ASME B4.3-1978 (2004) — General Tolerances for Metric Dimensioned Products

28 10 月, 2026
ASME Standards

📐 ASME B4.3-1978 (2004) shows how to specify general tolerances for metric (millimeter) dimensions that carry no individual tolerance indication. It is the U.S. counterpart of the international standard ISO 2768, “Permissible machining variations in dimensions without tolerance indications,” prepared by ISO/TC3 (Limits and Fits) and approved in 1972. The American National Standards Committee B4 — reorganized in November 1975 and renamed “Standardization of Allowances and Tolerances for Manufactured Parts” — decided to prepare a similar American standard based on ISO 2768, and final approval was granted by the American National Standards Institute on March 16, 1978, followed by reaffirmation in 2004. Designed to be used together with ASME B4.2 (Preferred Metric Limits and Fits), this document is the key to keeping “untoleranced” dimensions unambiguous on metric drawings.

💡 B4.3 solves a very practical problem: some dimensions on a drawing are functionally unimportant and should not each carry an individual tolerance callout. Left uncontrolled, machinists and inspectors will argue about how tight “good enough” is. B4.3 brings a recognized series to govern all such dimensions — saving drafting effort and eliminating ambiguity at once.

1. Scope and Basic Philosophy 📌

Section 1 (Scope) states the purpose: to show how to specify the general tolerances for metric dimensions without tolerance designation. The fine and medium tolerance series shown in Table 1 are mostly applicable to machined parts, while the coarse series covers tolerances for use on all types of dimensions — castings, forgings, weldments, stampings, and other non-machined features.

Section 2 (Tolerance Indication) establishes a governing principle: all drawing dimensions of parts shall be associated with tolerance data. These data may be expressed in one of three ways:

Direct callout: specified limits or a tolerance applied directly to the dimension;
Referenced documents: tolerances specified in other documents referenced on the drawing;
General tolerance note: a note referring to all dimensions on a drawing for which tolerances are not otherwise specified.

⚠️ A general tolerance is not a license to be sloppy. B4.3 requires every dimension on the drawing to have a tolerance home: direct callout, referenced document, or general note. A dimension covered by none of these has no acceptance basis and invites disputes.

2. Four Recommended Ways to Write the General Tolerance Note 📋

Section 3 gives four methods for linear dimensions; the designer selects whichever fits the drawing:

Method	Expression	When to Use
Method 1 — IT grade reference	“UNLESS OTHERWISE SPECIFIED ALL UNTOLERANCED DIMENSIONS ARE ±IT14/2”	Ties into the IT grade system (B4.2 Appendix B, Table B1); the deviation equals half the IT grade
Method 2 — Series reference	“UNLESS OTHERWISE SPECIFIED, THE GENERAL TOLERANCE SPECIFIED IN ANSI B4.3 MEDIUM SERIES APPLY”	The most common; cites the fine/medium/coarse series of Table 1
Method 3 — Series table	Reproduce the stepped tolerance table of Table 1 on the drawing	Most direct for the shop floor; no need to consult the standard
Method 4 — Decimal-place rule	Tolerances keyed to the number of decimal digits (e.g., one decimal ±0.3, no decimals ±3)	Where dimensions do not vary much in magnitude and drafting must stay simple

The Standard also allows a single tolerance value for all untoleranced nominal dimensions (for example “UNLESS OTHERWISE SPECIFIED ALL UNTOLERANCED DIMENSIONS ARE ±0.8 mm”), with an explicit note that this method is recommended only where the magnitudes of the dimensions on the drawing do not vary appreciably — otherwise the single value is too tight for large dimensions or too loose for small ones.

💡 Method 4 (decimal-place rule) is the fastest for quick design, but it relies on the convention “more decimal digits means tighter.” If a part really needs different levels of precision in different areas, go back to Method 2 and pick the series consciously instead.

