GD&T symbols explained

Every line element of a surface — or the derived axis when applied to a feature of size — must lie within the stated zone.

Tolerance zone

Two parallel lines (surface) or a cylinder (axis / feature of size)

When to use it

Long shafts, guide rails, pins that must slide. Applied with (M) to an axis it becomes a functional straightness-of-axis control.

How it's inspected

Surface plate + dial indicator sweep, or a scanned mesh evaluated line-by-line in Control X / PolyWorks.

Common mistake

Calling out surface straightness when the real requirement is a straight axis. They are different controls.

All points of the surface must sit between two parallel planes the stated distance apart.

Tolerance zone

Two parallel planes

When to use it

Mating faces, gasket seats, machine bases, anything that must not rock or leak.

How it's inspected

Best-fit plane through the scanned surface, then max peak-to-valley deviation. This is the single easiest GD&T control to verify from 3D scan data.

Common mistake

Measuring flatness against a datum. Flatness never references a datum — it is a self-contained form control.

Each individual cross-section of a round feature must fall between two concentric circles.

Tolerance zone

Two concentric circles in any cross-section

When to use it

Bearing journals, seal running surfaces, rollers.

How it's inspected

Roundness tester, or section the scan perpendicular to the fitted axis and evaluate each slice separately.

Common mistake

Assuming a diameter tolerance already controls roundness. A two-point measurement cannot detect lobing.

The whole cylindrical surface — roundness, straightness and taper together — must lie between two coaxial cylinders.

Tolerance zone

Two coaxial cylinders

When to use it

Hydraulic bores, precision bushings, anything where a shaft must run the full length.

How it's inspected

Fit a cylinder to the full scanned surface and report the radial deviation band.

Common mistake

Over-specifying it. Cylindricity is expensive; often circularity plus straightness is enough.

Each 2D cross-section of the surface must lie inside a band around the nominal curve.

Tolerance zone

Two curves offset from the true profile, in a stated cross-section

When to use it

Extruded shapes, airfoil sections, sheet-metal cross-sections.

How it's inspected

Cross-section the scan on the drawing plane and compare to the CAD curve.

Common mistake

Using it where the whole 3D surface actually matters — use profile of a surface instead.

The entire surface must lie inside a 3D band around the nominal geometry. Can control form, orientation and location at once.

Tolerance zone

Two surfaces offset from the true (CAD) surface

When to use it

The workhorse of reverse-engineered and organic parts: castings, impellers, blades, ergonomic housings.

How it's inspected

Deviation colour map against CAD in Geomagic Control X or PolyWorks, aligned to the datum reference frame.

Common mistake

Leaving the datums off. Without datums it is a form-only control and will pass parts that are in the wrong place.

The feature must be square to the datum within the stated zone.

Tolerance zone

Two parallel planes (surface) or a cylinder (axis) at 90° to the datum

When to use it

Bolt-hole axes to a face, machined shoulders, fixture locating surfaces.

How it's inspected

Establish the datum plane from the scan, then measure the angular deviation of the feature.

Common mistake

Assuming a 90° basic angle plus a linear tolerance controls squareness. It does not.

The feature must hold the stated basic angle relative to the datum.

Tolerance zone

Two parallel planes at the basic angle to the datum

When to use it

Ramps, dovetails, angled mounting faces, chamfered seats.

How it's inspected

Fit a plane to the feature and measure the angle to the datum plane.

Common mistake

Dimensioning the angle with a ± tolerance and an angularity callout at the same time.

The feature must stay parallel to the datum within the zone — orientation only, not location.

Tolerance zone

Two parallel planes (or a cylinder) parallel to the datum

When to use it

Slide ways, opposing clamp faces, stacked plates.

How it's inspected

Fit the feature, fit the datum, evaluate the angular error over the feature length.

Common mistake

Expecting parallelism to control the distance between the faces — that is the size dimension's job.

The feature's axis or centre plane must lie within a zone centred on the theoretically exact location defined by basic dimensions.

Tolerance zone

A cylinder (or two parallel planes) centred on the true position

When to use it

Bolt patterns, dowel holes, connector cut-outs — by far the most-used location control.

How it's inspected

Align the scan to the datum reference frame, fit each hole axis, report the radial deviation from true position.

Common mistake

Mixing basic dimensions with ± dimensions in the same pattern, which creates ambiguous tolerance stack-up.

The median points of the feature must lie within a cylinder about the datum axis.

Tolerance zone

A cylinder centred on the datum axis, applied to derived median points

When to use it

Rare. Deprecated in ASME Y14.5-2018 — use position or runout instead unless mass balance is genuinely the requirement.

How it's inspected

Requires derived median point evaluation; slow and expensive on a CMM.

Common mistake

Using it where runout would do the job at a fraction of the inspection cost.

The median plane of the feature must lie within the zone about the datum centre plane.

Tolerance zone

Two parallel planes centred on the datum centre plane

When to use it

Rare, and also deprecated in ASME Y14.5-2018. Position on a centre plane is the modern equivalent.

How it's inspected

Derived median plane evaluation from opposing surface points.

Common mistake

Using it as shorthand for 'centred'. Position handles that better and is easier to verify.

Combines circularity and coaxiality for each individual cross-section.

Tolerance zone

Full indicator movement in one cross-section, part rotated about the datum axis

When to use it

Rotating shafts, pulley seats, gear blanks — the cheapest useful control on turned parts.

How it's inspected

Rotate on centres with a dial indicator, or simulate rotation from the scan about the fitted datum axis.

Common mistake

Applying it to a non-rotating feature where position would communicate the requirement better.

Controls circularity, straightness, taper and coaxiality over the whole feature simultaneously.

Tolerance zone

Full indicator movement across the entire surface during rotation

When to use it

Long bearing journals, brake rotors, seal faces where the full surface must run true.

How it's inspected

Indicator traversed along the surface while rotating, or full-surface deviation about the datum axis in the scan.

Common mistake

Specifying total runout where circular runout is sufficient — it multiplies machining cost.