Position Tolerance: true position, MMC bonus, and real examples.

Position tolerance is the most-used symbol in GD&T — and the most often misread. This guide covers the cylindrical tolerance zone, the true position formula, MMC and LMC bonus calculations, composite position, and the five mistakes that cause aerospace and automotive FAI rejections.

What is position tolerance

Position tolerance (symbol ⌖, also called true position) constrains the location of a feature's axis, center plane, or center point to a tolerance zone defined relative to specified datums. Unlike size tolerances, which control how big a feature is, position tolerance controls where it is.

It is used on virtually every machined part with mating features: bolt circles, dowel pin holes, locating slots, bearing bores, hydraulic ports. The reason it is so heavily used: a cylindrical position tolerance zone allows 57% more usable area than the equivalent ±X / ±Y rectangular zone, while still guaranteeing assembly. This is the single most important reason GD&T exists.

The tolerance zone

The position tolerance zone shape depends on the feature type:

• Round features (holes, bosses, pins): the zone is a cylinder. The axis must lie inside the cylinder. Zone is named by diameter (e.g. ⌀0.1 means a 0.1 mm diameter cylinder).
• Slots and elongated features: the zone is two parallel planes. The center plane of the feature must lie between the planes.
• Spherical features: the zone is a sphere (rare). The center point must lie inside the sphere.

The zone is located at the basic dimensions from the datum reference frame. Basic dimensions are shown boxed (e.g. 25.0) and have no tolerance themselves — all the tolerance is captured by the position symbol.

The feature control frame

The position callout sits inside a feature control frame (FCF). Reading order is left to right:

Translated word-for-word: "Position tolerance, cylindrical zone of diameter 0.1, applied at Maximum Material Condition, with primary datum A, secondary datum B, tertiary datum C."

Three things to notice in this frame:

• The ⌀ symbol in the second compartment tells you the zone is cylindrical. Without it, the zone would default to two parallel planes — wrong for a hole.
• The Ⓜ modifier says bonus tolerance is available as the hole grows above its smallest (MMC) size. See section below.
• The datum sequence A → B → C matters. Datum A fully locks 3 degrees of freedom, B locks 2 more, C locks the last 1. Swap them and the part inspects differently.

The position formula

For a round feature inspected with X and Y deviations from the basic location, the position deviation diameter is:

The multiplier of 2 converts radial deviation to diameter — because the tolerance zone is specified by diameter, not radius. This is the single most common mistake in position calculation: forgetting the factor of 2.

For a feature inspected on a CMM with measured XYZ in 3D space, the deviation also has a Z component:

For most plate and bracket parts where the hole is normal to a flat face, ΔZ is zero and the 2D formula applies. The 3D formula is needed for compound-angle features and angled holes in cast or forged parts.

Worked example: 4-hole bolt pattern

An aluminium mounting plate has four ⌀5.0 +0.05/-0.00 holes called out at basic locations forming a 50 × 30 mm rectangle, with position tolerance ⌖ ⌀0.1 Ⓜ A B C.

After machining, the four holes are inspected on a CMM with the following measured center coordinates relative to the basic locations:

For hole H3, deviation is 0.128 mm but allowed is only 0.100 mm because the hole was produced at MMC (5.000, the smallest allowed size) and so received zero bonus tolerance. The hole fails — even though H2, with a similar deviation, passes because it earned bonus from growing to 5.030.

This is the central insight of position with MMC: tighter holes need to be more accurately located. The math rewards consistent feature size with looser positional control.

MMC bonus tolerance

The Ⓜ modifier (Maximum Material Condition) unlocks bonus tolerance as the feature deviates from its tightest condition. For a hole, MMC is the smallest allowed diameter — the hole that gives the least clearance to a mating fastener.

The bonus formula is:

The total allowed position tolerance becomes:

From the H2 row in the table above: hole MMC is 5.000, hole was made at 5.030, so bonus = 0.030 mm. Stated tolerance was 0.100 mm. Total allowed = 0.130 mm. Measured deviation 0.098 mm — pass.

MMC is used when the design intent is assembly fit: the worst-case clearance between the hole and the bolt is what matters, not the absolute position of either. As the hole grows, there is more clearance available — and the geometry naturally allows looser positional control without risking interference.

LMC bonus tolerance

The Ⓛ modifier (Least Material Condition) is the mirror of MMC. Bonus is granted as the feature moves away from its loosest size — that is, as a hole gets smaller, not larger.

