Dimensioning and general tolerances: ISO 2768, ISO 8015 and ASME Rule #1

Every number on a drawing has a tolerance, whether it is written next to it or not. Most dimensions you place never get an individual tolerance. They fall back on a general tolerance in the title block. Know exactly what that fallback allows and what it does not control. That knowledge separates a drawing the machine shop can quote from one that ends in a concession.

Dimensions are placed to ISO 129-1:2018 + Amd 1:2020 and ASME Y14.5-2018 (R2024). Dimensions without their own tolerance take the ISO 2768 general tolerance tables. ISO and ASME split on one point of principle that every design engineer needs to understand: whether size controls form.

Dimensioning principles that checkers enforce

ISO 129-1 sets out how dimensions and tolerances are presented; ASME Y14.5-2018 opens with a set of fundamental rules. The two agree on the substance. Paraphrased:

Principle	What it means on the drawing	Typical graduate error
Each feature is toleranced	ASME Y14.5-2018 states “Each feature shall be toleranced”: by an individual tolerance, a limit, a geometric tolerance or a general note	A basic dimension with no feature control frame, or a note missing from the title block
Complete	Every feature is fully defined; nobody has to scale the print or assume	Hole depth or a chamfer size missing
Minimum necessary	Each dimension appears once, on the view that shows the feature most clearly	The same length on two views, or overall length plus every step
Dimension for function	Dimension from the surfaces that locate or mate, not from the order the CAD model was built	Positions measured from a chamfer edge because that was sketch 1
Reference dimensions	Extra information goes in brackets (US: parentheses), untoleranced and not inspected	A reference dimension with a tolerance, or used as an inspection point
Implied 90 degrees	Lines drawn at right angles, and centre lines crossing at right angles, are 90 degrees with the general angular tolerance	Writing 90° on every corner

Over-dimensioning is the most common fault. If the overall length and every step are all toleranced, the drawing contains a closed loop, and the tolerances cannot all be met at once. Leave one dimension out, or give it in brackets as reference.

Symbols save words. Ø is diameter, R radius, SØ and SR spherical diameter and radius, and □ a square section. A boxed value is a theoretically exact (US: basic) dimension, controlled by a geometrical tolerance. Always put Ø on a diameter dimensioned in a side view, where the circle is not visible.

Chain vs baseline dimensioning

How you arrange dimensions decides how tolerance accumulates. In chain dimensioning each feature is located from the previous one. The position of the last feature relative to the first then carries the sum of every tolerance in the chain. In baseline dimensioning every feature is located from one datum face, so each position carries only its own tolerance. The distance between two features, though, now carries the sum of two.

The rule: put the tolerance on the dimension that matters. If the middle step carries a bearing that must be 25 mm wide, dimension it directly and accept accumulation elsewhere. When several parts stack in an assembly, you are into a tolerance stack-up. The tolerance stack-up calculator handles worst case and root sum square, and the stack-up worked example walks through a full loop.

ISO 2768-1 general tolerance tables

ISO 2768-1:1989 is still current (a revised single-part ISO 2768 is at final draft stage in 2026 but not yet published). It gives four classes: f (fine), m (medium), c (coarse) and v (very coarse). The note “ISO 2768-m” applies class m to every linear and angular dimension without its own tolerance. The table starts at 0.5 mm, so smaller dimensions need an individual tolerance.

Angular tolerances depend on the length of the shorter side of the angle. The same angular error moves the end of a long leg further.

ISO 2768-mK: the withdrawn part that is still everywhere

ISO 2768-2:1989 added three classes (H, K, L) of general geometrical tolerances for features without an individual geometrical tolerance. The combined note “ISO 2768-mK” means linear and angular class m plus geometrical class K.

ISO 2768-2 (withdrawn)	H	K	L
Straightness and flatness, up to 10 mm	0.02	0.05	0.1
Straightness and flatness, over 100 to 300 mm	0.2	0.4	0.8
Perpendicularity, shorter side up to 100 mm	0.2	0.4	0.6
Perpendicularity, over 100 to 300 mm	0.3	0.6	1
Circular run-out	0.1	0.2	0.5

ISO 2768-2 has been withdrawn and replaced by ISO 22081:2021, which works differently. It states a general geometrical specification as a profile tolerance relative to a datum system, with no H, K, L look-up table. In practice “ISO 2768-mK” remains common on legacy drawings and supplier standards, and inspectors still recognise it. For new work, follow your company drawing standard. If it still uses mK, use it consistently, and expect a revision when the single-part ISO 2768 is published.

General tolerances on ASME drawings

ASME Y14.5 has no ISO 2768 equivalent. US shops put a tolerance block in the title block, keyed to decimal places. Typical entries are X.X ±0.1 and X.XX ±0.05 in millimetres, or .XX ±.01 and .XXX ±.005 in inches. These values are company practice, not a standard, so never assume one company’s block applies to another’s drawing.

ISO 8015 independency vs ASME Rule #1

This is where ISO and ASME drawings genuinely differ. ISO 8015:2011 sets the fundamental rules of the ISO GPS system. Its invocation principle reads: “Once a portion of the ISO GPS system is invoked in a mechanical engineering product documentation, the entire ISO GPS system is invoked, unless otherwise indicated”. Its independency principle says each requirement is met independently: a size tolerance controls local size only, not form.

ASME Y14.5 takes the opposite default. Rule #1 (the envelope principle) applies where only a size tolerance is given. The limits of size of a regular feature of size then also control its form, and at maximum material condition (MMC) the feature must have perfect form.

On an ISO drawing you get envelope behaviour only where you ask for it, by adding Ⓔ after the size tolerance (ISO 14405-1:2025). An example is Ø10 h7 Ⓔ on a pin that must slide in a bore. Alternatively add a form tolerance such as straightness per ISO 1101:2017. On an ASME drawing the envelope is automatic; to relax it you add a note or modifier that says so.

The practical result: an ASME-trained engineer reading an ISO drawing may assume form is controlled when it is not. An ISO-trained engineer may add straightness tolerances that Rule #1 already implied.