FREE ENGINEERING SPREADSHEET
Free ISO 2768 Tolerance Chart Spreadsheet — Excel & Google Sheets
Download our free ISO 2768 tolerance chart spreadsheet for instant tolerance lookup during design, quoting, and inspection. Built by CNC machinists and used on the shop floor at our Qingdao facility — it covers every tolerance class in both parts of the standard, does the mm-to-inch math for you, and includes a printable reference sheet. No sign-up required.
✓
f / m / c / v & H / K / L Classes
✓
ISO 2768-1:1989 & ISO 2768-2:1989
✓
Excel & Google Sheets — No Sign-Up
Tolerance Classes
General tolerance designations per ISO 2768
f
Fine
m
Medium
c
Coarse
v
Very Coarse
Most Common CNC Machining Callout
ISO 2768-mK
GENERAL TOLERANCES
What Is ISO 2768? A Quick Overview
ISO 2768 is the international standard that defines general tolerances — the default dimensional and geometric limits that apply when a drawing does not specify individual tolerances on every feature.
Instead of cluttering a drawing with ±0.1 on every non-critical dimension, the designer writes one note in the title block and the standard fills in the gaps. The standard is technically identical to the older DIN 7168 and is recognized globally across European, Asian, and North American supply chains.
ISO 2768-1
Covers general tolerances for linear dimensions, angular dimensions, and external radii/chamfers. It defines four tolerance classes: f (fine), m (medium), c (coarse), and v (very coarse).
ISO 2768-2
Covers general geometric tolerances — straightness, flatness, perpendicularity, symmetry, and circular run-out. It defines three classes: H (high precision), K (medium), and L (low precision).
ISO 2768-mK
A callout like ISO 2768-mK means medium linear tolerances per Part 1 and K-class geometric tolerances per Part 2 — the most common designation in general mechanical engineering and the default for most CNC machining services.
TOLERANCE REFERENCE DATA
ISO 2768-1 Tolerance Chart: Linear Dimensions (f/m/c/v)
Permissible deviations for linear dimensions per ISO 2768-1. All values are in millimetres; inch conversions are included in the downloadable spreadsheet.
A dash (—) means the tolerance class is not defined for that size range. If your part falls into one of these gaps, choose a different class or specify an explicit tolerance on the drawing. Never interpolate between dash entries — the standard does not support it.
| Nominal Size Range (mm) | f — Fine (±mm) | m — Medium (±mm) | c — Coarse (±mm) | v — Very Coarse (±mm) |
|---|---|---|---|---|
| 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 |
Angular Tolerances (ISO 2768-1)
| Shorter Side Length (mm) | f — Fine | m — Medium | c — Coarse | v — Very Coarse |
|---|---|---|---|---|
| Up to 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′ |
| Over 400 | ±0°5′ | ±0°5′ | ±0°10′ | ±0°20′ |
External Radius & Chamfer Tolerances
| Nominal Size (mm) | f & m (±mm) | c & v (±mm) |
|---|---|---|
| 0.5 – 3 | ±0.2 | ±0.4 |
| >3 – 6 | ±0.5 | ±1.0 |
| >6 – 30 | ±1.0 | ±2.0 |
Angular Tolerances Follow the Shorter Side
Angular tolerances depend on the length of the shorter side of the angle, not the angle measurement itself. Classes f and m share identical angular values — there is no penalty for using m over f for angular dimensions.
Verified Against the Standard
All values are verified against ISO 2768-1:1989. Deviations apply to dimensions without individual tolerance indications; features with explicit tolerances on the drawing always take precedence.
GEOMETRIC TOLERANCE DATA
ISO 2768-2 Tolerance Chart: Geometric Tolerances (H/K/L)
Geometric tolerances control form and position — how flat, straight, perpendicular, or symmetrical a feature must be when no GD&T frame is specified. All values in millimetres.
