Guide
How does MMC bonus tolerance work on a hole pattern?
MMC bonus tolerance is the extra geometric tolerance a feature earns when its actual size moves away from its maximum material condition. On a hole, the maximum material condition is the smallest allowed diameter, so every bit of extra hole size is added to the position tolerance written in the feature control frame, because a larger hole can sit further off location and still clear its fastener.
By Saola Manufacturing engineering team · Published · Updated
Most explanations stop at the definition and a single hole. This guide works one complete example instead: a four-hole bolt pattern on a die-cast aluminum cover, from the fastener that sets the tolerance, through the arithmetic for each measured hole, to the functional gauge that checks all four at once. The rules follow ASME Y14.5-2018; ISO drawings reach the same result through ISO 2692.
On this page
What is bonus tolerance at maximum material condition?
Bonus tolerance is the difference between a feature’s actual size and its maximum material condition, added to the stated geometric tolerance when the feature control frame carries the circled M modifier. It exists because the worst case for assembly happens only when the feature is at its tightest size, so the tolerance can safely grow as the feature moves away from that size.
Maximum material condition (MMC) is the size limit at which the part holds the most material. For an internal feature such as a hole or slot, that is the smallest allowed size. For an external feature such as a pin, boss or shaft, it is the largest allowed size. The opposite limit is least material condition (LMC).
Without a modifier, a position tolerance applies regardless of feature size (RFS): the zone is the same whether the hole comes out small or large. Under ASME Y14.5-2018, RFS is the default, so the circled M has to be written in the feature control frame, right after the tolerance value, for bonus to apply. Once it is there, the tolerance written in the frame is only the minimum. It is the value that applies when the hole is produced exactly at MMC.
The size that counts is the size of the actual mating envelope: for a hole, the largest perfect cylinder that fits inside it. That matters on real parts. A hole that is slightly bell-mouthed or tapered can read large with a caliper at the entry and still be smaller deeper down, and only the smallest envelope earns bonus.
How do you calculate bonus tolerance step by step?
Subtract the MMC size from the actual mating size for a hole, or the actual size from the MMC size for a pin, and add the result to the tolerance in the feature control frame. The sum is the diameter of the position zone that particular feature is allowed on that particular part.
- Find MMC. For a hole dimensioned as a limit or plus-minus size, take the lower limit. For a pin, take the upper limit.
- Measure the actual mating size of the feature, not a single two-point reading.
- Reject on size first. If the actual size is outside the size limits, the part fails no matter how well the feature is located; bonus never rescues a size failure.
- Compute the bonus. Hole: actual size minus MMC. Pin: MMC minus actual size.
- Add it to the stated tolerance to get the total allowed position tolerance.
- Compare with the measured deviation. Position deviation is expressed as a diameter, so it equals twice the radial distance between the measured axis and its true position.
The bonus is largest when the feature is at LMC. For a hole, maximum total tolerance therefore equals the stated tolerance plus the full size tolerance.
What does a worked bolt-pattern example look like on a die-cast housing?
Take a die-cast aluminum cover held to a housing by four M6 screws, with clearance holes dimensioned 6.6 to 6.8 mm and a position tolerance of diameter 0.3 mm at MMC to datums A, B and C, evaluated per ASME Y14.5-2018. Each hole earns its own bonus, so four holes that are equally far off location can pass or fail depending on their size, as the table shows.
In this example MMC is the lower hole limit and LMC is the upper one, so the total allowed position tolerance ranges from the stated value at MMC up to the stated value plus the full size tolerance at LMC. The measured values are illustrative, chosen to show each outcome; the arithmetic follows the rules for position at MMC per ASME Y14.5-2018.
| Hole | Actual mating size (mm) | Offset X / Y from true position (mm) | Measured position (⌀ mm) | Bonus (mm) | Allowed at MMC (⌀ mm) | Result at MMC | Result if RFS |
|---|---|---|---|---|---|---|---|
| 1 | 6.62 | 0.10 / 0.12 | 0.312 | 0.02 | 0.32 | Pass | Fail |
| 2 | 6.60 | 0.12 / 0.10 | 0.312 | 0.00 | 0.30 | Fail | Fail |
| 3 | 6.75 | 0.15 / 0.18 | 0.469 | 0.15 | 0.45 | Fail | Fail |
| 4 | 6.78 | 0.16 / 0.12 | 0.400 | 0.18 | 0.48 | Pass | Fail |
Holes 1 and 2 sit the same distance from true position, yet only hole 1 passes, because it was drilled slightly larger. Hole 3 is large, but its offset is larger still. Hole 4 is the case that makes the modifier worth writing: under RFS it would be scrap, while at MMC it is a good part that will assemble, because a bigger hole leaves more room around the screw. Read the other way, the table shows why a buyer should never judge a positional result without the size of the same hole next to it.
On a cast part the example has a practical twist. Holes that are cored in the die carry draft, so their diameter changes along the depth, and the mating envelope is set by the narrowest section. Many designers therefore cast the holes undersize and finish them by drilling or milling in the same setup as the datum faces, which brings size and location under the control of one machine. See die casting and CNC milling for how those two steps fit together, and the ISO 2768 and NADCA tolerance guide for as-cast limits.
What is virtual condition, and why does it matter for fit?
Virtual condition is the constant boundary created by the MMC size and the geometric tolerance acting together: for a hole it is MMC minus the position tolerance, and for a pin it is MMC plus the position tolerance. It is the size of the worst-case opening the mating part must pass through, and it does not change as the hole size changes.
