Engineering lookup guide · 12 min read

ISO 2768 Tolerance Chart: How to Use It

ISO 2768-1:1989 supplies four general tolerance classes—f, m, c, and v—for covered linear and angular dimensions when a drawing explicitly invokes the standard. It does not apply automatically, and an individual tolerance beside a dimension takes precedence. This guide explains how to select the applicable table and range. It does not reproduce ISO’s normative tolerance values; obtain the controlling value from a licensed copy of the applicable edition.

Follow the lookup method Open the official ISO 2768-1 record

By MakerStage Engineering Team · Published 6 August 2026

Start with scope

What ISO 2768-1 actually controls

A general tolerance is a drawing-level rule that fills in a tolerance only for covered dimensions without their own tolerance.

A tolerance defines the acceptable variation around a nominal value. ISO 2768-1 simplifies drawings by letting one class cover specified kinds of dimensions that do not already have an individual tolerance. For broader machining capability and cost context, use the CNC tolerance selection guide.

The standard’s stated primary scope is parts produced by metal removal or formed from sheet metal. Confirm suitability before applying it to castings, molded plastics, weldments, 3D printed parts, or other processes.

Two terms to know before checking scope

Nominal dimension: The intended value printed on the drawing. Use this value—not the measured result—to choose a table range.
General vs individual tolerance: A general tolerance fills a covered gap. An individual tolerance is written beside one dimension or characteristic and takes precedence only for that dimension or characteristic.

Hypothetical drawing example: if the title block invokes ISO 2768-1 class m but a shaft is marked Ø12.00 ±0.02 mm, the written ±0.02 mm governs that shaft diameter. Do not add a general ISO tolerance to it.

Covered when untoleranced

Linear sizes, diameters, steps, radii, and distances
External radii and chamfer heights on broken edges
Angular dimensions, including right angles not governed by a referenced general geometrical-tolerance standard
Dimensions created by machining assembled parts

Not governed by Part 1

Dimensions with their own individual tolerances
Dimensions covered by another referenced standard
Bracketed reference or auxiliary dimensions shown for information rather than inspection acceptance
Boxed theoretically exact dimensions whose allowed variation comes from a separate geometrical control

Scope source: official ISO 2768-1 scope preview.

Decision flow for choosing an individual tolerance or the applicable ISO 2768-1 linear, broken-edge, or angular table — Figure 1. Start with the drawing, confirm that ISO 2768-1 and a class are invoked, then choose the table by characteristic type.

Four classes

f, m, c, and v describe the selected tolerance class

The drawing's class letter selects a column in the official table. It is not a quality grade, fit designation, or promise that every supplier can hold that tolerance.

Fine

For ordinary linear dimensions, f is the tightest tabulated class where a value exists. For angular dimensions and broken edges, f and m use identical values.

Medium

A commonly encountered class, but not an automatic ISO default for CNC machining or every supplier.

Coarse

A wider general band for features whose function permits more variation. Critical fits still need explicit control.

Very coarse

For ordinary linear and angular dimensions, v is generally the widest tabulated class where a value exists. In the broken-edge table, c and v use identical values. Separately, some ordinary-linear class/range combinations have no tabulated value.

Class m is not a default. The designer selects the class from functional need, and the supplier confirms that the manufacturing and inspection methods are capable.

Six-step ISO 2768-1 lookup method

Use six checks before applying an ISO 2768-1 value

Start with the drawing—not the table. These checks prevent you from using the right number for the wrong feature or document.

Read the controlling note
Invoked means explicitly named. Confirm that the title block, drawing note, specification, or contract names ISO 2768-1, the applicable edition, and class f, m, c, or v.
Check precedence and exclusions
Check the dimension itself before using the general class. A written individual tolerance or another referenced standard wins. Reference or auxiliary dimensions are informational. Boxed theoretically exact dimensions receive their allowed variation from separate geometrical controls. Neither receives a Part 1 general tolerance.
Classify the characteristic
Choose ordinary linear, external radius or chamfer height for a broken edge, or angular. Each category uses a different official table.
Select with the nominal metric value
Nominal means the value printed on the drawing. If the drawing says 42.0 mm and inspection reads 41.92 mm, use 42.0 mm to choose the range. The measured value is used later for acceptance.
Consult the licensed table
The normative table is the official table whose values control the drawing. In a licensed copy of the applicable edition, read the intersection of the feature type, nominal range, and class. Never invent a value for a dash.
Calculate and inspect
Bilateral means the same permitted deviation applies above and below nominal. Calculate both limits, use a suitable measuring tool, and apply the agreed pass/fail rule near a limit.