Straightness & Flatness
| Nominal Length (mm) | H (±mm) | K (±mm) | L (±mm) |
|---|---|---|---|
| Up to 10 | 0.02 | 0.05 | 0.1 |
| >10 – 30 | 0.05 | 0.1 | 0.2 |
| >30 – 100 | 0.1 | 0.2 | 0.4 |
| >100 – 300 | 0.2 | 0.4 | 0.8 |
| >300 – 1000 | 0.3 | 0.6 | 1.2 |
| >1000 – 3000 | 0.4 | 0.8 | 1.6 |
Perpendicularity
| Nominal Length (mm) | H (±mm) | K (±mm) | L (±mm) |
|---|---|---|---|
| Up to 100 | 0.2 | 0.4 | 0.6 |
| >100 – 300 | 0.3 | 0.6 | 1.0 |
| >300 – 1000 | 0.4 | 0.8 | 1.5 |
| >1000 – 3000 | 0.5 | 1.0 | 2.0 |
Symmetry
| Nominal Length (mm) | H (±mm) | K (±mm) | L (±mm) |
|---|---|---|---|
| Up to 100 | 0.5 | 0.6 | 0.6 |
| >100 – 300 | 0.5 | 0.6 | 1.0 |
| >300 – 1000 | 0.5 | 0.8 | 1.5 |
| >1000 – 3000 | 0.5 | 1.0 | 2.0 |
Circular Run-Out
0.1 mm
Class H
0.2 mm
Class K
0.5 mm
Class L
Important limitation: ISO 2768-2 does not cover parallelism, cylindricity, concentricity, profile, or true position. If your part requires control of these characteristics, you must specify them with explicit GD&T callouts — general tolerances will not apply. Values verified against ISO 2768-2:1989.
SPREADSHEET GUIDE
How to Use the ISO 2768 Tolerance Spreadsheet
Our free spreadsheet puts every table on this page into an interactive format — no more scrolling through PDFs or switching between browser tabs.
01
Enter Your Dimension
Type your nominal dimension into the Tolerance Lookup tab. Linear, angular, and geometric tolerances are all covered.
02
Select the Class
Choose a tolerance class from the dropdown — f, m, c, or v for dimensional tolerances, H, K, or L for geometric tolerances.
03
Read the Tolerance
The spreadsheet returns the exact ± tolerance in both millimetres and inches, ready for design reviews, quoting, or inspection.
When to Use Each Tolerance Class
Choosing the right ISO 2768 tolerance class is a balancing act between function, manufacturability, and cost. Here is what each class means in practice on the shop floor.
| Class | On the machine | When to use it | Cost impact |
|---|---|---|---|
| f — Fine | Careful setup, sharp tooling, light finishing passes, often 100% CMM inspection. A 50 mm dimension allows ±0.15 mm. | Bearing seats, dowel pin holes, press-fit interfaces, sealing surfaces, aerospace and medical components with tight tolerance stacks. | Applied globally, can increase machining cost 2–5× versus m-class. Reserve it for features where function demands it. |
| m — Medium (Industry Default) | Standard CNC machining practice — no special setup or tooling beyond competent CAM programming. Any ISO 9001 shop can hold it. | General mechanical parts: brackets, housings, mounting plates, spacers, covers. The vast majority of CNC machined parts ship with m-class; it is Baetro’s default standard for all CNC machining unless the drawing specifies otherwise. | Baseline. No premium. |
| c — Coarse | Easily achievable on any CNC equipment; generous clearance, no precise fit required. | Non-critical geometry: guard panels, spacers with loose clearance holes, rough mounting features, welded fabrications that will be post-machined. | Below baseline; fastest and cheapest to produce. |
| v — Very Coarse | Suitable for raw stock and pre-machining conditions rather than finished features. | Raw stock dimensions, flame-cut blanks, cast surfaces, and features that will be machined in a subsequent operation. Rarely specified on finished CNC parts. | Lowest cost; not for finished functional features. |
A practical rule: for any given part, roughly 80–90% of features can use m-class general tolerances. The remaining 10–20% — the features that actually locate, seal, or transmit load — need explicit tolerances on the drawing. Our engineers review every CAD file for free and flag features that may be over- or under-toleranced before a single chip is cut.
STANDARDS COMPARISON
ISO 2768 vs. Other Tolerance Standards
Engineers working across global supply chains often encounter multiple tolerance standards on the same project. Here is how ISO 2768 compares.
ISO 2768 fills the gaps with blanket tolerance classes; the other standards handle fits, feature-specific GD&T, and national equivalents.
Limits & Fits
ISO 286
Specific fit designations (H7/g6, H7/p6) for cylindrical features. Best for shaft/hole assemblies and bearing fits where the fit itself is functional.
GD&T
ASME Y14.5
Per-feature symbolic control with datums. Best for high-precision fits, aerospace, defense, and functional gauging where every control is individually defined.
Equivalents
DIN 7168 & GB/T 1804
DIN 7168 is technically identical to ISO 2768-1 and superseded — use ISO 2768 for new designs. GB/T 1804 closely mirrors ISO 2768-1 and is functionally equivalent on drawings from Chinese suppliers.
