pass, no special inspection	1.0× (baseline)
±0.05mm	Slightly slower finishing pass, standard CMM check	1.1 – 1.2×
±0.025mm	Dedicated finishing tool, two-stage roughing/finishing, 100% inspection	1.5 – 2.0×
±0.01mm	Climate-controlled inspection, sharp tooling changed early, in-process measurement, higher scrap	2.0 – 3.0×
±0.005mm and tighter	Grinding, lapping or jig boring — different process entirely	3.0 – 5.0×

The rule we give our own customers

Tolerance the fit, not the part. A bore that receives a bearing gets ±0.01mm. The mounting face 40mm away gets ±0.1mm. The outer profile gets ISO 2768-m default. When a drawing marks every dimension at ±0.01mm, nobody knows which three features actually matter — and the shop has to assume all of them do.

One more trap: tolerance stack-up. If five parts each at ±0.05mm assemble in a chain, the worst-case assembly deviation is ±0.25mm, not ±0.05mm. If your assembly has a functional gap requirement, do the stack-up before finalizing individual part tolerances — not after the parts arrive.

FAQ

Tolerance Questions We Answer Every Week

What is ISO 2768-mH?

ISO 2768-mH is the default general tolerance standard for machined parts. The "m" (medium) sets linear dimension tolerances — for example ±0.5mm at 100mm nominal — and the "H" sets geometric tolerances for flatness, perpendicularity and symmetry. If a drawing says only "ISO 2768-mH" with no other tolerances, this is what the shop must hold.

What tolerance can CNC machining actually hold?

Standard CNC milling and turning holds ±0.05mm (ISO 2768-m) without special effort. ±0.01mm is achievable on features under 50mm with sharp tooling, proper fixturing and in-process measurement — and costs more. Below ±0.005mm you are in grinding or jig-boring territory, not conventional CNC.

Does tighter tolerance always cost more?

Yes, and the curve is steep. Going from ±0.1mm to ±0.05mm might add 10–20% to machining cost. Going from ±0.05mm to ±0.01mm typically adds 50–150%, because it requires slower passes, more measurement steps, climate-controlled inspection and higher scrap rates. Specify tight tolerances only on features that functionally need them.

What is the difference between ISO 2768-f, -m, -c and -v?

These are the four ISO 2768 tolerance classes: f (fine), m (medium), c (coarse), v (very coarse). Each defines progressively looser allowable deviation on linear dimensions, external radii and chamfer heights. "m" is the industry default for machined parts; "f" costs more; "c" and "v" are for sheet metal and rough fabrication.

What is the standard surface finish for CNC machined parts?

As-machined CNC typically gives Ra 1.6 μm (63 μin) for milling and Ra 0.8 μm (32 μin) for turning. Ra 0.4 μm is achievable with a fine finishing pass and sharp tooling. Anything smoother requires polishing or grinding as a separate operation.

Should I use GD&T or plus/minus tolerancing?

GD&T communicates function more precisely and usually permits looser (cheaper) tolerances on non-critical features. Use GD&T when a part has datum-dependent relationships — mating faces, bearing bores, bolt patterns. Plain ± tolerancing is fine for simple, non-assembly parts. If your supplier is in a different country, GD&T removes interpretation ambiguity.

Not Sure?

Send the Drawing — We'll Flag the Expensive Tolerances

When you send us a drawing, our quoting engineer reviews every tolerance callout and tells you which ones are driving cost without adding function. That review is free and comes back with the quote — usually within 24 hours.

Upload Drawings & Get Quote Aluminum Grade Chart