Quick cheat sheet: which lookup path should I use?

Match the characteristic to its controlling nominal input, then use the invoked class in the applicable official table.

Scroll horizontally if the full table is not visible.

Ordinary linear dimension

Use: Nominal size shown on the drawing
Look up: Linear-dimension table and invoked class
Stop and clarify: An individual tolerance or another standard governs, or the table supplies no value.

External broken edge

Use: Nominal external radius or chamfer height
Look up: Broken-edge table and invoked class
Stop and clarify: The feature is an internal fillet, another radius type, or outside the table scope.

Angular dimension

Use: Nominal length of the shorter side
Look up: Angular table and invoked class
Stop and clarify: The angle magnitude or a measured length was used, or a separate geometrical requirement governs.

Choose the official table from the characteristic type
Characteristic	Controlling nominal input	Official lookup path	Stop and clarify when
Ordinary linear dimension	Nominal size shown on the drawing	Linear-dimension table and invoked class	An individual tolerance or another standard governs, or the table supplies no value.
External broken edge	Nominal external radius or chamfer height	Broken-edge table and invoked class	The feature is an internal fillet, another radius type, or outside the table scope.
Angular dimension	Nominal length of the shorter side	Angular table and invoked class	The angle magnitude or a measured length was used, or a separate geometrical requirement governs.

Convert the selected deviation into limits

Lower limit = nominal − deviation

Upper limit = nominal + deviation

Let N be the nominal dimension and T the symmetric deviation selected from the applicable table. The lower and upper limits are the smallest and largest acceptable values. The total tolerance is the full span between them, so a symmetric ±T deviation creates a span of 2T.

Hypothetical math—not an ISO table value: if N = 40.00 mm and the applicable table supplies T = 0.03 mm, the limits are 39.97 mm and 40.03 mm. The total tolerance is 0.06 mm. The actual T must come from the controlling drawing or a licensed copy of the applicable edition.

Use the standard’s millimetre values to select ranges. If the drawing or inspection record uses inches, convert using 1 in = 25.4 mm exactly and round only to the documented resolution.

Symbolic tolerance band with lower limit N minus T, nominal N, upper limit N plus T, and total tolerance 2T — Figure 2. For the bilateral tolerance taught here, the permitted deviation T extends equally below and above nominal N, creating a total span of 2T.

This diagram defines the specification limits only. When a measurement is near either limit, the acceptance decision must also follow the agreed conformity decision rule and account for measurement uncertainty.

A breakpoint stays in its ending range

If the official row is written as “over A up to B,” a nominal value exactly equal to B remains in that row. Only a value above B moves forward.

Metric values control range selection

The standard uses millimetre values to select its ranges. Never select an interval from a rounded display conversion.

A dash or missing range means stop

If the selected cell has a dash, supplies no value, or the nominal size is outside the published range, specify the tolerance individually or obtain clarification. Never treat the gap as zero or extrapolate a value.

Broken edges

External radii and chamfer heights use a separate category

This category exists because a broken edge is specified differently from an ordinary size. Do not apply it to internal fillets or every radius on the part.

A chamfer is a flat bevel across an outside corner. An external radius is a convex rounded outside corner. An internal fillet is the concave rounded corner inside a pocket or between two surfaces.

Select with the dimension shown on the drawing. Use the nominal metric radius or chamfer height—not a measured edge or rounded inch conversion—to select the interval in the applicable table.

Two machined aluminum blocks showing a straight external chamfer and a convex rounded external edge — Figure 3. The broken-edge category covers external radii and chamfer heights; it is not a blanket tolerance for every radius.

Angular dimensions

Angular ranges use the shorter side length

First confirm that no referenced geometrical-tolerance requirement governs. Then use the nominal length of the shorter side that forms the angle to select the ISO 2768-1 Table 3 range—not the angle value or a measured side length.

