Material Condition Modifiers (MMC / LMC) & Bonus Tolerance
How maximum material condition adds bonus tolerance, why bolt holes should be toleranced at MMC, and the math behind functional gauges
Material condition modifiers tell the inspector whether a geometric tolerance expands as the feature departs from its maximum material condition. Under maximum material condition (MMC, symbol M), a positional tolerance gains bonus tolerance equal to the difference between the actual feature size and the MMC size — so a hole that is larger than minimum gets a wider allowed position zone. This is not a loophole: it precisely models a clearance-fit assembly, where a larger hole can accept more positional error and still assemble. The result is cheaper manufacturing with zero loss of function, which is why MMC is the workhorse of production drawings. Least material condition (LMC) protects minimum wall thickness; regardless of feature size (RFS) applies the tolerance unchanged.
1. The three conditions: MMC, LMC, RFS
Maximum material condition is the size that makes the part heaviest/largest for an external feature (maximum shaft diameter) or smallest for an internal feature (minimum hole diameter) — the condition that is hardest to assemble. Least material condition is the opposite: minimum shaft, maximum hole. RFS means the geometric tolerance applies at any size with no adjustment.
Rule #2 of ASME Y14.5 makes RFS the default for size features unless M or L is specified. In practice most positional tolerances on production drawings deliberately add M to get bonus tolerance.
2. Bonus tolerance: the calculation
For a hole toleranced at MMC: bonus tolerance = actual hole size − MMC size (hole). Total positional tolerance = stated zone + bonus. Example: a Ø6.0 mm hole with a Ø0.1 mm positional tolerance at MMC; if the machined hole measures Ø6.2 mm, bonus = 0.2 mm and the allowed zone becomes Ø0.3 mm.
The same logic applies to external features inverted: a shaft at its minimum diameter gains bonus against the MMC diameter. The tolerance zone grows exactly when the clearance fit has more room — nothing about function is sacrificed.
3. When to use MMC, LMC or RFS
Use MMC on bolt holes, dowel holes and any clearance-fit location — it reflects assembly reality and lowers scrap. Use LMC when the critical requirement is minimum wall thickness or distance to an edge (a hole near a casting wall). Use RFS when the feature has a functional relationship independent of size, such as a sealing surface whose flatness must hold regardless of diameter.
Do not apply MMC to form or orientation tolerances of non-size features, and remember the modifier sits inside the control frame right after the tolerance value, before the datum letters.
4. Functional gauges and inspection economics
A functional gauge (GO gauge) is designed at the MMC boundary: a pin of Ø(MMC hole − position tolerance) inserted into the hole must pass when the hole is at MMC. Gauging is fast, cheap and shop-floor friendly — one gauge checks both size and position simultaneously.
On a CMM the same result is evaluated mathematically: fit the measured axis and compare the actual position against the expanded zone. Because bonus tolerance is earned by being on the safe side of size, parts that ‘fail’ a fixed nominal zone often pass the correct MMC evaluation — the biggest GD&T inspection misconception in manufacturing.
Quick reference
| Hole size (mm) | Position tol @ MMC | Bonus | Total allowed zone |
|---|---|---|---|
| 6.00 (MMC) | Ø0.10 | 0.00 | Ø0.10 |
| 6.10 | Ø0.10 | 0.10 | Ø0.20 |
| 6.20 | Ø0.10 | 0.20 | Ø0.30 |
| 6.30 (LMC) | Ø0.10 | 0.30 | Ø0.40 |
Sources & references
- ASME Y14.5-2018 — Dimensioning and Tolerancing (material condition, Section 4.11)
- ISO 2692 — Geometrical tolerancing: Maximum material requirement (MMR)
- ASME Y14.43 — Dimensioning and Tolerancing for gauges and fixtures (functional gauge practice)
- Xometry Learning Center — MMC & Bonus Tolerance (public engineering reference)