ISO 2768 & IT Grades

The standard system for specifying general tolerances on drawings without tolerancing every dimension individually. Covers linear dimensions, angular dimensions, and geometrical tolerances in four precision classes.

When to Use ISO 2768?

Use ISO 2768 When	Do NOT Use ISO 2768 When
Dimensions have no functional fit requirement	Mating parts require specific clearance or interference fits
Non-critical cosmetic or structural dimensions	Bearing bores, shaft seats, seal grooves
Simplifying drawings — avoid tolerancing every feature	Critical alignment or positioning features
Sheet metal, weldments, structural assemblies	Features that interface with purchased components (bearings, O-rings, gears)
Prototypes where functional tolerances are still being refined	Tolerances tighter than the finest ISO 2768 class provide

How to Specify on a Drawing Write ISO 2768-mK in the title block. The letter before the hyphen = linear class (f/m/c/v). The letter after the hyphen = geometrical class (H/K/L). If no letter after the hyphen, no geometrical tolerances are specified by this standard.

ISO 2768 Class Selection

Class	Precision Level	Typical Use	Cost Impact
f (fine)	Highest general	Precision parts, mating surfaces not requiring specific fit, tight cosmetic requirements	+15–30% vs medium
m (medium)	Standard CNC	General CNC machined parts. Most widely used class. Suitable for the majority of machined components.	Baseline
c (coarse)	Relaxed	Sheet metal parts, structural weldments, non-critical castings, large assemblies	-10–20% vs medium
v (very coarse)	Most relaxed	Welded structures, rough castings, non-precision fabricated parts, very large dimensions	-20–35% vs medium

Default to ISO 2768-m Unless you have a specific reason to go finer or coarser, ISO 2768-m is the standard choice for CNC machined parts. It matches what a typical 3-axis machining center achieves in a single setup without special measures. Going finer requires smaller tools, more passes, or grinding. Going coarser only makes sense for large structural parts.

ISO 2768-1: Linear Tolerances (mm)

Permissible deviations for linear dimensions. Tolerances apply to all dimensions on the drawing that do not carry individual tolerance indications.

Nominal Size Range (mm)	ISO 2768-f	ISO 2768-m	ISO 2768-c	ISO 2768-v
0.5 – 3	±0.05	±0.1	±0.2	—
3 – 6	±0.05	±0.1	±0.3	±0.5
6 – 30	±0.1	±0.2	±0.5	±1.0
30 – 120	±0.15	±0.3	±0.8	±1.5
120 – 400	±0.2	±0.5	±1.2	±2.5
400 – 1000	±0.3	±0.8	±2.0	±4.0
1000 – 2000	±0.5	±1.2	±3.0	±6.0
2000 – 4000	—	±2.0	±4.0	±8.0

External Radii and Chamfers (mm)

Nominal Size Range (mm)	ISO 2768-f	ISO 2768-m	ISO 2768-c	ISO 2768-v
0.5 – 3	±0.2	±0.2	±0.4	±0.4
3 – 6	±0.5	±0.5	±1.0	±1.0
6 – 30	±0.5	±1.0	±1.0	±2.0
30 – 120	±1.0	±1.5	±2.0	±4.0
120 – 400	±2.0	±2.5	±4.0	±8.0

Angular Tolerances (excluding right angles)

Shorter Side Length (mm)	ISO 2768-f	ISO 2768-m	ISO 2768-c	ISO 2768-v
≤ 10	±1°	±1°	±1°30′	±3°
10 – 50	±0°30′	±0°30′	±1°	±2°
50 – 120	±0°20′	±0°20′	±0°30′	±1°
120 – 400	±0°10′	±0°10′	±0°15′	±0°30′
> 400	±0°5′	±0°5′	±0°10′	±0°20′

ISO 2768-2: Geometrical Tolerances

General geometrical tolerances for features without individual GD&T callouts. Three classes: H (normal), K (medium), L (coarse). Specified separately from linear classes — e.g., ISO 2768-mK means linear class m + geometrical class K.

Straightness and Flatness

Nominal Length Range (mm)	Class H	Class K	Class L
≤ 10	0.02	0.05	0.1
10 – 30	0.03	0.1	0.2
30 – 100	0.05	0.15	0.3
100 – 300	0.1	0.3	0.6
300 – 1000	0.2	0.5	1.0
1000 – 3000	0.3	0.8	1.5

Values in mm. Select the row based on the longer of the two sides for flatness.

