What Problem Does MMC Solve?
Imagine a shaft that must fit through a hole. If the shaft is produced at its absolute largest allowed diameter — maximum material condition — it needs perfect position to still pass through. But if the shaft comes out slightly smaller than maximum, there is physical room to spare. The shaft could be off-center by a little and still assemble without interference.
MMC formalises this physical reality. Instead of applying a fixed geometric tolerance regardless of how the part was made, MMC says: as the feature departs from its maximum material size, grant bonus tolerance equal to that departure. The result is that more parts pass inspection — without compromising the functional requirement that parts actually assemble.
This is the key insight: MMC is not a shortcut to avoid tight tolerances. It is a mathematically exact description of the functional requirement for assembly.
Defining Maximum Material Condition
Maximum material condition is the state where a feature contains the most material within its size tolerance. For an external feature (shaft, pin, boss), MMC is the largest allowed diameter. For an internal feature (hole, slot, pocket), MMC is the smallest allowed diameter.
External Feature — Shaft ø10.0 / 9.8
MMC = ø10.0 (largest = most metal)
LMC = ø9.8 (smallest = least metal)
Internal Feature — Hole ø10.2 / 10.4
MMC = ø10.2 (smallest hole = most metal)
LMC = ø10.4 (largest hole = least metal)
The memory trick: MMC is always the condition that leaves the least room for mating parts. Least room means tightest fit. Tightest fit is where you need the most precise geometry.
The Bonus Tolerance Formula
When the Ⓜ modifier is applied in a feature control frame, the geometric tolerance stated on the drawing is the minimum. As the actual feature size departs from MMC toward LMC, additional tolerance is earned — called bonus tolerance.
Total tolerance = Stated tolerance + Bonus
A worked example for a shaft with position tolerance:
| Actual Diameter | Departure from MMC | Stated Tol. | Bonus | Total Position Tol. |
|---|---|---|---|---|
| ø10.0 (MMC) | 0 | ø0.10 | 0 | ø0.10 |
| ø9.95 | 0.05 | ø0.10 | 0.05 | ø0.15 |
| ø9.90 | 0.10 | ø0.10 | 0.10 | ø0.20 |
| ø9.85 | 0.15 | ø0.10 | 0.15 | ø0.25 |
| ø9.8 (LMC) | 0.20 | ø0.10 | 0.20 | ø0.30 |
Notice that at LMC, the total tolerance is three times the stated value. On a high-volume production run, this means dramatically fewer rejections — all while guaranteeing every accepted part will assemble correctly.
Reading the Feature Control Frame with Ⓜ
The Ⓜ modifier can appear in two positions within a feature control frame: after the tolerance value (applying to the controlled feature), or after a datum letter (applying to the datum feature). Each has a different effect.
→ ø0.1 minimum position; bonus earned as shaft shrinks from MMC
→ datum B also earns datum shift as it departs from MMC
MMC on the datum is called datum shift. When datum feature B is a pin and it is smaller than MMC, the entire tolerance zone can shift relative to the datum. This is an advanced topic — on most shop drawings, you will only see Ⓜ on the controlled feature.
Three Material Condition Modifiers Compared
ASME Y14.5 defines three material condition modifiers. Understanding all three prevents confusion on drawings that use them in combination.
Ⓜ — MMC
Maximum material. Smallest hole, largest shaft. Bonus as feature moves away from MMC. Use for assembly / fit.
Ⓛ — LMC
Least material. Largest hole, smallest shaft. Bonus as feature moves away from LMC. Use for wall thickness / edge break.
No modifier — RFS
Regardless of Feature Size. Tolerance applies equally at all sizes. No bonus. Default in ASME Y14.5-2009+.
When to Use — and When Not to Use — MMC
MMC is appropriate when the only functional requirement is assembly clearance. Bolt-hole patterns, shaft-in-bore assemblies, clearance-fit pins — these are natural candidates. If parts must assemble, MMC reflects the actual functional requirement without over-constraining the manufacturing process.
The wrong time to use MMC is on features that have a functional requirement independent of size — such as a sealing surface, a precision bearing bore, or a datum feature that will be used to locate other measurements. Apply RFS there.
A simple test: ask "If this feature is smaller/larger, does the assembly still work?" If yes and the only concern is clearance fit, use MMC. If performance, sealing, or precision location are involved, use RFS.
Virtual Condition — The Number That Never Changes
MMC introduces a concept that confuses many inspectors: virtual condition. Virtual condition is the worst-case boundary that the feature and its tolerance zone produce together. It does not change regardless of actual size.
Internal (hole): VC = MMC − Geometric Tolerance
For our shaft example (MMC ø10.0, position tol ø0.1): VC = ø10.1. No shaft at any allowed size, at any allowed position, will ever extend beyond a ø10.1 envelope. The mating hole must be at least ø10.1 to guarantee assembly. This is the number your tooling designer needs — not the nominal diameter, not the tolerance band.
最大実体状態とは、形体が許容寸法の範囲内で最も多くの材料を含む状態。外側形体（軸など）では最大径、内側形体（穴など）では最小径に相当する。実体公差方式（Ⓜ）を適用することで、形状の実際の寸法に応じたボーナス公差を許容できる。
One Rule to Apply Immediately
When you next see a bolt-hole pattern drawing, check whether the position callout includes Ⓜ. If it does not, ask whether the tolerance is truly independent of size. In most bolt-hole applications, omitting Ⓜ wastes perfectly good parts and adds unnecessary scrap to your production line. Adding it correctly is not "loosening the tolerance" — it is describing the actual functional requirement more precisely.