True Position with MMC / LMC Bonus.
Compute true position from X/Y deviations. Apply MMC or LMC modifiers to get bonus tolerance from feature size deviation. ASME Y14.5 compliant.
Feature type
Material condition modifier
Drawing call-out
Measured
Bonus tol (MMC, hole) = Actual − Smallest hole
Bonus tol (MMC, pin) = Largest pin − Actual
Total allowed ⌀ = Stated tol + Bonus
What is Position Tolerance?
True position is a GD&T (Geometric Dimensioning and Tolerancing) callout that controls the location of a feature (typically a hole, pin, or slot) relative to specified datums. It's defined by ASME Y14.5 in the US and ISO 1101 internationally.
Position Tolerance Formula
Actual position = 2 × √(ΔX² + ΔY²)
Total allowed = Position tolerance + Bonus tolerance
PASS if Actual ≤ Total allowed
MMC, LMC, and RFS Modifiers
The "modifier" applied to a position tolerance changes how much extra tolerance you get based on the actual size of the feature:
- RFS (Regardless of Feature Size) — No bonus. Position tolerance applies regardless of hole/pin size. The most restrictive.
- MMC (Maximum Material Condition) — Bonus tolerance accumulates as the feature departs from MMC. Most common modifier; gives manufacturing flexibility.
- LMC (Least Material Condition) — Bonus accumulates as the feature departs from LMC. Used for wall thickness or minimum stock material concerns.
Bonus Tolerance Worked Example
Hole specified ⌀10 +0.05/-0 with position ⌀0.1 (M).
- MMC of hole = 10.00 (smallest hole)
- Actual hole measured: 10.04
- Bonus tolerance = 10.04 − 10.00 = 0.04 mm
- Total position allowed = 0.1 + 0.04 = ⌀0.14
- Measured deviation: ΔX = 0.04, ΔY = 0.03 → Actual = 2 × √(0.04² + 0.03²) = ⌀0.10
- PASS — actual ⌀0.10 is within total allowed ⌀0.14 (0.04 mm headroom)
Common Position Tolerance Mistakes
- Forgetting bonus tolerance only applies with M or L modifier in the feature control frame.
- Confusing MMC of hole (smallest) with MMC of pin (largest).
- Reporting deviation as ΔX or ΔY only — true position is the diametrical spec, must use 2× √sum-of-squares.
- Measuring without proper datum simulation — surface plate setup must replicate the drawing's DRF.
When Position Tolerance Fails
Most position failures come from one dominant axis. If ΔX is much larger than ΔY (or vice versa), the issue is usually:
- Fixture clamping in the dominant direction
- Tool offset error in that axis
- Machine backlash or thermal growth
Investigate the dominant axis first — fixing that often saves the part.
Related Tools
For multi-feature analysis, use the Tolerance Stack-up calculator. For hole/shaft fits, see ISO 286 Fits. Document the position result in your AS9102 Form 3. For full GD&T symbol reference, visit the GD&T Reference page.