Geometric dimensioning and tolerancing

Why it matters

Size tolerances (limits and fits) say nothing about whether a surface is flat, a bore is round or a hole is in the right place. Geometric dimensioning and tolerancing (GD&T) adds that missing information in a precise symbolic language, so the designer, machinist and inspector all read the same functional requirement. Used well, it opens up tolerances where function allows, which cuts manufacturing cost without risking assembly.

Key ideas

Feature and feature of size. A feature is a physical surface, hole, slot or pin. A feature of size has an opposed pair of surfaces with a size dimension (a hole, a shaft, a slot width); only features of size can carry material-condition modifiers.

The geometric characteristics (ASME Y14.5 / ISO 1101, IS 8000) fall into five groups:

• Form (no datum): straightness, flatness, circularity (roundness), cylindricity.
• Orientation (needs a datum): parallelism, perpendicularity (squareness), angularity.
• Location (needs datums): position; concentricity and symmetry exist in ISO but were withdrawn from the 2018 ASME standard in favour of position, runout or profile.
• Profile: profile of a line, profile of a surface (with or without datums).
• Runout (needs a datum axis): circular runout and total runout.

Tolerance zone. Each control defines a zone inside which the feature must lie: two parallel planes for flatness, two coaxial cylinders for cylindricity, two concentric circles for circularity, a cylinder of diameter t for the position of an axis (when the tolerance has a Ø symbol).

Feature control frame. A rectangular box read left to right: geometric symbol | tolerance value (with Ø if the zone is cylindrical) and any modifier | primary, secondary and tertiary datum letters. Example: position | Ø0.1 Ⓜ | A | B | C.

Datums and the datum reference frame. Datum features on the part (marked A, B, C) are simulated by precise inspection surfaces. The primary datum plane contacts the part at a minimum of three points, the secondary at two, the tertiary at one — the 3-2-1 principle that removes all six degrees of freedom. Measurement repeats only if everyone uses the same datum order.

Basic dimensions. True (theoretically exact) locations are given by boxed basic dimensions with no tolerance of their own; the tolerance lives in the feature control frame.

Material condition modifiers.

• MMC (Ⓜ): maximum material — smallest hole, largest shaft.
• LMC (Ⓛ): least material — largest hole, smallest shaft.
• RFS: regardless of feature size, the default in current standards when no modifier is shown; the geometric tolerance is fixed.

Bonus tolerance. When a geometric tolerance is specified at MMC, the allowed geometric tolerance increases by the amount the actual size departs from MMC towards LMC. For a hole that means the hole being larger than its minimum; for a shaft, smaller than its maximum. Physically, a larger hole has more room to move and still accept the mating pin, so assembly is not harmed.

Virtual condition. The worst-case boundary created by MMC size plus the geometric tolerance at MMC. It is the size of the pin on a functional (receiver) gauge used to check position at MMC.

Rule #1 (envelope principle, ASME). For a feature of size with no other note, the form must lie within a perfect-form envelope at MMC. ISO's default is the independency principle unless Ⓔ is used — check which standard the drawing follows.

Formulas

Positional deviation (diametral) = 2·√(Δx² + Δy²)

• Δx, Δy: measured minus basic (true) coordinates of the axis, mm. The result is the diameter of the smallest zone centred on true position that contains the axis; compare it with the Ø position tolerance.

Bonus (hole) = actual hole size − MMC size of hole Bonus (shaft) = MMC size of shaft − actual shaft size

Allowed position tolerance = stated tolerance at MMC + bonus

Virtual condition (hole) = MMC size − geometric tolerance at MMC Virtual condition (shaft) = MMC size + geometric tolerance at MMC

• All in mm. Bonus formulas apply only when Ⓜ is shown; with RFS the bonus is zero.

Worked examples

Example 1 (standard): is the hole in position?

Given: basic location (10.0, 20.0) mm, measured axis (10.2, 20.3) mm, position tolerance Ø0.5 mm RFS.

1. Δx = 10.2 − 10.0 = 0.2 mm, Δy = 20.3 − 20.0 = 0.3 mm.
2. Positional deviation = 2·√(0.2² + 0.3²) = 2·√0.13 = 2 × 0.3606 = 0.721 mm.
3. Compare: 0.721 mm > 0.5 mm.

Positional deviation Ø0.721 mm — the hole is rejected.

Example 2 (GATE level): bonus tolerance and the functional gauge.

Given: hole size limits 10.0 to 10.2 mm; position Ø0.1 Ⓜ relative to A|B|C. Inspected hole: actual size 10.12 mm, axis offsets Δx = 0.08 mm, Δy = 0.06 mm.

1. MMC of the hole = smallest size = 10.0 mm. Size 10.12 mm lies within 10.0–10.2, so size is acceptable.
2. Bonus = 10.12 − 10.0 = 0.12 mm.
3. Allowed position tolerance = 0.1 + 0.12 = 0.22 mm.
4. Positional deviation = 2·√(0.08² + 0.06²) = 2 × 0.10 = 0.20 mm.
5. 0.20 ≤ 0.22, so the hole passes (it would have failed with RFS, where only 0.1 mm is allowed).
6. Functional gauge pin = virtual condition: 10.0 − 0.1 = 9.9 mm.

Allowed tolerance Ø0.22 mm, actual Ø0.20 mm: accept. Gauge pin Ø9.9 mm.

Common mistakes

• Reporting √(Δx² + Δy²) as the positional deviation. A diametral zone needs twice the radial offset.
• Treating MMC of a hole as its largest size. MMC is the condition with most material: smallest hole, largest shaft.
• Claiming bonus with RFS, or on a feature that is not a feature of size (a flat surface cannot have Ⓜ).
• Ignoring datum order. Changing primary and secondary datums changes how the part is held and the measured result.
• Confusing circularity (a cross-section check, no datum) with circular runout (rotation about a datum axis, which also picks up eccentricity).
• Thinking a form tolerance can be larger than the size tolerance under the envelope rule; it cannot exceed it.

For GATE PI

Expect symbol identification (which characteristic is form, orientation, location or runout, and which need datums), interpretation of a feature control frame, and short numericals on positional deviation, bonus tolerance at MMC and virtual condition. Practise quickly deciding MMC and LMC for holes and shafts, and always check size before checking position.

Quick check

1. Which four characteristics are pure form controls?
2. A shaft is Ø20.0–Ø19.9 mm with straightness Ø0.05 Ⓜ. What is its virtual condition?
3. Axis offsets are Δx = 0.03 mm and Δy = 0.04 mm. What is the positional deviation?
4. How many points of contact does the primary datum plane need?

Answers: 1. Straightness, flatness, circularity, cylindricity. 2. 20.0 + 0.05 = 20.05 mm. 3. 2 × 0.05 = Ø0.10 mm. 4. Three.