What is True Position in GD&T?
Under ASME Y14.5 and ISO 1101, Position (often called True Position) defines the allowable deviation of a feature of size (such as a drilled hole, threaded insert, pin, or slot) from its theoretically exact location established by basic dimensions and datums.
Unlike traditional plus/minus bilateral tolerances that form rectangular coordinate tolerance zones, True Position establishes a cylindrical (or diametrical) tolerance zone centered at the exact theoretical coordinate. This delivers 57% more usable tolerance area compared to rectangular coordinate tolerancing while ensuring 100% functional mating part assembly.
Sample Feature Control Frame: Position tolerance zone of 0.25 mm diameter at Maximum Material Condition (MMC) relative to primary Datum A, secondary Datum B, and tertiary Datum C.
How to Calculate True Position from Measured Coordinates
When inspecting a drilled hole or machined pin using a Coordinate Measuring Machine (CMM) or optical measurement system, the actual measured coordinates $(X_{act}, Y_{act})$ rarely land exactly on the nominal basic print dimensions $(X_{basic}, Y_{basic})$.
The deviations along the primary coordinate axes are:
ΔY = Y_actual - Y_basic
Because True Position specifies a diametrical (full diameter) cylindrical tolerance zone rather than a radial zone, the radial deviation must be multiplied by 2:
Step-by-Step Calculation Example:
Assume a drawing specifies a hole location at basic coordinates $X = 50.00\text{ mm}$ and $Y = 30.00\text{ mm}$ with a position tolerance of ⌀ 0.20 mm.
- CMM Measured Location: $X_{act} = 50.06\text{ mm}$, $Y_{act} = 29.93\text{ mm}$
- Deviation in X: $\Delta X = 50.06 - 50.00 = +0.06\text{ mm}$
- Deviation in Y: $\Delta Y = 29.93 - 30.00 = -0.07\text{ mm}$
- Radial Distance: $\sqrt{(0.06)^2 + (-0.07)^2} = \sqrt{0.0036 + 0.0049} = \sqrt{0.0085} \approx 0.0922\text{ mm}$
- Actual Position: $2 \times 0.0922 = \mathbf{0.1844\text{ mm}}$
Verdict: Because the actual position ($0.184\text{ mm}$) is less than or equal to the drawing callout ($0.20\text{ mm}$), the feature is conforming.
Maximum Material Condition (MMC) & Bonus Tolerance
When the Maximum Material Condition modifier symbol (Ⓜ) appears in the tolerance block of a feature control frame, it introduces the concept of Bonus Tolerance.
Maximum Material Condition (MMC) represents the state of a feature where it contains the maximum amount of material within its stated size limits:
- For an Internal Feature (Hole or Slot): MMC is the smallest allowable hole diameter.
- For an External Feature (Pin, Shaft, or Boss): MMC is the largest allowable pin diameter.
Total Allowable Position = Drawing Tolerance + Bonus Tolerance
Example: Hole Tolerance with MMC Bonus
Drawing Callout: ⌀ 10.00 ± 0.10 mm, with Position ⌖ | ⌀ 0.15 Ⓜ | A | B | C |
| Actual Hole Size | Condition | Bonus Tolerance | Total Allowed Position |
|---|---|---|---|
| ⌀ 9.90 mm | At MMC (Smallest Hole) | 0.00 mm | ⌀ 0.15 mm |
| ⌀ 9.95 mm | Departure from MMC | +0.05 mm | ⌀ 0.20 mm |
| ⌀ 10.00 mm | Nominal Hole Size | +0.10 mm | ⌀ 0.25 mm |
| ⌀ 10.10 mm | At LMC (Largest Hole) | +0.20 mm | ⌀ 0.35 mm |
Notice that if the machinist drills the hole at ⌀ 10.10 mm (still within size tolerance), the allowable position tolerance increases from ⌀ 0.15 mm to ⌀ 0.35 mm — more than doubling the manufacturing window without compromising mating assembly!
Inspection Methods: Functional Gages vs CMM
Verifying True Position can be performed via two main methods depending on production volume:
1. Hard Functional Gaging (Go Gages)
When MMC is specified, the physical interface can be verified using a fixed-pin attribute gage. The virtual condition pin diameter is calculated as:
If the functional gage pin enters the manufactured hole, the part is 100% guaranteed to assemble with the mating component in production.
2. Coordinate Measuring Machine (CMM)
Modern quality inspection uses touch-trigger or continuous scanning probes on a CMM. The software establishes the datum coordinate system (DRF), measures the feature centroid, calculates $\Delta X$ and $\Delta Y$, measures the feature diameter, and calculates actual position and bonus tolerance automatically.
Top 3 Common Mistakes in True Position Inspection
- Applying Bonus to Non-Size Features: The Ⓜ modifier can only be applied to features of size (cylinders, spheres, parallel slots). It cannot be applied to planar surfaces or line profiles.
- Neglecting Datum Precedence: Measuring position without adhering strictly to the primary, secondary, and tertiary datum alignment sequence invalidates CMM alignment results.
- Failing to Multiply Radial Deviation by 2: In manual quality reporting, inspectors sometimes record $\sqrt{\Delta X^2 + \Delta Y^2}$ instead of doubling it for the diametrical zone, erroneously reporting an in-spec part as defective.
Automate GD&T Characteristic Numbering on Blueprints
BalloonPlot AI automatically reads feature control frames, basic dimensions, and datum references directly from PDF engineering drawings, generating complete inspection plans without manual data entry.