True Position GD&T

What True Position Controls

The GD&T position symbol (⊕) controls the location of a feature — typically the axis of a hole, pin, or cylinder — relative to specified datum references. The tolerance zone is a cylinder whose diameter equals the positional tolerance value stated in the feature control frame.

For example, the callout ⊕ ⌀0.1 | A | B | C means the axis of the hole must lie within a cylinder of diameter 0.1 mm, whose centreline is at the theoretically exact location as defined by datums A, B, and C. The basic (boxed) dimensions on the drawing locate this theoretical true position.

Cylindrical Zone vs ±XY: Which Gives More Tolerance?

This is the most practically important thing to understand about position tolerance. Consider a hole with the following options:

A ±0.05/±0.05 callout creates a square zone. The equivalent cylindrical position tolerance that fits inside that square has diameter ⌀0.1 mm (the side of the square). But the circumscribed circle of the same square has diameter ⌀0.141 mm — allowing 41% more movement in the diagonal direction. The GD&T zone is functionally correct because a pin fitting into a hole can deviate in any radial direction equally, not just in X or Y.

Maximum Material Condition (MMC) Bonus Tolerance

When the MMC modifier (Ⓜ) appears in the feature control frame, the stated position tolerance applies at the maximum material condition of the feature. As the feature departs from MMC toward least material condition (LMC), the positional tolerance increases by the same amount.

Example: A hole is sized 10.0 +0.3/−0.0 mm with position tolerance ⊕ ⌀0.2 Ⓜ | A | B.

This represents the physical reality: a larger hole can accommodate more mating pin positional error before the pin fails to clear. MMC callouts maximise yield by accepting parts that are functionally correct even when their position deviates more than the stated tolerance, provided they have the corresponding size departure.

Calculating True Position from CMM Data

Most CMM software calculates true position automatically, but understanding the arithmetic helps you interpret reports and catch errors. For a hole in 2D (XY plane):

Where ΔX and ΔY are the deviations from the theoretical true position coordinates. The result is the diameter of the smallest cylinder centred on true position that contains the actual axis.

Worked example: CMM measures hole centre at X = 50.05, Y = 30.08. True position is X = 50.00, Y = 30.00. ΔX = 0.05, ΔY = 0.08.

TP = 2 × √(0.05² + 0.08²) = 2 × √(0.0025 + 0.0064) = 2 × √0.0089 = 2 × 0.0943 = 0.189 mm

Compare 0.189 to the callout. If the callout is ⊕ ⌀0.2, the hole passes (0.189 < 0.200). For 3D position (X, Y, Z), add ΔZ² under the radical: TP = 2 × √(ΔX² + ΔY² + ΔZ²).

Inspection Without a CMM: Surface Plate Method

For simple hole patterns that reference a flat datum surface (Datum A) and two edge datums (B and C):

1. Clean and deburr the part. Place on the surface plate with datum A face down (use precision parallels if the surface is not datum A).
2. Use a height gauge or digital indicator on a height stand to locate datum B and C reference edges. Zero your height gauge to the true position Y-coordinate of the first hole.
3. Use a dial test indicator on a gauge pin inserted into the hole to find the actual hole centre. Read ΔY from the height gauge.
4. Rotate the part 90° (or use a second height gauge traverse) to find ΔX.
5. Calculate TP = 2 × √(ΔX² + ΔY²) and compare to the callout.

Setting Up Datums Correctly

Position tolerance is meaningless without correctly established datums. The three-datum (A, B, C) DRF (datum reference frame) establishes the 6 degrees of freedom needed to fully locate a feature. Common setup errors:

• Using a datum surface that isn't flat: Cast and forged surfaces need machined datum pads. Clamping directly to a rough surface introduces angular error that is indistinguishable from position error.
• Reversing datum precedence: If the drawing calls |A|B|C|, datum A is the primary datum (3-point contact), B is secondary (2-point), C is tertiary (1-point). Reversing them changes which degrees of freedom are constrained first.
• Not using the same datum for machining and inspection: If you machine the hole from datum A on the machine but inspect it referencing datum B, you are measuring a different DRF than the one that controlled the cut.