Oblique angle showing that nominal side L2 is shorter than nominal side L1 and therefore selects the angular tolerance range — Figure 4. L2 is shorter than L1 in this example, so L2 is the lookup input.

Calculate angular limits symbolically

Lower angle = nominal angle − α

Upper angle = nominal angle + α

Hypothetical example: for nominal sides of 40 mm and 70 mm, select the angular interval using 40 mm. Then obtain α from the invoked class and apply it above and below the nominal angle.

Drawing use

State the edition and class in the title block

A supplier cannot infer a class from the absence of individual tolerances. Make the governing note explicit and keep critical requirements beside their dimensions.

The title block is the drawing panel that usually identifies the part, revision, units, material, and general notes. It is where a drawing-level ISO 2768 requirement is commonly stated.

Clear title-block note

GENERAL DIMENSIONAL TOLERANCES: ISO 2768-1:1989, CLASS m.

The shorter designation ISO 2768-m appears on many drawings. Including the part, edition, and class makes the governing requirement unambiguous. The engineering drawing interpretation guide explains how title blocks, notes, dimensions, and revisions work together.

Drawing-release checklist

1Identify the units, drawing revision, ISO part and edition, and selected class.
2Place individual tolerances on features that control assembly or function—for example, a pin-and-hole fit, two mating surfaces, or a dimension whose variation adds to an assembly stack.
3Specify geometrical controls where form, orientation, or location matters. A datum is a theoretically exact reference—such as a plane, axis, or point—established from a datum feature on the part and used to locate or orient another feature.
4State surface finish, thread class, burr or edge condition, and inspection needs separately; ISO 2768-1 does not supply them.
5Ask the supplier to confirm that both the manufacturing process and the inspection method can hold and verify the required tolerance.

Before requesting a quote, add the title-block note, critical individual tolerances, and inspection requirements using the RFQ drawing checklist. MakerStage’s CNC milling and turning overview explains the supported processes and free design-for- manufacturability feedback.

Inspection workflow

Inspect the requirement that actually governs

Inspection starts with the drawing requirement, not the number on the measuring tool. First identify the applicable limits; then compare the measured result using a suitable method.

Inspection sequence: limits, measure, decide

Keep these three jobs separate so a display reading is never mistaken for the complete acceptance decision.

1Obtain the limits from the individual tolerance or the applicable ISO 2768-1 lookup; inspect geometrical requirements separately.
2Choose a measurement method and resolution suitable for the characteristic and tolerance.
3Apply the agreed conformity decision rule and account for measurement uncertainty near a limit.

Ruby-tipped coordinate measuring machine probe contacting the flat top surface of a fixtured machined aluminum block — Figure 5. Inspection starts by identifying the governing requirement, then selecting a measurement method with suitable uncertainty.

A result can sit just inside a limit while its stated measurement-uncertainty interval crosses that limit. Apply and document the agreed conformity decision rule. The dimensional inspection methods guide compares practical inspection options and documentation.

If the agreed conformity decision rule determines that a result is nonconforming, record the nonconformance. A supplier or inspector cannot self-waive it; acceptance needs a documented concession from the authority designated by the drawing, contract, or quality procedure.

Standards transition

mK is a legacy combined callout

In ISO 2768-mK, m refers to Part 1 dimensional tolerances and K referred to a geometrical class in ISO 2768-2:1989. That second part is withdrawn.

Published dimensional edition: ISO 2768-1:1989; ISO lists this as the published Part 1 edition. Use the edition named by the drawing or contract.; Part 1 record
Under publication: ISO 2768 Edition 2; Will replace ISO 2768-1:1989. Confirm the required edition before releasing a new drawing.; Edition 2 record
Withdrawn legacy standard: ISO 2768-2:1989; Withdrawn 4 February 2021. H, K, and L may still govern an existing drawing or contract but are not current guidance for new work.; Part 2 record
Successor standard: ISO 22081:2021; Gives rules for defining and interpreting general geometrical specifications and general size specifications. It is not an automatic one-to-one replacement for class K.; ISO 22081 record

A withdrawn standard can still appear in a contract or legacy drawing. Do not simply replace an old ISO 2768-mK note with ISO 22081 and assume the acceptance meaning stays the same. The drawing owner must confirm which revision governs, define the required geometrical controls, and approve the clarification before manufacture.