Side-by-Side Comparison
| Standard | Scope | Approach | Best For |
|---|---|---|---|
| ISO 2768 | General tolerances for undimensioned features | Blanket tolerance classes (f/m/c/v, H/K/L) | General mechanical parts, non-critical features |
| ISO 286 | Limits and fits for cylindrical features | Specific fit designations (H7/g6, H7/p6) | Shaft/hole assemblies, bearing fits |
| ASME Y14.5 | Geometric dimensioning and tolerancing (GD&T) | Per-feature symbolic control with datums | High-precision fits, aerospace, defense, functional gauging |
| DIN 7168 | General tolerances (superseded) | Identical to ISO 2768-1 technically | Legacy drawings; use ISO 2768 for new designs |
| GB/T 1804 | Chinese national standard for general tolerances | Closely mirrors ISO 2768-1 | Drawings from Chinese suppliers; functionally equivalent to ISO 2768 |
ISO 2768
General tolerances in the title block
ISO 286
Explicit fits on critical features
ASME Y14.5
GD&T for the functional 20%
If your drawing has a tolerance block, it should reference ISO 2768 for general tolerances. Critical-fitting features — bearing bores, shaft diameters, dowel holes — should carry explicit ISO 286 fit designations or ASME Y14.5 GD&T callouts. ISO 2768 fills the gaps; it should never be the only tolerance control on a functional assembly.
ISO 2768 Questions
Frequently Asked Questions
ISO 2768-mK is the most common general tolerance callout on CNC machining drawings. The lowercase “m” specifies medium tolerance class for linear and angular dimensions per ISO 2768-1; the uppercase “K” specifies K-class geometric tolerances for straightness, flatness, perpendicularity, symmetry, and run-out per ISO 2768-2. For a 50 mm dimension, ISO 2768-m allows ±0.3 mm. This callout is the default standard at most CNC machine shops, including ours.
ISO 2768-1 covers dimensional tolerances — how much a length, diameter, angle, radius, or chamfer may deviate from nominal. ISO 2768-2 covers geometric tolerances — how much a surface may deviate from perfect flatness, straightness, perpendicularity, or symmetry. Both parts are typically referenced together (as in “ISO 2768-mK”), but it is valid to reference only Part 1 if geometric tolerances are controlled elsewhere.
Use ISO 2768-m (medium) as your default for general CNC machining. It balances precision with cost and is achievable on any properly maintained CNC mill or lathe. Reserve f (fine) for features with a functional requirement for tighter control — bearing fits, sealing surfaces, dowel locations. Avoid applying f-class globally; it drives up cost without adding value on non-critical features.
Yes — but with caveats. A standard 3-axis or 5-axis CNC machining center can hold ISO 2768-f tolerances (±0.05 mm under 6 mm, ±0.1 mm for 6–30 mm), but doing so consistently requires sharp tooling, light finishing passes, and inspection verification, so many shops charge a premium. At Baetro, our standard tolerance is ISO 2768-m, with precision CNC machining to f-class available on request.
ISO 2768 is a blanket tolerance standard — one callout covers every undimensioned feature on the drawing. ASME Y14.5 is a feature-specific symbolic language with datums, tolerance zones, and material condition modifiers. They are often used together: ISO 2768 covers the non-critical 80% of features, and GD&T controls the functional 20%. ISO 2768 follows the independence principle, while ASME Y14.5 follows the envelope principle (Rule #1 — perfect form at MMC).
No. ISO 2768 does not specify surface roughness (Ra, Rz) or finish requirements. If your part requires a specific surface finish — such as Ra 1.6 µm for a sealing surface or Ra 0.8 µm for a bearing journal — you must call it out separately on the drawing. Surface finish specifications are covered by standards like ISO 1302 and ISO 4287.
If the drawing references ISO 2768 without a class letter, then no specific tolerance class is applicable. This is either a drafting error, or the drawing already has explicit tolerances on every dimension and the reference is informational. In practice, ask the designer to clarify which class they intend — the difference between f and m can mean a 2× difference in machining cost.
Tolerance tightens, cost compounds — and not linearly. A part toleranced to ISO 2768-m machines in one or two passes with standard tooling. Dropping to f-class may require a finishing pass, sharper tooling, and CMM inspection. Dropping further to ±0.01 mm — beyond any ISO 2768 class — often requires grinding, honing, or wire EDM. Each step roughly doubles the machining cost for that feature. Our DFM review helps you identify which features truly need tight tolerances and which can safely use the standard m-class default.
Get CNC Parts Machined to Your Specified Tolerances
Specify ISO 2768-m, ISO 2768-f, or your own custom tolerances; our engineers review your design for free and flag over- or under-toleranced features before cutting. Parts ship in 3–7 days with full inspection reports from our ISO 9001 certified facility in Qingdao — 30+ CNC machines including 5-axis machining centers, no minimum order quantity, worldwide shipping.