LMC is used when wall thickness or minimum material is the controlling factor. A common example: a hole in a thin-walled casting where breaking through the wall is the failure mode. The smaller the hole, the more material remains around it, the more positional slop is acceptable.

The bonus formula is:

For a hole with LMC 5.05 and actual size 5.02, bonus = 0.03 mm. The total allowed position grows as the hole shrinks from LMC.

Composite position tolerance

For a pattern of holes that must both locate correctly to the part datums and fit a mating part as a group, GD&T uses composite position tolerance — two stacked feature control frames sharing the same ⌖ symbol:

The upper frame is the Pattern-Locating Tolerance Zone Framework (PLTZF) — it locates the entire group to A|B|C with a generous ⌀0.5 zone. The lower frame is the Feature-Relating Tolerance Zone Framework (FRTZF) — it controls how the holes locate relative to each other within a tighter ⌀0.1 zone, oriented only to datum A.

Practical effect: the bolt pattern as a whole can shift up to ⌀0.5 from nominal, but the holes within the pattern must match each other within ⌀0.1. This decouples assembly-to-frame tolerance from inter-hole pattern tolerance — and is how high-volume manufacturers avoid demanding ⌀0.1 absolute position when only the relative spacing matters for the mating part.

The five inspection failures

Across aerospace and automotive FAI submissions, these five position-tolerance mistakes account for the majority of rejections:

1. Forgetting the factor of 2. Engineer calculates √(0.04² + 0.03²) = 0.05 and reports "position 0.05 mm". The actual position deviation diameter is 0.10 mm — failed against a ⌀0.08 zone. Always multiply radial deviation by 2.
2. Missing the ⌀ symbol in the FCF. Without ⌀, the zone is two parallel planes, not a cylinder. CMM software interprets the call-out literally — and reports failures or non-conformances based on a planar zone the designer never intended.
3. Wrong datum sequence. Inspecting hole position with B as primary instead of A produces different deviations because the part is constrained from a different reference surface. Auditors check that the inspection setup matches the drawing datum sequence exactly.
4. Forgetting MMC bonus when one applies. Hole made at 5.030 with MMC at 5.000 and Ⓜ applied — engineer reports failure against 0.100 instead of 0.130. Re-work or scrap a perfectly good part. Always check whether bonus applies before declaring a fail.
5. Mixing pattern and feature deviation. Reporting hole position relative to a different hole in the pattern instead of to the datum reference frame. For PLTZF, position is always to the datums, not to other features.

ASME vs ISO: small but real differences

Position tolerance is defined in both ASME Y14.5 (US, 2018 revision) and ISO 1101 (international, 2017 revision). The two are mostly compatible — but three differences cause headaches when an Indian supplier ships to a US OEM, or vice versa:

• RFS default. ASME Y14.5-2018 makes RFS the default — no symbol needed. ISO 1101 also defaults to RFS but uses the Ⓡ modifier to explicitly call it out in older drawings.
• Concentricity and symmetry. ASME Y14.5-2018 removed concentricity (◎) and symmetry (≡) — both are now expressed using position with a center-plane callout. ISO 1101 retains them as separate symbols.
• Profile substitution. ASME allows profile of a surface to replace position in many cases. ISO requires explicit position on holes that engage mating fasteners.

Calculating position from your measurements

If you have measured ΔX and ΔY (and optionally ΔZ) deviations from a CMM or other coordinate inspection, the math is straightforward but easy to get wrong by hand. MetricMech's Position Tolerance Calculator handles the formula, MMC and LMC bonus calculation, pass/fail verdict, and produces an audit-ready PDF for FAI submission. It supports up to 50 features in one batch — useful when you have a hole pattern with dozens of locations to verify.

From measurement to process improvement

Position deviation data tells you more than pass or fail. Patterns across many parts reveal whether the deviation is random (process noise) or systematic (machine setup, fixture wear, tool deflection). A consistent +0.05 ΔX across 50 holes on the same lot points to a fixture offset — fixable with one shim. A random scatter across all four axes points to spindle deflection or chatter — fixable with feeds and speeds.

CadNexa's manufacturing analytics suite groups position-deviation data by feature class, fixture ID, and machine — making the systematic-vs-random pattern visible at a glance. For high-mix shops doing dozens of part numbers per shift, this is the difference between fighting fires and fixing root causes.