3. Linear General Tolerance Series (Table 1) 📏

Table 1 gives the permissible variations in millimeters for three series (Fine, Medium, Coarse) over basic-dimension steps from 0.5 mm up to 2000 mm:

Series	0.5–3	3–6	6–30	30–120	120–315	315–1000	1000–2000
Fine	±0.05	±0.05	±0.1	±0.15	±0.2	±0.3	±0.5
Medium	±0.1	±0.1	±0.2	±0.3	±0.5	±0.8	±1.2
Coarse	±0.2	±0.3	±0.5	±0.8	±1.2	±2	±3

⚠️ Choose the series by need, not by preference. Machined parts normally use Fine or Medium. Setting the general tolerance too loose can let functionally significant dimensions run away; setting it too tight drives up cost on dimensions that do not matter.

4. Angular and Taper Tolerances (Table 2) 📐

Table 2 covers general tolerances for angles and tapers. The angular tolerance is based on the length of the shorter of the two legs forming the angle. The tolerance may be expressed as an angle in decimal degrees or in degrees and minutes, as a taper in percentage (mm per 100 mm), or in milliradians. Typical steps for shorter leg lengths up to 10, 10–50, 50–120, and 120–400 mm are:

Length of Shorter Leg (mm)	Angular Tolerance (degrees/min)	Angular Tolerance (milliradians)
Up to 10	±1°	±17
10–50	±0°30′	±9
50–120	±0°20′	±6
120–400	±0°10′	±3

The angular general tolerance may be specified on the drawing as: “UNLESS OTHERWISE SPECIFIED THE GENERAL TOLERANCES IN ANSI B4.3 APPLY”; or the numerical values of Table 2 may be added to the drawing format; or a single value in degrees and minutes such as 0°30′ may be given.

🚨 The link between angular tolerance and the shorter leg matters: for the same angle tolerance, the longer the leg, the larger the linear deviation at its end. State the leg-length basis in the callout and judge machining and inspection against the same reference, or each party will measure “its own truth.”

5. Engineering Practice Essentials 🛠️

🔍 Drawing convention: place one general tolerance note near the title block citing the series (fine/medium/coarse) or the IT grade; never let two conflicting general notes coexist on the same drawing.
🔧 Division of labor with functional tolerances: the general tolerance covers only unimportant dimensions; every dimension that participates in fits, alignment, or assembly interfaces must carry its own explicit tolerance and must not rely on the general note.
📊 Pairing with B4.2: use the preferred metric limits and fits of B4.2 for hole-and-shaft features that need precision fits, and B4.3 general tolerances for everything else; together they keep drawings both concise and rigorous.
📋 International alignment: the same logic corresponds to ISO 2768 (ISO 2768-1/-2). In cross-supplier or cross-country collaboration, state the exact standard and edition in procurement and technical agreements to avoid silent parameter differences.

6. Frequently Asked Questions ❓

❓ Q: How does B4.3 relate to ISO 2768?
A: B4.3 is the American national version based on ISO 2768, “Permissible machining variations in dimensions without tolerance indications.” The value system and the series logic are aligned, but the drawing should cite the specific edition it references.

❓ Q: Which series should I pick — fine, medium, or coarse?
A: Machined parts normally use Fine or Medium; the Coarse series suits cast, forged, or welded features. “Coarser is cheaper” only counts when the function allows it — never when the dimension matters.

❓ Q: What wins when a direct callout conflicts with the general tolerance note?
A: The direct tolerance on the individual dimension takes precedence. The general note only “catches” dimensions that have neither a direct callout nor a tolerance specified in a referenced document.

🔍 Q: Why are angular tolerances keyed to the shorter leg?
A: For the same angular deviation, the leg length determines the magnitude of the linear offset at its end. Keying the tolerance to the shorter leg guarantees that no angular feature, whatever its orientation, develops an excessive actual deviation.

ASME B4.3-1978 (2004) scan.pdf