What is the difference between MMC and LMC?

MMC (Maximum Material Condition) is the size where the feature has the most material — smallest hole or largest shaft. LMC (Least Material Condition) is the opposite — largest hole or smallest shaft. The MMC modifier (Ⓜ) grants bonus tolerance as the feature deviates AWAY from MMC. The LMC modifier (Ⓛ) grants bonus tolerance as the feature deviates AWAY from LMC. MMC is used when assembly fit is the design intent. LMC is used when wall thickness or minimum material is the controlling factor.

When should I use MMC instead of LMC?

Use MMC when assembly fit is the design intent — bolt holes, dowel locations, mating pin clearances, any feature where the worst-case worry is the hole being too small to fit the bolt. Use LMC when wall thickness, minimum material, or breakthrough risk is the controlling factor — holes near thin edges in castings, cooling passages where wall is critical, alignment holes near the edge of a part. The rule of thumb: MMC for assembly, LMC for material strength.

Can I use MMC and LMC on the same feature?

Not on the same characteristic in the same feature control frame. A single position tolerance gets either Ⓜ or Ⓛ or neither (RFS). But a single feature can have multiple feature control frames stacked — for example a hole could have position tolerance at MMC plus a separate concentricity check at LMC. This is rare in practice; most features need only one material-condition modifier or none at all.

What does Ⓢ (RFS) mean compared to MMC and LMC?

RFS (Regardless of Feature Size) is the default condition in ASME Y14.5-2018. No bonus tolerance is granted regardless of how the feature is produced within its size limits. The Ⓢ symbol is no longer required in the 2018 standard — absence of Ⓜ or Ⓛ implies RFS. Use RFS when the function requires the same positional control whether the feature is at MMC or LMC — for example, a dowel pin hole on an optical alignment fixture must be in the right location absolutely, not relatively to the dowel size.

MMC vs LMC: when to use each modifier.

GD&T · ASME Y14.5 Material Condition Modifiers Updated May 2026

MMC and LMC are GD&T material-condition modifiers. They sound like opposites — and they are — but they solve different problems. MMC protects assembly fit. LMC protects material thickness. Picking the wrong one wastes parts or breaks function. This page covers both with side-by-side examples.

The two modifiers, side-by-side

Ⓜ

MMC — Maximum Material Condition

The size at which the feature has the most material: smallest hole, largest shaft, largest pin.

Bonus rule: as the feature deviates away from MMC, that deviation becomes additional positional tolerance.

Design intent: assembly fit. As hole grows above MMC, more clearance — so positional control can be looser.

Ⓛ

LMC — Least Material Condition

The size at which the feature has the least material: largest hole, smallest shaft, smallest pin.

Bonus rule: as the feature deviates away from LMC, that deviation becomes additional positional tolerance.

Design intent: minimum-material protection. As hole shrinks below LMC, more material remains — so positional control can be looser without breaking the wall.

Bonus tolerance math

Both modifiers work the same way mathematically, just measuring deviation from opposite ends of the size band.

MMC bonus

Bonus = |Actual Size − MMC Size|

LMC bonus

Bonus = |LMC Size − Actual Size|

Total allowed position equals the stated tolerance plus the bonus. Pass if measured position deviation ≤ total allowed.

Worked comparison

A ⌀5.0 +0.10/-0.00 hole produced at various sizes, called out as ⌖ ⌀0.10 with either modifier. MMC = 5.00, LMC = 5.10.

Actual hole ⌀	MMC bonus	Total allowed (MMC)	LMC bonus	Total allowed (LMC)
5.00 (at MMC)	0.00	0.10	0.10	0.20
5.02	0.02	0.12	0.08	0.18
5.05 (middle)	0.05	0.15	0.05	0.15
5.08	0.08	0.18	0.02	0.12
5.10 (at LMC)	0.10	0.20	0.00	0.10

At the middle of the size range, both modifiers give the same total allowed (0.15). At the extremes, they diverge — MMC is loosest when the hole is largest; LMC is loosest when the hole is smallest. The choice between them is purely about where in the size range you want the tightest control.

When to use MMC

Bolt holes and clearance holes. Worst case is the hole being too small to fit the bolt. MMC's tightest control at the smallest hole protects assembly.
Mating pin clearances. Two parts joining via a dowel pin — MMC on the receiving hole guarantees the dowel always fits.
Bearing seats. Inner ring on a shaft — MMC on the shaft hole protects against the shaft being too small for press fit.
Sub-assembly mating features. Where the part interfaces with another part, MMC protects the worst-case assembly condition.

When to use LMC

Holes near a thin wall. A hole 10 mm from a casting edge with 2 mm wall thickness — LMC protects against the hole drifting toward the edge and breaking through.
Cooling passages. Where wall thickness between coolant channels must stay above a minimum for pressure rating, LMC on the channel hole position protects the wall.
Bosses on thin-wall castings. A mounting boss with a tapped hole near the edge — LMC on the tap protects boss material around the threads.
Alignment features near an edge. Where positional drift toward the edge would compromise the part, LMC's tightest control at the loosest size protects material.

The rule of thumb MMC for assembly — protects the worst-case fit between mating parts.
LMC for material — protects the worst-case wall thickness or minimum stock.
RFS for absolute position — when neither bonus is appropriate and exact location matters.

The 5 spec mistakes

Using MMC on a wall-thickness-critical feature. A hole near a thin casting edge with MMC granted bonus as the hole grew — at LMC size, the hole drifted to the edge and broke through. Should have been LMC.
Using LMC on a bolt clearance hole. Bonus granted as the hole shrank means the bolt may not fit. Should have been MMC.
Defaulting to MMC because it's "common". MMC is the most-used modifier but it's not the right choice for every callout. Read the design intent before applying.
Using RFS by accident. ASME Y14.5-2018 made RFS the default — the Ⓢ symbol is no longer required. If your drawing has neither Ⓜ nor Ⓛ on a position callout, you are getting RFS (no bonus). Confirm that's what you want; otherwise add the modifier.
Misreading the bonus formula. MMC bonus = |Actual − MMC|. LMC bonus = |LMC − Actual|. Reversing these gives a wrong pass/fail verdict that may scrap good parts or pass bad ones.

Going deeper For the full position-tolerance math including the cylindrical zone formula and composite position (PLTZF/FRTZF), see the Position Tolerance reference. For the production-economics story of how missing MMC bonus turned a 12% scrap rate into 1.4%, see the MMC bonus tolerance article. For computing bonus on actual measurements, the Position Tolerance Calculator handles MMC, LMC, and RFS with up to 50 features at once.

ASME vs ISO

ASME Y14.5-2018 makes RFS the default. The Ⓢ symbol is optional — its absence implies RFS. ISO 1101 traditionally also defaults to RFS but uses different symbol conventions in older revisions. Both standards define MMC and LMC identically, so the math and the design-intent reasoning are universal across drawings issued by US, European, or Indian customers.

References

ASME Y14.5-2018 — Dimensioning and Tolerancing
ISO 2692:2014 — Geometrical product specifications (GPS) — Geometrical tolerancing — Maximum material requirement (MMR), least material requirement (LMR) and reciprocity requirement (RPR)
ISO 1101:2017 — Geometrical product specifications (GPS) — Geometrical tolerancing