True Position: What ⌖ Really Means on a Drawing

The Problem with ± Dimensions

Walk into any machine shop and ask how holes are toleranced. Most machinists will say ±0.05, ±0.1 — a number in each direction for X and Y. This creates a square tolerance zone: any point inside the square passes.

Now think about what that actually means geometrically. A bolt hole doesn't care about your X and Y axes. It only cares whether it lines up with the mating bolt. The bolt lives at the center of a circle — and a square zone has corners that extend further from the nominal point than the inscribed circle.

This produces an inconsistency: two holes with identical actual deviation from nominal can get different results — one passing, one failing — depending purely on which direction the error lands. A hole displaced 0.07 mm diagonally fails the ± check but would be functionally fine. A hole displaced 0.05 mm exactly along one axis passes but might matter more functionally. The zone doesn't match the physics.

What True Position Actually Specifies

The ⌖ symbol controls the location of a feature — a hole, a slot, a pin — relative to one or more datums. The tolerance value after ⌖ defines the diameter of a cylindrical zone centered on the theoretically exact (true) position.

"Theoretically exact" is a precise term in GD&T. The nominal coordinates from the drawing define a perfect location in 3D space. The tolerance cylinder is centered on that exact point. The actual feature axis must fall entirely within the cylinder.

The Position Formula

At inspection, the CMM (or the inspector with a coordinate measuring system) measures the actual X and Y location of the hole center. The deviation from nominal in each axis gives Δx and Δy. True position error is calculated as:

The factor of 2 converts the radius of deviation to a diameter — because the drawing tolerance is expressed as a diameter. This is a common point of confusion: if the tolerance is ø0.1, the maximum allowable deviation radius is only 0.05 mm.

A worked example: a hole is found at X = +0.03 mm, Y = −0.04 mm from its nominal position.

If the drawing calls out ⌖ ø0.1, this hole is exactly at the limit — just barely passing. If the tolerance were ±0.05 in both X and Y, the same hole would pass on X (0.03 < 0.05) and pass on Y (0.04 < 0.05), but the diagonal distance is actually right at the limit. The cylindrical zone is honest about the geometry in a way the square zone is not.

Reading the Feature Control Frame

True position always appears inside a rectangular feature control frame, read left to right:

Box	Content	Meaning
1st	⌖	Geometric characteristic: position
2nd	ø0.1	Tolerance value; ø means cylindrical zone
3rd	A	Primary datum reference
4th	B	Secondary datum reference
5th	C	Tertiary datum reference (if needed)

The datum references are critical. Without them, "true position" is meaningless — position relative to what? On most Japanese machined parts, you will see datum A as the primary face (controls tilt), datum B as a reference bore or edge (controls rotation), and datum C as another edge (controls the remaining translation). The 3-2-1 locating principle from the datum article applies directly here.

In 36 years of quality work, I have seen more failed inspections caused by wrong datum setup than by parts that were actually out of position. The part is correct. The measurement setup is wrong. The feature control frame tells you exactly how to hold the part — ignore any of the datum calls and your result is garbage. — Jaw, Quality Engineer

Basic vs. Toleranced Dimensions

True position works together with basic dimensions — dimensions shown in a rectangular box on the drawing, without a tolerance. These boxed dimensions define the theoretically exact location of the feature. The position tolerance in the feature control frame is the only tolerance that applies to the location; the basic dimension itself has zero tolerance by definition.

This is different from general tolerances (which apply to all other unboxed dimensions). When you see a hole with a boxed 50 and a boxed 30 locating it, those are exact coordinates. The ⌖ value is the only permitted deviation from those exact coordinates.

On older Japanese drawings — particularly those following JIS B 0001 drawing standards from before the 1990s — you may see the basic dimension notation done differently, sometimes with a circle around the dimension rather than a box. The meaning is the same: theoretically exact, no independent tolerance.

Bolt Hole Patterns in Practice

The most common application of true position on Japanese industrial drawings is bolt hole patterns. A flange with six M8 holes on a 100 mm bolt circle will have each hole located by a basic angle (60° spacing) and a basic diameter (100 mm PCD), with true position controlling each hole individually.

The question is always: what tolerance value to specify? A useful rule of thumb for clearance holes:

Fit type	Typical ⌖ tolerance	Basis
Clearance bolt/hole (general)	ø0.5 – ø1.0	Clearance = hole dia. − bolt dia.; share with position
Dowel pin / locating pin	ø0.01 – ø0.05	Needs near-perfect location for function
Press-fit bore	ø0.02 – ø0.1	Depends on bore diameter and assembly force
Tapped hole (for bolt)	ø0.3 – ø0.8	Bolt threads provide compliance; more generous

The 57% Bonus — Why True Position Saves Money

Here is the practical factory argument for true position over ± tolerancing. Assume a drawing uses ±0.05 in X and ±0.05 in Y to locate a hole. The square zone has an area of 0.1 × 0.1 = 0.01 mm². The equivalent cylindrical zone (inscribed in that square, diameter = 0.1 mm) has an area of π × 0.05² ≈ 0.00785 mm² — smaller than the square zone.

But the correct equivalent comparison is different. If you re-specify the same functional requirement as a cylindrical zone that fits the bolt hole physics, the inscribed circle of the ± square has radius 0.05 mm, giving TP = ø0.1. That cylindrical zone now accepts parts in the corners — parts that were previously rejected by ± even though they would assemble correctly.

Studies on typical manufacturing processes show 5–15% of parts fall in the "corner zones" — inside the cylinder but outside the square. These are good parts being falsely rejected under coordinate tolerancing. True position eliminates that waste without loosening the functional requirement.

One Thing to Always Check

Before accepting any true position measurement result from a CMM report, verify three things: (1) the datum setup matches the drawing — A, B, C in the correct sequence; (2) the basic dimensions used in the calculation match the drawing exactly; and (3) the tolerance value has been correctly read as a diameter, not a radius. CMM software sometimes displays results as radius deviations. An error here causes the entire batch disposition to be wrong.