In the example, the virtual condition of each clearance hole is the lower size limit minus the stated tolerance, which works out to a diameter of 6.3 mm per ASME Y14.5 arithmetic. A small hole that is well located and a large hole that is further off location both keep that same cylinder of clear space open at true position. That is the real reason bonus tolerance is safe: the modifier trades size for location without ever shrinking the space the screw needs.
If the virtual condition of a hole is equal to or larger than that of the screw or pin passing through it, the two assemble in every combination the drawing allows.
How should the position tolerance be sized for the fasteners?
Use the fastener formulas: for a floating fastener, where a bolt passes through clearance holes in both parts, the tolerance per part is the hole MMC minus the fastener MMC. For a fixed fastener, where a screw threads into one part, that same difference has to be shared between the two parts.
For the cover in the example, the M6 screw has a nominal major diameter of 6.0 mm and the clearance hole MMC is 6.6 mm, so the difference available per ASME Y14.5 fastener-formula guidance is a diameter of 0.6 mm. Because the screws thread into tapped holes in the housing, this is a fixed-fastener case and the difference is split per ASME Y14.5 practice, here as 0.3 mm on the cover holes and 0.3 mm on the tapped holes, which is how the value in the feature control frame was chosen.
- Unequal splits are allowed. If the cover holes are finish-machined and the tapped holes are harder to hold, give the tapped holes the larger share.
- Tapped holes are a special case. The screw follows the thread axis, not the hole at the surface, so a projected tolerance zone is often specified on the threaded part. The RFQ preparation guide covers how to show thread callouts clearly.
Should the pattern be checked with a functional gauge or a CMM?
A functional gauge is the natural check for position at MMC on a production run, because it physically reproduces the virtual condition and accepts or rejects the whole pattern in one placement. A coordinate measuring machine (CMM) is better for first articles, process studies and any case where you need to know how far a part is from the limit, not just whether it passed.
For the four-hole cover, the gauge would carry datum simulators for A, B and C and four pins at the virtual condition size, located at the basic dimensions. If the cover drops over all four pins while seated on the datums, the pattern meets its position requirement at every hole size, with bonus applied automatically. The design of such gauges, including how gauge-maker tolerances are allocated, is covered by ASME Y14.43, which spells the word “gage”.
- A gauge checks location, not size. Hole size still needs its own check, such as a go/no-go plug, because the functional gauge cannot detect a hole that is over its upper limit.
- A gauge gives attribute data. It says pass or fail, so it cannot show a process drifting toward the edge. Pair it with periodic CMM measurement if trends matter.
- A CMM needs the right evaluation. The software has to be told the modifier is MMC and which size to use for bonus; a program written for RFS will reject good parts such as hole 4 in the example.
This is where MMC reduces cost: it accepts more parts that will actually assemble and makes a fast go/no-go check possible, without changing the part itself.
When should you not use the MMC modifier?
Leave MMC off when the feature’s function depends on its location at every size, not just on clearance. Typical examples are holes for press-fit dowels that locate another part, bearing and shaft bores, and features that set wall thickness or balance.
A dowel hole that locates a mating part should be where the drawing says, whatever its size, so RFS is the honest callout. Where minimum wall thickness is the concern, for example a hole close to the edge of a thin casting, the least material condition modifier is the better tool: it protects the material that remains, where MMC protects clearance.
What should a drawing sent to an overseas supplier say about MMC?
State the standard and edition, show the modifier in every feature control frame where it applies, and say how you expect the pattern to be verified. With those three points on the print, a supplier in Vietnam or anywhere else can plan fixturing and inspection before quoting.
- Edition. Write “Dimensioning and tolerancing per ASME Y14.5-2018” or the ISO equivalent in the title block. Under ISO rules the maximum material requirement is invoked the same way, by the circled M, as set out in ISO 2692.
- Modifier placement. A circled M after a datum letter means something different from one after the tolerance value: it lets the datum feature shift, which adds pattern-wide freedom rather than bonus for each hole. Make sure the frame says what you mean.
- Verification. Say whether you want a functional gauge result, CMM data for every hole, or both, and whether the report should list actual size and bonus next to each position value.
When the drawing is ready, send it for a quote. Any position callout that reads ambiguously, such as a missing modifier on a clearance pattern, is raised in the reply before production is planned.
Frequently asked
Does bonus tolerance apply to a pin as well as a hole?
Yes. For an external feature, MMC is the largest size, so the bonus grows as the pin gets smaller. The virtual condition of a pin is its MMC size plus the position tolerance.
Is bonus tolerance shared between the holes in a pattern?
No. Each hole earns bonus from its own actual size. Datum shift, from a datum feature referenced at maximum material boundary, is different: it moves the whole pattern together.
Can I use bonus tolerance if the drawing shows no modifier?
Not under ASME Y14.5-2018, where regardless of feature size is the default, and not under ISO 2692, which also requires the circled M to be written explicitly. Older ANSI/ASME editions (Y14.5-1973) implied MMC for position, which is another reason to name the edition on the drawing.
Does MMC apply to flatness or runout?
Runout never takes a material condition modifier. Flatness can only take it when applied to a feature of size, such as the derived median plane of a tab, not to a single surface.
Why did the CMM report reject a part that fits in assembly?
The most common cause is a program evaluating position regardless of feature size when the drawing says MMC. Ask for the report to show hole size, bonus and allowed tolerance beside each position result.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures, ASME, 2011 (reaffirmed 2020)
- ISO 2692:2021, Geometrical product specifications (GPS) — Geometrical tolerancing — Maximum material requirement (MMR), least material requirement (LMR) and reciprocity requirement (RPR), ISO, 2021
- MBE PMI validation and conformance test cases for ASME Y14 GD&T, NIST, 2016 (updated 2025)