Perpendicularity

Shorter Side Length (mm)	Class H	Class K	Class L
≤ 10	0.2	0.4	0.6
10 – 30	0.3	0.6	1.0
30 – 100	0.4	0.8	1.5
100 – 300	0.5	1.0	2.0
300 – 1000	0.7	1.5	3.0

Symmetry

Nominal Length Range (mm)	Class H	Class K	Class L
≤ 10	0.5	0.6	0.6
10 – 30	0.5	0.6	1.0
30 – 100	0.5	0.8	1.5
100 – 300	0.5	1.0	2.0
300 – 1000	0.5	1.5	3.0

Runout

Nominal Diameter Range (mm)	Class H	Class K	Class L
≤ 1	0.1	0.2	0.5
1 – 6	0.1	0.3	0.6
6 – 18	0.12	0.4	0.8
18 – 50	0.15	0.5	1.0
50 – 120	0.2	0.6	1.2
120 – 250	0.25	0.8	1.5
250 – 500	0.3	1.0	2.0
500 – 1000	0.4	1.2	2.5

IT Grade Reference

ISO 286 defines 20 standard tolerance grades (IT01 through IT18). Lower number = tighter tolerance. The tolerance value depends on the nominal dimension — larger dimensions get wider absolute tolerances for the same IT grade. Values below are in micrometers (μm).

IT Grade	Practical Meaning	1–3mm	6–10mm	18–30mm	50–80mm	120–180mm	250–315mm
IT01	Gauge block reference	0.3	0.4	0.6	0.8	1.0	1.2
IT0	Reference standard	0.5	0.6	0.9	1.2	1.5	2.0
IT1	Precision gauge	0.8	1.0	1.5	2.0	2.5	3.0
IT2	High-precision gauge	1.2	1.5	2.5	3.0	4.0	5.0
IT3	Ultra-precision work	2.0	2.5	4.0	5.0	6.0	8.0
IT4	Precision grinding / wire EDM	3	4	6	8	10	13
IT5	Gauge manufacturing	4	6	9	13	16	20
IT6	Precision machining	6	9	13	19	25	32
IT7	Precision fit (bearings, shafts)	10	15	21	30	40	52
IT8	General precision machining	14	22	33	46	63	81
IT9	General machining (ISO 2768-m equivalent)	25	36	52	74	100	130
IT10	Medium precision	40	58	84	120	160	210
IT11	Loose machining	60	90	130	190	250	320
IT12	Coarse (ISO 2768-c equivalent)	100	150	210	300	400	520
IT13	Sheet metal, cold forming	140	220	330	460	630	810
IT14	Stamping, die casting	250	360	520	740	1000	1300
IT15	Sand casting, general fab	400	580	840	1200	1600	2100
IT16	Rough casting	600	900	1300	1900	2500	3200
IT17	Very rough forming	1000	1500	2100	3000	4000	5200
IT18	Extremely rough	1400	2200	3300	4600	6300	8100

Quick Conversion

μm to mm: divide by 1,000. Example: IT7 at 18–30mm = 21μm = 0.021mm total tolerance = ±0.0105mm.

IT grade to ISO 2768 class: IT9 ≈ ISO 2768-m for small dimensions, IT12 ≈ ISO 2768-c. These are rough equivalents, not exact conversions.

Achievable Tolerances by Process

Every process has a practical accuracy limit. Tighter than standard requires extra operations, more setups, slower feeds, or secondary processes — all of which increase cost.

Process	Standard (Typical)	Precision (Extra Cost)	Ultra-Precision (High Cost)	IT Equivalent
CNC Milling (3-axis)	±0.025mm	±0.005mm	±0.002mm	IT8 → IT5 → IT3
CNC Milling (5-axis)	±0.010mm	±0.005mm	±0.002mm	IT7 → IT5 → IT3
CNC Turning	±0.025mm	±0.005mm	±0.002mm	IT8 → IT5 → IT3
Swiss-Type Turning	±0.010mm	±0.005mm	±0.002mm	IT7 → IT5 → IT3
Surface Grinding	±0.005mm	±0.002mm	±0.001mm	IT5 → IT3 → IT2
Jig Boring	±0.010mm	±0.005mm	±0.002mm	IT7 → IT5 → IT3
Wire EDM	±0.010mm	±0.003mm	±0.001mm	IT7 → IT4 → IT2
Sinker EDM	±0.015mm	±0.005mm	±0.002mm	IT8 → IT5 → IT3

Cost Escalation Moving from standard to precision tolerances (±0.025mm to ±0.005mm) typically doubles machining cost. Moving to ultra-precision (±0.002mm) can triple or quadruple cost compared to standard. Each tighter tier requires slower cutting speeds, more finishing passes, additional inspection, and often grinding or EDM as a secondary operation.

Tolerance Stacking

In assemblies, individual part tolerances accumulate. A stack of features each within tolerance can still produce an out-of-spec assembly if the combined deviation exceeds the allowable total.

