How to Read GD&T: Start With the Datums

Suppose every two-point diameter reading on a shaft falls within Ø20 h7. The shaft can still be bowed enough to jam in its mating hole. Diameter tells you the distance between opposing points; it does not, by itself, tell you whether the shaft is straight, a face is square or a hole is correctly located.

Geometric dimensioning and tolerancing (GD&T) adds those missing controls. It specifies a feature's form, its orientation or location relative to datums, and, for rotating parts, its runout. ISO 1101 and ASME Y14.5 use similar symbols, but not always the same default rules. Check which standard the drawing names before interpreting a callout.

Read a feature control frame from left to right. Each compartment answers a different question.

Cell	Contents	Answers
First	Geometric characteristic symbol	What property is controlled?
Second	Tolerance value (may carry Ø and modifiers)	How much variation is allowed, and in what kind of zone?
Third onward	Datum letters (one to three)	Which references establish the measurement?

Ø changes the tolerance zone

A position tolerance of 0.1 and one of Ø0.1 are not interchangeable. Without Ø, the zone is between two parallel planes 0.1 apart. With Ø, it is a cylinder 0.1 in diameter around the true position. For a hole whose axis can shift in any radial direction, that cylindrical zone is usually what the designer intends.

Modifiers after the value

Symbol	Name	Meaning
Ⓜ	Maximum material requirement (MMR)	Departure from maximum material size may allow bonus tolerance
Ⓛ	Least material requirement (LMR)	Departure from least material size may allow bonus tolerance
Ⓕ	Free state	A non-rigid part is measured with no external force applied
Ⓟ	Projected tolerance zone	The zone extends outside the part, to control interference once a bolt is fitted
Ⓔ	Envelope requirement	Size and form considered together (must be stated explicitly under ISO)

The common controls fall into four families. A useful first question is whether the control needs a datum reference.

Family	Symbol and name	Datum required
Form	Straightness, flatness, roundness, cylindricity, line profile, surface profile	No (profile may or may not)
Orientation	Parallelism, perpendicularity, angularity	Yes
Location	Position, concentricity / coaxiality, symmetry	Yes
Runout	Circular runout, total runout	Yes

Form: judge the feature itself

Straightness, flatness, roundness and cylindricity describe the shape of a feature. Cylindricity controls the entire cylindrical surface, not just one cross-section. These controls normally need no datum because the comparison is against an ideal form of the feature itself.

Orientation and location: judge a relationship

Parallelism, perpendicularity and angularity describe how one feature is oriented to a datum. Position describes where a feature is relative to a datum system. Its ideal location comes from theoretically exact dimensions (TEDs), shown in boxes; the position callout supplies the allowable variation.

Runout: rotate the part

For circular runout, rotate the part about the datum axis and read an indicator at one cross-section. For total runout, sweep the indicator across the surface as the part turns. Both readings can reflect form error and eccentricity, making runout useful when the question is whether an assembled rotating part will wobble.

Datum letters are not an unordered list. A primary, secondary and tertiary datum establish a reference frame in that order. The sequence determines how the part is located for inspection.

1. The primary datum establishes the first reference, often a stable mounting face. In the familiar 3-2-1 example, three contacts constrain three degrees of freedom.
2. The secondary datum constrains two more degrees of freedom, often with two contacts.
3. The tertiary datum constrains the remaining degree of freedom, often with one contact.

This 3-2-1 model is a useful way to picture the setup, though actual datum simulators depend on the features and the governing standard. Reversing A|B|C to B|A|C can change the reference frame and therefore the reported measurement.

Choose a method that measures the specified characteristic and recreates the drawing's datum setup.

Characteristic	Common methods	Watch out for
Flatness	Surface plate and indicator, optical flat, CMM scan	Too few points and you will understate the error
Roundness	Roundness tester (rotating spindle), vee block and indicator	The vee-block method distorts on odd-lobed forms
Parallelism / perpendicularity	Square and indicator, CMM	The datum surface must be established first
Position	CMM, functional gauge (go gauge)	With Ⓜ applied, a functional gauge is the most direct check
Circular runout	Bench centres and indicator	How the datum axis is set up matters a great deal

• Using orientation to express a form requirement. Parallelism also limits flatness, but if the functional requirement is flatness itself, call it out explicitly.
• Choosing an unstable datum feature. A rough cast face may not locate the part repeatably. Select references that reflect assembly function and can be simulated consistently.
• Omitting Ø from a hole-position callout. A zone between two planes controls only one direction. If radial location matters, confirm that the intended zone is cylindrical.