Why size tolerances are not enough: the case for GD&T

A dimension with a plus/minus tolerance answers one question: how big is this feature? It does not say whether a pin is straight or a face is flat. Nor does it say whether a bore is square to the face it sits in, or which edge a hole is measured from. On a simple part a good machinist fills those gaps with habit. On a part that must assemble with parts from another supplier, the gaps become arguments, concessions and scrap.

Geometrical tolerancing (US: geometric dimensioning and tolerancing, GD&T) closes the gaps. You will meet two rulebooks for it. ISO 1101:2017 sits inside the ISO GPS (geometrical product specifications) system, which BS 8888 applies to UK practice. The US uses ASME Y14.5-2018 (R2024).

What a plus/minus tolerance cannot tell you

A size dimension leaves most functional requirements open. Each row below is a real one, with what ± dimensions say about it and what they leave open.

Functional requirement	What ± dimensions say	What they leave open	GD&T control (lesson)
A pin must enter a bore	Pin and bore diameter limits	Bow, taper and lobing of the pin (under ISO defaults)	Envelope requirement, straightness, cylindricity (1, 3)
A face must seat without rocking	Thickness of the part	Warp and twist of the face	Flatness (3)
A bore must be square to its mounting face	Nothing	Tilt of the bore axis	Perpendicularity (3)
A bolt hole must line up with its partner	±x and ±y from two edges	Which edge comes first; a square zone; how the part is held to measure	Position with datums (2, 4)
A shaft must run true in its bearings	Each diameter	Offset between diameters	Run-out (5)
A curved surface must match a mating contour	Coordinates of a few points	The surface between the points	Profile of a surface (5)

None of these gaps is a drafting error. Size tolerances cannot state shape, orientation or a measuring origin.

A bent pin that passes inspection

Take a pin toleranced Ø10 0/−0.05 mm on an ISO drawing. ISO 8015:2011 applies the independency principle: every requirement is met on its own. A size tolerance then controls local size only: the two-point diameter measured across any cross-section. A pin that is 9.97 mm at every section passes, however much it bows.

ASME Y14.5 takes the opposite default. Its Rule #1 (the envelope principle) says the limits of size of a regular feature of size also control its form. At maximum material condition (MMC), 10.00 mm for this pin, the feature must have perfect form. The same bowed pin is rejected on an ASME drawing. An ISO designer gets the same protection only by asking for it: with the envelope requirement symbol Ⓔ after the size (ISO 14405-1:2025) or with an explicit form tolerance.

Plus/minus location gives a square zone

Locate a hole with 40 ±0.1 mm from the left edge and 25 ±0.1 mm from the bottom edge. Its axis may then lie anywhere in a 0.2 × 0.2 mm square. Along the axes it may move 0.1 mm; at a corner it may move

$$r_{\text{corner}} = \sqrt{0.1^2 + 0.1^2} = 0.141\ \text{mm}$$

The mating bolt does not care which direction the error goes, so the square is unfair. It rejects a hole 0.12 mm off along one axis but accepts one 0.14 mm off on the diagonal. A round zone through the corners, Ø0.283 mm, accepts every part that works and has 57% more area:

$$\frac{\pi \times 0.283^2 / 4}{0.2^2} = \frac{0.0628}{0.04} = 1.57$$

Plus/minus dimensions from two edges have a second, quieter problem. They do not say which edge the part is set up on first. Nor do they say what happens if the edges are not square to each other. Two inspectors can measure the same hole and disagree. Position tolerancing fixes both problems with a cylindrical zone and a datum reference frame; lesson 4 works through it with numbers.

What GD&T adds to a drawing

Ingredient	What it does	How it appears
Geometrical characteristic	Names what is controlled: form, orientation, location, run-out or profile	A symbol in the first cell of the frame
Tolerance zone	Defines the shape and size of the space the feature must lie in	The value, with Ø for a cylindrical zone
Datums	Fix the zone in space and define how the part is held to measure it	Datum letters in the frame, datum feature symbols on the part
Theoretically exact dimensions (US: basic dimensions)	Give the perfect location or shape of the zone; they carry no tolerance of their own	A boxed dimension
Modifiers	Change the rule, for example Ⓜ for maximum material, Ⓔ for envelope	Symbols after the value or a datum letter

All of this sits in the feature control frame (ISO calls it the tolerance indicator), which lesson 6 reads cell by cell.

The GD&T symbols, grouped by type

ISO 1101:2017 defines 14 symbols (concentricity and coaxiality share one). ASME Y14.5-2018 has 12, because it withdrew concentricity and symmetry and directs users to position, run-out or profile. ASME treats profile as its own group; ISO classes a profile tolerance as form, orientation or location depending on whether it references datums.

The chart tells you what the symbols look like. The table below tells you how to use them, which is what a checker will ask about.

Characteristic	Group	ISO 1101:2017	ASME Y14.5-2018	Datum reference	What it controls
Straightness	Form	Yes	Yes	Never	Line elements of a surface, or an axis
Flatness	Form	Yes	Yes	Never	A nominally flat surface
Roundness (US: circularity)	Form	Yes	Yes	Never	Each circular cross-section
Cylindricity	Form	Yes	Yes	Never	Roundness, straightness and taper of the whole cylinder together
Profile of a line	Profile	Yes	Yes	Optional	Each cross-section of a curved surface
Profile of a surface	Profile	Yes	Yes	Optional	Any surface: form alone, or with orientation and location when datums are cited
Parallelism	Orientation	Yes	Yes	Always	Surface or axis parallel to a datum
Perpendicularity	Orientation	Yes	Yes	Always	Surface or axis at 90° to a datum
Angularity	Orientation	Yes	Yes	Always	Surface or axis at any stated angle to a datum
Position	Location	Yes	Yes	Usually	Axis, median plane or (ISO) surface relative to datums and exact dimensions
Concentricity, coaxiality	Location	Yes	Removed	Always	Centre point or axis relative to a datum axis
Symmetry	Location	Yes	Removed	Always	Median plane relative to a datum plane
Circular run-out	Run-out	Yes	Yes	Always	Each circular element as the part turns about the datum axis
Total run-out	Run-out	Yes	Yes	Always	The whole surface as the part turns about the datum axis

The pattern is worth memorising: form never takes a datum, orientation and run-out always do, and location almost always does. Profile is the flexible one.

How the rest of this module builds on this

Lesson	Question it answers
2 Datums and datum reference frames	Measured from where, and with the part held how?
3 Form and orientation tolerances (from 6 October 2026)	How flat, straight, round, parallel or square?
4 Position, MMC and bonus tolerance (from 6 October 2026)	Where is the hole, and how much extra tolerance does a bigger hole earn?
5 Profile and run-out (from 13 October 2026)	How close to the true shape, and how true does it spin?
6 Reading a feature control frame (from 13 October 2026)	What does every cell mean, in ISO and in ASME?

If your drawings mostly carry general tolerances today, Module 1, lesson 4 covers them in more depth. It explains the ISO 2768 fallback and the independency versus Rule #1 split. Geometrical tolerances also feed stack-ups. A position or perpendicularity tolerance is one more contributor in the loop, and the tolerance stack-up calculator takes it as a line like any other.