Size describes how large a feature is, while geometry describes its form, orientation, or location. A hole can have the correct diameter and still be in the wrong position. Part 1 does not by itself control flatness, straightness, position, coaxiality, or runout. Use the geometric tolerancing fundamentals to separate size from form, orientation, and location.

Common Questions

Frequently Asked Questions

What is ISO 2768?

ISO 2768-1:1989 defines general tolerances for linear and angular dimensions that do not carry individual tolerance callouts. It provides four classes—f, m, c, and v—and applies only when the drawing or controlling specification invokes the standard and identifies a class. It does not apply automatically to every untoleranced dimension.

What does ISO 2768-m mean on a drawing?

ISO 2768-m means the drawing invokes ISO 2768-1 class m, or medium, for covered linear and angular dimensions without individual tolerances. For linear and broken-edge dimensions, the nominal size selects the range. For angular dimensions, use the nominal length of the angle's shorter side. A tolerance written beside a specific dimension takes precedence, so the class-m value is not added to that individual tolerance.

What does ISO 2768-mK mean?

ISO 2768-mK is a legacy combined designation: m refers to Part 1 dimensional tolerances, while K referred to the geometrical class in ISO 2768-2:1989. ISO withdrew Part 2 in 2021 and lists ISO 22081:2021 as its replacement. Do not silently convert K into an ISO 22081 requirement; obtain engineering clarification.

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

The letters identify four general-tolerance classes: f is fine, m is medium, c is coarse, and v is very coarse. The permitted deviation changes with nominal size and characteristic type. A class name does not prove that a process can hold the value, and ISO does not make class m a universal manufacturing default.

Is ISO 2768-2 still valid?

ISO 2768-2:1989 is withdrawn. ISO records 4 February 2021 as its withdrawal date and lists ISO 22081:2021 as the replacement. ISO 22081 does not reproduce the old H, K, and L classes as a drop-in chart; current geometrical specifications need defined values, rules, and an appropriate datum framework.

How do I find the ISO 2768 tolerance for a dimension?

First confirm that the dimension is covered, individually untoleranced, and governed by an invoked ISO 2768-1 class. Use the nominal metric value shown on the drawing—not a measured result or rounded inch conversion—to find the corresponding interval in a licensed copy of the standard. Do not assume class m unless the drawing specifies it.

Does ISO 2768 override a tolerance shown next to a dimension?

No. An individual tolerance shown beside a dimension governs that characteristic instead of the general ISO 2768-1 value. The general class fills defined gaps; it is not an extra tolerance added to explicit limits. Other referenced standards, bracketed auxiliary dimensions, and boxed theoretically exact dimensions also sit outside the Part 1 general-tolerance tables.

What is the difference between ISO 2768 and ISO 286?

ISO 2768-1 fills in general tolerances that a drawing leaves unstated. ISO 286 provides a standardized system of tolerance grades and deviations for specifying fits between holes and shafts. The designer must still select an explicit fit designation or limits—for example, to make a pin slide freely, locate closely, or press tightly into a hole.

Can an out-of-tolerance part still be accepted?

A supplier or inspector cannot self-waive a nonconformance. Acceptance requires a documented concession from the authority designated by the governing drawing, contract, or quality procedure—often the customer or design authority. ISO 2768-1 notes that exceeding a general tolerance does not always impair function, but the authorized disposition still needs to be recorded.

Related Resources

CNC Tolerance Selection Guide

Connect drawing tolerances to machining, inspection, and cost decisions.

Engineering Drawing Interpretation

Read title blocks, dimensions, tolerances, surface finish, and GD&T.

Dimensional Inspection Methods

Choose calipers, micrometers, CMM inspection, FAI, and reporting.

Put the governing tolerances in the RFQ package

Include the drawing revision, ISO edition, selected class, individually toleranced critical features, and inspection requirements. MakerStage provides free DFM feedback with CNC machining RFQs.

Upload Your Drawing for a CNC Quote