Mechanical and GD&T symbols

Why it matters

Plus/minus tolerances control size, but they do a poor job of controlling form (is it flat?), orientation (is it square?) and location (is the hole where it should be relative to the surfaces that matter?). Geometric Dimensioning and Tolerancing (GD&T) solves this with a compact symbolic language. Mechanical engineers, machinists, inspectors and maintenance mechanics all meet it on prints.

In the US the standard is ASME Y14.5 (current edition 2018); internationally, ISO GPS standards such as ISO 1101 cover similar ground with some differences. Check which one the title block references.

The feature control frame

A GD&T requirement is written in a feature control frame, a row of boxes attached to the feature:

[ ⌖ | Ø0.2 Ⓜ | A | B | C ]

Read it left to right:

1. Geometric characteristic symbol (here ⌖, position).
2. Tolerance zone: Ø means the zone is a cylinder 0.2 mm in diameter; no Ø means a zone between two parallel lines or planes.
3. Material condition modifier (optional): Ⓜ maximum material condition (MMC), Ⓛ least material condition (LMC). No modifier means "regardless of feature size".
4. Datum references in order of priority: primary A, secondary B, tertiary C.

"The axis of this hole must lie within a 0.2 mm diameter cylinder at MMC, located relative to datums A, B and C."

The characteristics, by group

ASME Y14.5-2018 lists 12 characteristics; older editions also had concentricity and symmetry, which you will still see on older prints.

Datums

A datum is a theoretically exact reference: a plane, axis or point. The datum feature is the real surface on the part that establishes it, marked with a datum feature symbol (a letter in a box attached to a triangle on the surface, for example A).

The order in the frame matters. A typical part sits on datum A (the primary plane, three points of contact), is pushed against B (two points), and then against C (one point): the 3-2-1 principle. Inspection fixtures copy this setup.

Basic dimensions

Dimensions in a rectangular box are basic: theoretically exact values with no tolerance of their own. The GD&T frame supplies the tolerance. A hole located by boxed 25 and 40 from datums B and C, with a position tolerance of Ø0.2, must have its axis inside a 0.2 mm cylinder centred at exactly (25, 40).

Worked example: bonus tolerance at MMC

A hole is sized Ø10.0 to Ø10.2 with position Ø0.2 Ⓜ to A, B, C.

• For a hole, MMC is the smallest size (most material left): Ø10.0.
• At MMC, the position tolerance is Ø0.2.
• If the hole is made at Ø10.1, it is 0.1 away from MMC, and that departure is added as bonus tolerance: Ø0.2 + 0.1 = Ø0.3.
• At the largest size, Ø10.2, the position tolerance becomes Ø0.4.

This makes sense functionally: a bigger hole can be slightly further out of place and a bolt will still fit. That is why Ⓜ is common on clearance holes.

Other mechanical symbols

• Threads: metric M8×1.25-6H (8 mm nominal, 1.25 mm pitch, tolerance class 6H for an internal thread); unified inch 1/4-20 UNC-2B (1/4 in, 20 threads per inch, coarse, class 2B internal). Threads are usually drawn simplified, with a dashed or thin line for the thread depth.
• Surface texture: a check-mark symbol with a value, for example Ra 1.6 (μm), meaning average roughness. A bar across the top means material must be removed by machining.
• Welding symbols (AWS A2.4): a reference line with an arrow; symbols below the line apply to the arrow side, above the line to the other side. A triangle is a fillet weld.
• Chamfer: 2 × 45°. Fillet/round: R3.
• Section and detail views: a circle labelled DETAIL B, scaled up, for small features.

Common mistakes

• Reading the datum order as alphabetical rather than as written in the frame.
• Forgetting that boxed (basic) dimensions have no plus/minus.
• Treating the Ø in the frame as the hole size; it describes the shape of the tolerance zone.
• Applying bonus tolerance when there is no Ⓜ modifier.
• Mixing ASME and ISO rules on one print.

Official source

• ASME Y14.5 Dimensioning and Tolerancing: https://www.asme.org/codes-standards/find-codes-standards/y14-5-dimensioning-tolerancing

Checked on 2026-10-23.

Recap

• A feature control frame reads: characteristic, zone (Ø = cylindrical), modifier, datums in priority order.
• Groups: form, orientation, location, profile, runout.
• Basic dimensions are exact; the frame gives the tolerance.
• At MMC, a hole gets bonus tolerance as it grows from its smallest size.