GD&T is a language for saying what a part must do, not just how big it is. There are 14 geometric characteristics in ASME Y14.5 and ISO 1101, grouped into form, orientation, location, profile and runout. This guide walks all 14 from the inspection side — because a callout only counts if someone can measure it. For each symbol you get the meaning, the tolerance-zone shape, whether it needs a datum, and how we actually verify it with a CMM or a 3D scanner.
§ Reading a feature control frame
Every GD&T callout is a feature control frame read left to right in three parts: the geometric characteristic symbol, the tolerance zone (with any material condition modifier), and the datum references in order of precedence. A frame reading "position | Ø0.2 (M) | A | B | C" means: the axis of this feature must lie in a cylindrical zone 0.2 mm in diameter, that zone may grow as the feature departs from maximum material condition, and the zone is located relative to datum A first, then B, then C.
§ Form controls — no datum required
| Symbol | Controls | Tolerance zone | How it's inspected |
|---|---|---|---|
| Straightness | Line elements of a surface, or an axis | Two parallel lines (surface) or a cylinder (axis) | Scan a line of points along the feature; fit and measure peak-to-valley deviation |
| Flatness | A whole planar surface | Two parallel planes | Grid of points across the face; best-fit plane, then max deviation both ways |
| Circularity (roundness) | One cross-section of a round feature | Two concentric circles in that plane | Probe or scan a full circle at one height; least-squares circle, radial spread |
| Cylindricity | The whole cylindrical surface | Two concentric cylinders | Multiple circles at several heights plus axial lines; the strictest of the four |
Practical note: cylindricity simultaneously controls circularity, straightness and taper. It is powerful and expensive. Call it only where the function needs it — a hydraulic bore, a bearing journal — not on every turned diameter.
§ Orientation controls — always need a datum
| Symbol | Meaning | Tolerance zone | Inspection note |
|---|---|---|---|
| Perpendicularity | Feature is 90° to the datum | Two parallel planes, or a cylinder for an axis | Establish the datum plane first from real measured points, never from the table |
| Parallelism | Feature is parallel to the datum | Two parallel planes, or a cylinder | Very sensitive to a poorly established datum — a 0.01 mm datum error propagates directly |
| Angularity | Feature is at a specified basic angle | Two parallel planes at that angle | The angle is basic (boxed), the tolerance lives only in the frame |
§ Location controls
- Position — by far the most used and most useful control. Locates a feature's axis or centre plane within a cylindrical (or planar) zone from basic dimensions and datums. Replaces plus-minus dimensioning of hole patterns and gives you 57 % more tolerance area than a square zone of the same width.
- Concentricity — controls the median points of a feature relative to a datum axis. Hard to measure, rarely what you actually mean. In almost every case runout or position does the job better; ASME Y14.5-2018 removed it for this reason.
- Symmetry — the same story for median planes. Also removed in Y14.5-2018. Use position on the centre plane instead.
§ Profile controls — the universal tools
Profile of a line and profile of a surface are the two most versatile controls in the standard. Profile of a surface creates a uniform tolerance band that follows the true (basic) shape of the surface — and because it constrains form, orientation and location at once, it can legitimately replace several other callouts. With datums it locates the surface; without datums it controls form only. It is also the natural way to tolerance scanned and free-form geometry, because a 3D scanner produces exactly the deviation-from-nominal map that profile is defined in terms of.
- Profile of a surface — a 3D band, by default equally disposed (half in, half out) around the basic surface. Can be made unilateral or unequally disposed with the U modifier.
- Profile of a line — the same idea applied to individual cross-sections. Use it where the part may bow overall but each section must hold its shape, such as extrusions and sheet metal.
§ Runout controls
| Symbol | What it captures | Measurement |
|---|---|---|
| Circular runout | Circularity plus coaxiality, one cross-section at a time | Indicator fixed at one position, rotate the part 360°, read total indicator movement |
| Total runout | The entire surface: circularity, cylindricity, coaxiality, taper | Indicator traverses along the surface while the part rotates — one composite reading |
§ The modifiers that change everything
- MMC (M) — maximum material condition. Bonus tolerance is granted as the feature departs from MMC. Use for clearance holes and assembly fits; it is free tolerance for the shop and it still guarantees assembly.
- LMC (L) — least material condition. Protects minimum wall thickness and minimum edge distance.
- RFS — regardless of feature size. The default when no modifier is shown. No bonus tolerance.
- Ø — the tolerance zone is cylindrical rather than two parallel planes. Almost always what you want on a hole position.
- (P) projected tolerance zone — projects the zone above the surface, for threaded holes and press-fit pins where the mating fastener sticks out.
- (F) free state — the part is inspected unclamped, for thin, flexible or moulded parts.
§ Five callouts that make a part hard to inspect
- Datums on surfaces too small or too rough to establish a stable reference frame — the whole measurement inherits their instability.
- Concentricity or symmetry where runout or position would answer the same question in a fraction of the time.
- Tight flatness on a large thin part with no free-state note — it passes clamped and fails on the bench, or vice versa.
- Position on a threaded hole with no projected zone modifier — you have toleranced the hole, not the bolt that comes out of it.
- Profile tolerances tighter than the scanner or CMM uncertainty. As a working rule, the measurement system should consume no more than 10 – 20 % of the tolerance band.
§ Where to go next
Our reference library has the full symbol table with drawing callouts and inspection methods you can keep open on a second screen while you draft, plus an ISO 286 fits calculator for the size tolerances that sit alongside your geometric ones. If you want a second opinion on a specific frame, the GD&T Advisor tool walks you from the function of the feature to a defensible callout.
Was this helpful?
Take it further
Have a part like this? Or want to learn the workflow yourself?
