Drawing Notes and General Tolerances: ISO 2768 and ASME Y14.5

General tolerances in the title block are not a fallback for sloppy dimensioning — they are a deliberate engineering decision that sets the quality floor for every untoleranced feature on the drawing, and the difference between ISO 2768-m and ISO 2768-f can mean the difference between a part that assembles and one that does not.

Not every dimension on an engineering drawing requires an individual tolerance callout. For the vast majority of dimensions — those that are not critical to fit, form, or function — a general tolerance applied to all such dimensions simplifies the drawing and communicates the overall quality standard for the part. ISO 2768 defines the standard general tolerance classes for linear dimensions, angular dimensions, and geometric features. ASME Y14.5 takes a different approach through its envelope principle and title block notes. This article covers ISO 2768 tolerance classes, what they cover, how they are specified on drawings, and the general notes framework used in ASME-governed drawings.

ISO 2768: General Tolerances in Two Parts

ISO 2768 is divided into two parts:

• ISO 2768-1: General tolerances for linear and angular dimensions (applies to machined parts without individual tolerance callouts)
• ISO 2768-2: General geometrical tolerances for features without individual GD&T callouts — form, orientation, and runout tolerances for the overall part

Both parts are typically specified together on a drawing title block note: “GENERAL TOLERANCES PER ISO 2768-mK” where “m” is the ISO 2768-1 class and “K” is the ISO 2768-2 class.

ISO 2768-1: Tolerance Classes for Linear and Angular Dimensions

Four tolerance classes are defined, from tightest to loosest:

• f (fine): For high-precision machined parts where good dimensional accuracy is required. Requires precision machining throughout.
• m (medium): The most commonly used class in general mechanical engineering. Appropriate for standard turned, milled, and ground parts made on modern CNC equipment.
• c (coarse): For parts made with larger process variation — heavy machining, large castings, structural steel. Allows significant dimensional variation on non-critical features.
• v (very coarse): For rough work, large fabrications, and non-functional dimensions where precise measurement is impractical or unnecessary.

Tolerance values per class (selected nominal size ranges):

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

These are bilateral (±) tolerances. Every linear dimension without an individual tolerance callout is subject to the applicable row of this table based on the nominal size range and the class specified in the title block.

ISO 2768-1 also defines general angular tolerances by nominal arm length:

• For short arms (up to 10 mm): f = ±1°; m = ±1°; c = ±1°30′; v = ±3°
• For medium arms (10–50 mm): f = ±0°30′; m = ±0°30′; c = ±1°; v = ±2°
• For long arms (over 400 mm): f = ±0°5′; m = ±0°10′; c = ±0°20′; v = ±0°30′

ISO 2768-2: Geometrical General Tolerances

ISO 2768-2 defines three classes of general geometric tolerance (H, K, L) for straightness, flatness, cylindricity, circular runout, and perpendicularity/angularity of the overall workpiece — not individual features. These are the default GD&T tolerances that apply when no individual feature control frame is specified.

Classes:

• H (tight): High-precision requirements, precision equipment
• K (medium): General engineering requirements, most machined parts
• L (loose): Rough machining, larger variation acceptable

Example geometric tolerance values (straightness and flatness, class K):

• Up to 10 mm nominal length: 0.05 mm
• 10–30 mm: 0.1 mm
• 30–100 mm: 0.2 mm
• 100–300 mm: 0.4 mm
• 300–1000 mm: 0.8 mm

These are relatively loose values compared to typical individual GD&T callouts on critical features. They represent the background quality level — the baseline from which specific features are specified tighter as needed.

What ISO 2768 Does NOT Cover

ISO 2768 does not apply to:

• Linear dimensions that are toleranced individually on the drawing (individual callout overrides the general tolerance)
• Auxiliary dimensions (shown in parentheses — these are reference only, no tolerance applies)
• Theoretically exact (basic) dimensions (shown in a box — tolerance comes from the associated GD&T callout)
• Thread callouts (governed by the thread tolerance class in the designation)
• Weld joint dimensions (governed by welding standards)
• Surface texture (governed by individual symbols or the default stated separately)
• Features to which a specific tighter GD&T callout has been applied (the tighter callout governs)

Title Block Note Placement and Format

The ISO 2768 general tolerance specification is placed in the title block, typically in a dedicated “TOLERANCES” or “GENERAL TOLERANCES” field. The format:

• ISO 2768-mK: Medium dimensional tolerance, K geometric tolerance
• ISO 2768-fH: Fine dimensional, H geometric (high precision parts)
• ISO 2768-cL: Coarse dimensional, L geometric (weldments, rough fabrications)

When ISO 2768 is specified, the inspector applies the appropriate tolerance from the tables for any dimension that does not have its own individual callout. It is not necessary to state “±0.2” for every non-toleranced dimension — the title block note covers them all.

ASME Drawing Notes Framework

ASME Y14.5-governed drawings use a different approach for general tolerances. Rather than a tiered class system, ASME drawings state the general tolerances explicitly in the title block or in a general notes zone:

Common ASME title block note examples:

• UNLESS OTHERWISE SPECIFIED: LINEAR ±0.01, ANGULAR ±0°30′, SURFACE FINISH Ra 3.2 μm
• ALL DIMENSIONS IN MILLIMETERS
• REMOVE ALL BURRS AND SHARP EDGES: R0.5 MAX OR 0.5×45° CHAMFER
• ALL THREADS: [thread class] UNLESS NOTED
• TOLERANCES PER ASME Y14.5-2018

Additional notes for specific requirements:

• HEAT TREAT TO [specification] AFTER MACHINING
• ANODIZE PER [specification], TYPE II, CLASS 2
• PASSIVATE PER ASTM A967 AFTER MACHINING
• MAGNETIC PARTICLE INSPECTION PER [specification] — 100%
• DO NOT SCALE DRAWING
• INTERPRET PER ASME Y14.5-2018

When Specific Tolerances Override General Tolerances

The hierarchy is clear in both ISO and ASME systems: any specific tolerance on a feature overrides the general tolerance for that feature. This creates a two-tier system:

• Tier 1 (specific): Individual dimension tolerance, GD&T feature control frame, or specific note — governs that feature exclusively
• Tier 2 (general): Title block general tolerance — applies to all other features not covered by Tier 1

This means the engineer only needs to individually tolerance features where the general tolerance is inadequate for functional requirements. Non-critical distances between features, overall lengths used for reference, and clearance dimensions can all rely on the general tolerance — saving drawing space and reducing clutter while maintaining clear communication of quality intent.

Common Drawing Notes Checklist

A well-formed drawing notes section should include:

• Applicable standard (INTERPRET PER ISO/ASME designation)
• General tolerances (ISO 2768 class or ASME UOS statement)
• Units (ALL DIMENSIONS IN MM unless otherwise noted)
• Default surface finish
• Default material specification (if not in the title block)
• Deburring and edge break requirement
• Any required processes (heat treat, coating, inspection)
• Special handling or cleanliness requirements
• DO NOT SCALE (prevents dimension scaling from printed drawings)

Conclusion

General tolerances per ISO 2768 or ASME title block notes are the silent baseline that governs every non-individually-toleranced feature on an engineering drawing. Choosing the right ISO 2768 class — f for precision, m for general purpose, c for rough work — communicates the overall quality intent of the part clearly and efficiently. The hierarchy of specific over general tolerances ensures that critical features receive explicit individual attention while routine dimensions are handled by the general tolerance without cluttering the drawing. Combined with appropriate drawing notes for material, process, and standards, a well-structured title block is itself a precision engineering document.