Ⓜ Maximum Material Condition (MMC)
Maximum Material Condition (MMC) · Modificadores de zona · ISO 1101 + ASME Y14.5
Example in plan
How to interpret it
The Ⓜ modifier means the 0.1 mm geometric tolerance applies when the hole is at its smallest size (or the pin at its largest). As the feature moves away from MMC, you gain additional geometric tolerance (bonus).
What controls
The condition in which the feature contains the maximum amount of material permitted by its size tolerance: the hole at its smallest diameter and the shaft at its largest diameter. When Ⓜ accompanies a geometric tolerance, that tolerance applies exactly at MMC, and as the feature departs from that condition (the hole gets larger, the shaft gets smaller) extra geometric tolerance is gained in the same amount: this is the bonus. It does not enlarge the size tolerance or allow the feature to go outside it; it simply redistributes a margin that the assembly already allows.
How to verify
First measure the actual size of the feature (micrometer, bore gauge or probe) and calculate the bonus as the difference between that actual size and the MMC size: the available geometric tolerance is the frame value plus that bonus. In series production, a functional gauge built to the virtual condition does both checks at once: if it goes in, the part meets position and size combined. On a CMM, evaluation with the material modifier must be explicitly enabled; if the software is left in regardless-of-feature-size mode, it rejects good parts.
Datums and notes
Ⓜ after a datum letter (|A Ⓜ|) refers to the datum, not to the toleranced feature: it allows play between the part and the gauge when the datum itself is a feature of size. This is a different, and much rarer, case than the modifier applied to the tolerance value.
Workshop guideline values
- General
- Bonus of 0.05–0.2 mm on through holes with a generous size tolerance.
- Accuracy
- 0.01–0.05 mm on H7/H8 holes for close-fit assembly.
- High precision
- 0.005–0.01 mm, or practically none, on features with a very tight size tolerance.
Guidance only: the drawing's value always wins.
Common mistakes when interpreting it
- Believing Ⓜ enlarges the size tolerance: the feature must still be within its dimension; the only thing that grows is the geometric zone.
- Applying it to something that is not a feature of size: Ⓜ only makes sense on holes, shafts, slots and tabs, never on a flat face.
- Calculating the bonus from the nominal size or the batch average instead of the actual size of each part.
How to get it in the workshop / if it comes out of tolerance
On holes, MMC gives bonus tolerance if the hole gets larger; on shafts, if the shaft gets smaller. Key for functional gauges and press-fit assembly.
Before rejecting a part on position, check the actual size: a hole that came out above its MMC may still be good thanks to the bonus. Conversely, if you are a few hundredths short on position, drilling the hole at the high end of its size tolerance is the cheapest way to gain margin without touching the machine. And remember that this margin does not exist if the drawing does not have Ⓜ.
Other symbols in Zone modifiers
Related tools
ISO fits
Calculates indicative ISO 286 tolerances for shaft and hole, H7/g6, H7/h6, H7/k6 and H7/p6 fits with clearance, transition and interference graph.
Inspection Plans
Upload a plan, extract dimensions and GD&T with AI and export your inspection guideline in PDF or CSV.
Shop trigonometry
Workshop trigonometry: right triangle, C chamfer, Z countersink, sine bar, taper and polar→X/Y for CNC operators.