1. Summary of geometric characteristic symbols
| Category | Characteristic | Symbol | Tolerance zone / measurement notes |
|---|---|---|---|
| Form (no datum) | Straightness | — | Two parallel lines or planes; straight edge with feeler gauge, or dial indicator |
| Flatness | ▱ | Two parallel planes; surface plate plus dial indicator on a grid | |
| Roundness | ○ | Two concentric circles; roundness tester or CMM | |
| Cylindricity | ⌭ | Two coaxial cylinders; roundness tester | |
| Orientation (datum required) | Parallelism | ∥ | Parallel to the datum; surface plate and dial indicator |
| Perpendicularity | ⊥ | Perpendicular to the datum; square or dial indicator | |
| Angularity | ∠ | Deviation from the true angle; sine bar | |
| Location (datum required) | Position | ⌖ | Circle, sphere or zone; position gauge or CMM |
| Concentricity | ◎ | Cylinder coaxial with the datum; dial-indicator setup or CMM | |
| Symmetry | ≡ | Symmetrically distributed about the datum; indicate and compare before and after flipping | |
| Runout | Circular runout | ↗ | Read the maximum difference over one revolution; dial indicator setup |
| Total runout | ↗↗ | Maximum difference over a continuous full-surface reading | |
| Profile | Profile of a line / surface | ⌒ | Envelope of perfect form; template or CMM |
2. Tolerance principles (modifiers in the feature control frame)
| Symbol | Principle | Meaning |
|---|---|---|
| (no symbol) | Independence principle | Size and geometric tolerances are satisfied independently — the default principle |
| Ⓔ | Envelope requirement | The actual feature must not exceed the maximum material boundary (MMC); common on mating bores and shafts |
| Ⓜ | Maximum material requirement (MMR) | Bonus from departing MMC; common on position and concentricity |
| Ⓛ | Least material requirement (LMR) | Bonus from departing LMC; used where minimum wall thickness matters |
| Ⓟ | Projected tolerance zone | Zone projected beyond the part surface (ensures stud or pin assembly) |
Reading a datum callout
- Single datum: shown in the frame is "A".
- Compound datum:"A-B" — two features combined into a single datum.
- Datum system:"B / A / C" three-plane datum system: the primary datum constrains the most, and inspection must simulate them in that order.
3. Position tolerance Q&A (key section)
What exactly is position tolerance?
Position tolerance controls the the deviation of the actual position from its true position. The ideal position is defined by Theoretically exact dimensions (TED — boxed, e.g. [40]) and the datum. For a hole the zone is normally a cylinder centred on the true position (Φ0.2 means a 0.2 mm diameter circle), and the actual axis must lie entirely inside it.
Why is position tolerance recommended for hole patterns instead of ±0.1 on the hole spacing?
Three reasons:① Shape of the tolerance zone— coordinate tolerancing gives a square tolerance zone, position tolerance gives a circular one; for the same "0.1 at the extreme point", the circular zone is about 57% larger, handing the "wasted" diagonal clearance back to the process.② No tolerance accumulation— coordinate hole spacing is a chain of dimensions, so the error of each hole accumulates from the previous one; with position tolerance every hole is measured from the same true position and errors do not accumulate.③ Consistent with assembly— for a clearance hole all that matters is how far the axis sits from its ideal position, which is exactly what position tolerance defines.
What does Ⓜ (the circled M) in a position frame mean, and how is the bonus calculated?
Ⓜ = maximum material requirement: when the hole is actually machined larger than at MMC (the worst assembly condition, i.e. the smallest hole), so the position tolerance gains an equal bonus.
Worked example: Drawing calls out 4×Φ10+0.1/0, position Φ0.2 Ⓜ, datum A.
① Hole at MMC = Φ10.00 → position tolerance Φ0.2;
② If a hole is actually made Φ10.05 (0.05 away from MMC), the permitted position tolerance for that hole is Φ0.2 + 0.05 = Φ0.25;
③ At the largest hole, Φ10.1, the position tolerance may reach Φ0.3.
Meaning: the larger the hole, the easier it assembles — the position may loosen by exactly that much, but The assembly boundary (virtual condition Φ9.8 = MMC − position tolerance) never changes, so function is never compromised.
Worked example: Drawing calls out 4×Φ10+0.1/0, position Φ0.2 Ⓜ, datum A.
① Hole at MMC = Φ10.00 → position tolerance Φ0.2;
② If a hole is actually made Φ10.05 (0.05 away from MMC), the permitted position tolerance for that hole is Φ0.2 + 0.05 = Φ0.25;
③ At the largest hole, Φ10.1, the position tolerance may reach Φ0.3.
Meaning: the larger the hole, the easier it assembles — the position may loosen by exactly that much, but The assembly boundary (virtual condition Φ9.8 = MMC − position tolerance) never changes, so function is never compromised.
How is position tolerance inspected?
① Position gauge (functional gauge): a functional gauge built to MMC plus the tolerance zone gives a go/no-go verdict in one pass — the fastest option on the floor; ② CMM: measure the hole centre (x, y), compare it with the true position; position error = 2×√(Δx² + Δy²), then subtract the Ⓜ bonus before judging; ③ Vision system / profile projector: on sheet-metal parts measure the hole centre directly by vision. Note that datum A must be simulated as the primary datum (three-point or full-face contact) — a wrong datum simulation makes every number wrong.
How are theoretically exact dimensions (TED) given when calling out position tolerance?
All hole spacing uses Boxed dimension (e.g. [50] [25]) relative to the datum, with no tolerance of their own — all of it already sits in the position frame. A common mistake is giving both boxed dimensions and ± tolerances, which duplicates the control.
In one sentence: Position tolerance = where the hole should be (set by TED) + how far it may deviate (set by the frame) + how much extra is granted as the hole grows (set by the Ⓜ modifier).
4. Reference geometric tolerance values (GB/T 1184 accuracy grades)
| Grade | Typical applications |
|---|---|
| Grades 1–3 | Precision machine spindles, metrology guideways and similar high-accuracy parts |
| Grades 4–6 | General machine spindles, bearing fits, engine bores |
| Grades 7–9 | General drive shafts, pump and gearbox joint faces (most common) |
| Grades 10–12 | Low-precision non-functional faces, welded structures |
Geometric and size tolerances should be of the same order of magnitude: on an IT7 bore or shaft fit, the geometric tolerance is typically 1/2 to 1/3 of the size tolerance.