ISO 1101 position tolerance at maximum material condition
The drawing of a mounting flange for an aircraft oil sump has a pattern of four holes with the position tolerance ⌀0.05 Ⓜ A B C. When the part goes on the coordinate measuring machine, the automatic report shows a position deviation of 0.058 mm for the first hole. The inspector is about to reject the flange without checking whether the maximum material modifier lets the assembly pass.
How an ISO 1101 position tolerance at maximum material is calculated
An ISO 1101 position tolerance at maximum material lets the geometric position tolerance grow by an amount equal to the difference between the actual size of the feature produced and its size at maximum material condition (MMC). This extra tolerance, called bonus tolerance, guarantees mechanical assembly while widening the acceptance intervals in production.
| Size condition of the feature | Hole diameter | Bonus tolerance | Total position tolerance allowed |
|---|---|---|---|
| MMC (maximum material) | 10.000 mm (lower limit) | 0.000 mm | 0.050 mm |
| In between | 10.005 mm | +0.005 mm | 0.055 mm |
| In between | 10.010 mm | +0.010 mm | 0.060 mm |
| LMC (least material) | 10.015 mm (upper limit) | +0.015 mm | 0.065 mm |
The Ⓜ modifier (the letter M in a circle), applied under ISO 2692, ties the geometric position tolerance to the actual size of the hole or shaft being inspected.
Maximum material condition and virtual condition size
For an internal feature such as a bore or a hole, maximum material condition (MMC) is the smallest size in the tolerance range. It’s the case where the part holds the most metal.
The virtual condition size is the perfect geometric boundary that the hole surface must never cross, to keep the assembly with the pin or the clearance bolt.
For a hole with minimum diameter D min and position tolerance t, the virtual condition diameter is:
DV = D min - t
In the example below, that gives 10.000 - 0.050, i.e. a boundary at 9.950 mm.
If a hole axis moves away from its exact theoretical position, the actual hole diameter has to grow by as much, so the assembly pin still passes without interference.
Calculating the bonus from the measured diameter
The bonus applies as soon as the measured diameter D actual moves away from the maximum material limit D min.
Bonus = D actual - D min
This bonus is added directly to the basic position tolerance given in the drawing’s tolerance frame. The maximum position tolerance allowed is the following sum:
t allowed = t basic + (D actual - D min)
This enlarged tolerance holds as long as the actual hole diameter doesn’t exceed its upper size limit (LMC).
To analyse the syntax of these complex frames, see our page on ISO 1101 geometric symbols.
Worked example on an aerospace mounting flange
Take a locating hole of nominal diameter ⌀10 H7, whose standard size limits are 10.000 mm and 10.015 mm. The geometric specification frame calls for a position tolerance of ⌀0.05 Ⓜ A B C.
The part comes off a 5-axis machining centre and goes to the metrology laboratory for CMM inspection at 20 °C.
Probing the hole gives an actual diameter of 10.012 mm and a measured radial position deviation of 0.058 mm relative to datums A, B and C.
| Quantity | Value |
|---|---|
| Minimum size at maximum material, D min | 10.000 mm |
| Basic position tolerance, t basic | 0.050 mm |
| Measured hole diameter, D actual | 10.012 mm |
| MMC bonus, 10.012 - 10.000 | 0.012 mm |
| Total tolerance allowed, 0.050 + 0.012 | 0.062 mm |
| Position deviation measured on the CMM | 0.058 mm |
Verdict: the measured deviation, 0.058 mm, is above the basic tolerance of 0.050 mm, but it stays below the enlarged tolerance allowed by the bonus, 0.062 mm. The part is declared conforming and approved for assembly. Without the maximum material modifier, this flange would have been wrongly scrapped.
Practical pitfalls when inspecting at maximum material
The first pitfall is applying the bonus when the actual hole diameter is above its upper size limit. If the hole measures 10.022 mm against an upper limit of 10.015 mm, the part doesn’t conform dimensionally, even if the position deviation calculated with the bonus looked very favourable.
The second is reversing the calculation between an internal feature (hole) and an external feature (shaft). For a shaft, maximum material is the largest diameter d max, and the bonus is then d max - d actual. Applying the hole formula to a shaft destroys the assembly condition.
The third comes from forgetting the Ⓜ modifier on datum features A, B or C in the tolerance frame. If the Ⓜ symbol follows the datum letter (for example A Ⓜ), the datum reference frame can shift, creating extra positioning play that must be included in the CMM calculation on the inspection report.
To apply these bonus rules automatically and avoid metrology entry errors, our dimensional quality inspection modules make FAI traceability simpler, and the CoteCote tooling page covers managing your inspection equipment.