How to Calculate True Position in GD&T: Full Guide

True position is the GD&T (geometric dimensioning and tolerancing) control that defines how far a feature’s actual centre can deviate from its theoretically exact location. The result is always expressed as a diameter, not a radius, because the tolerance zone is a cylinder or circle centred on the nominal position. Manufacturing and quality teams use it to decide whether a drilled hole, a machined boss, or any located feature passes or fails inspection.

What Does True Position Mean in GD&T?

True position in GD&T specifies the exact location a feature must occupy relative to one or more datums, and the maximum diametric zone within which the feature’s actual centre may fall. It is defined by the position symbol (a circle with crosshairs), the tolerance value, and the datum references, all written in a feature control frame on the engineering drawing. The word “position” in GD&T always means the diametric tolerance zone, which is why the calculated value is 2 times the radial offset rather than the radial offset itself.

The concept matters because a linear X measurement and a linear Y measurement each capture only one axis of deviation. A hole that is 0.003 inches off in X and 0.002 inches off in Y has both errors simultaneously. True position combines them into a single diametric number using Pythagorean geometry. That number tells the inspector exactly how large a circle the actual feature centre sits within, which is the same shape as the GD&T tolerance zone.

What Is the True Position Formula?

The true position formula is:

TP = 2 × √(ΔX² + ΔY²)

Variables:

• TP: true position value (in the same units as the measurement, typically inches or millimetres)
• ΔX: deviation in the X axis: measured X coordinate minus nominal X coordinate
• ΔY: deviation in the Y axis: measured Y coordinate minus nominal Y coordinate
• √: square root
• 2: the factor that converts radial offset to the diametric zone (matches the GD&T convention)

Why the formula multiplies by 2: GD&T position tolerances define a circular zone by its diameter, not its radius. The Pythagorean term √(ΔX² + ΔY²) gives the radial distance from true position to actual position. Multiplying by 2 gives the diameter of the smallest circle that contains the actual centre, which is directly comparable to the tolerance value on the drawing.

How to Calculate True Position: Worked Example

Inputs: A drilled hole has a nominal position of (0.000”, 0.000”). The CMM measurement shows an actual position of (0.003”, −0.002”). The drawing specifies a position tolerance of ⌀0.010”.

Step 1: Find ΔX and ΔY ΔX = 0.003” − 0.000” = 0.003” ΔY = −0.002” − 0.000” = −0.002”

Step 2: Square both deviations ΔX² = 0.003² = 0.000009 ΔY² = (−0.002)² = 0.000004

Step 3: Sum the squares ΔX² + ΔY² = 0.000009 + 0.000004 = 0.000013

Step 4: Take the square root √0.000013 = 0.003606” (rounded to six decimal places)

Step 5: Multiply by 2 TP = 2 × 0.003606” = 0.007211” (rounded to six decimal places)

Step 6: Compare to the tolerance Calculated TP = ⌀0.0072” (rounded to four decimal places) ≤ Tolerance ⌀0.010”

Result: The hole passes. Its actual centre sits within a ⌀0.0072” zone, inside the ⌀0.010” tolerance specified on the drawing.

Use the true position calculator to test coordinate deviations against GD&T limits.

What Is Bonus Tolerance and How Does It Affect True Position?

Bonus tolerance applies when the position control carries an MMC (maximum material condition) modifier, shown as the circled M in the feature control frame. As the feature departs from its maximum material size toward its minimum material size, the tolerance zone increases by the same amount. For a hole with a nominal diameter of 0.250” and an MMC diameter of 0.248”, a measured actual size of 0.251” gives a bonus tolerance of 0.003” (0.251 − 0.248). That bonus is added to the stated position tolerance, widening the acceptance zone.

Not every position control uses MMC. Controls specified at RFS (regardless of feature size) carry no bonus tolerance, and the stated tolerance value applies without adjustment regardless of the actual feature size. Always check the feature control frame for the material condition modifier before applying any bonus.

How Does True Position Differ from Runout or Concentricity?

True position, runout, and concentricity all deal with location, but they measure different things. True position locates the centre of a feature relative to datum references using X/Y coordinate deviations. Runout measures the total surface variation of a feature as it rotates around a datum axis, combining location and form errors in one reading. Concentricity (now largely replaced by position or symmetry in modern GD&T practice) measures only the median point deviation of a cylindrical feature from a datum axis.

Use true position when you need to control the location of a hole, pin, or other feature to assembly datums. Use runout when the rotating behaviour of a surface matters. The three controls are not interchangeable, and specifying the wrong one for an application will either over-constrain or under-constrain the part’s functional behaviour.

Sources

• ASME Y14.5-2018: Dimensioning and Tolerancing, standard for GD&T position controls, tolerance zone definitions, and MMC/bonus rules.
• GD&T Basics: True Position Guide, formula derivation and step-by-step calculation reference.

See all engineering and GD&T tools in the engineering calculators hub.