Worst-Case (Linear) Stack

Assumes every feature is at its maximum deviation in the same direction. Simple and conservative.

Formula


          T_total = T_1 + T_2 + T_3 + ... + T_n

Statistical (RSS) Stack

Root-Sum-Square method. Assumes tolerances follow a normal distribution and features are independent. Gives a smaller, more realistic total. Use when producing in volume (100+ units).

Formula


          T_total = √(T_1² + T_2² + T_3² + ... + T_n²)

Practical Example

Three plates stacked together, each 10.0 ±0.1mm (ISO 2768-m class):

Method	Calculation	Total Stack	Result
Worst-Case	0.1 + 0.1 + 0.1	±0.3mm	Nominal = 30.0mm, range = 29.7 – 30.3mm
RSS	√(0.01 + 0.01 + 0.01)	±0.173mm	Nominal = 30.0mm, range = 29.83 – 30.17mm

Design Implication If the assembly must maintain 30.0 ±0.15mm, worst-case stacking shows the current tolerances are insufficient (0.3 > 0.15). Options: (1) tighten one or more part tolerances, (2) add a shimming adjustment, or (3) redesign to reduce the number of stacked dimensions. RSS gives a tighter prediction but offers no guarantee on any single assembly — some units will still hit worst-case.

When to Specify Tighter Tolerances

ISO 2768 covers general dimensions. Certain features always require individually specified tolerances. The key question: what happens if this dimension is at the limit of its general tolerance?

Scenario	Recommended Tolerance	Why	Typical IT Grade
Shaft in bearing bore	Individual fit (e.g., H7/k6)	Bearing life depends on correct interference/clearance	IT6–IT7
Seal groove diameter	±0.025mm or tighter	O-ring leaks if groove is too wide or too deep	IT7–IT8
Bolt hole pattern (bolted joint)	±0.1mm positional	Bolts must align through mating flanges	IT9–IT10
Locating dowel pins	H7/m6 or tighter	Dowels must be press-fit for repeatable location	IT6–IT7
Hydraulic cylinder bore	±0.005–0.01mm + roundness	Fluid leaks past piston if bore is out-of-round or oversized	IT5–IT7
Mating gear center distance	±0.02–0.05mm	Backlash and noise depend on correct center distance	IT6–IT8
Alignment features (keyways, flats)	±0.02–0.05mm	Misalignment causes vibration, uneven loading	IT6–IT8
Thread depth (tapped holes)	Specify min thread depth	Insufficient thread engagement causes pull-out failure	Per thread standard

Do Not Over-Tolerance Specifying ±0.01mm on every dimension is a common mistake. It forces the machinist to slow down on every cut, increases inspection time, and drives up cost with zero functional benefit. Tolerance only what matters functionally. Use ISO 2768 for everything else.

Common Mistakes

#	Mistake	Why It Matters	Correct Approach
1	Tolerancing every dimension to ±0.01mm	Quadruples cost. Forces grinding on features that do not need it. Adds unnecessary inspection.	Use ISO 2768-m for general dims. Tolerance only critical features individually.
2	Using ISO 2768 for bearing fits	ISO 2768-m at 50mm = ±0.3mm. Bearing seats need ±0.01mm or tighter. The bearing will be loose and fail.	Specify fit directly: H7/k6, H7/p6, etc. Never rely on general tolerances for fits.
3	Ignoring tolerance stacking in assemblies	Five parts each within ±0.1mm can stack to ±0.5mm. The assembly may not fit.	Calculate worst-case stack for critical assemblies. Adjust individual tolerances or add adjustments.
4	Specifying tight tolerances on thin walls	Thin walls deflect during machining. You cannot hold ±0.01mm on a 1mm wall regardless of what the drawing says.	Design adequate wall thickness (≥1.5mm for aluminum, ≥1.0mm for steel). Accept wider tolerances on thin features.
5	Mixing ISO 2768 with GD&T incorrectly	Applying a positional tolerance without referencing datums, or using general tolerances on features that also have GD&T callouts.	GD&T callouts override ISO 2768 for that feature. Define clear datum references on the drawing.
6	Not specifying ISO 2768 at all	The shop has no default to fall back on. Every ambiguous dimension becomes a question.	Always state ISO 2768-mK (or your chosen class) in the title block or drawing notes.
7	Using "reference" or "typ" without definition	Ambiguous. The shop does not know if "TYP" means exactly that value or a general tolerance applies.	Avoid "TYP" on critical dimensions. If used, define what tolerance applies in the notes.
8	Specifying tolerances the process cannot achieve	Calling out ±0.005mm on a sand casting or ±0.001mm on a milling feature results in rejection or excessive cost.	Check achievable tolerance by process before specifying. See the process table above.

← Polishing & Blasting

GD&T Basics →