True Position Calculator

True Position Calculator converts basic and measured coordinates into a diametral position error, adds MMC or LMC bonus from feature size, and reports pass or fail for the callout.

What the True Position Calculator Tells You About a Hole or Pin

The True Position Calculator turns the gap between a feature's basic location and its measured location into the diameter that a GD&T position callout is checked against. It adds any bonus earned from the feature's size, then gives a pass or fail, the direction the axis drifted and the gauge pin size for a functional check.

CMM programmers and QC inspectors use the True Position Calculator to double-check a report. Machinists use it to see which way to move a setup, and design engineers use it to see how much a callout really allows.

Enter basic and measured X and Y in inches, or switch to millimeters for true position in mm, all measured from the same datums. Add Z only for a spherical zone, or switch to Projected Zone and add a second reading lower in the hole. The Feature Size panel takes the size limits and actual size of the hole or pin, which the bonus and gauge results depend on.

Why the True Position Formula Doubles the Offset

A position tolerance written with a ø is a diameter, so the measured error has to be a diameter too. The straight-line offset from basic is a radius, and doubling it gives the zone the axis actually sits in.

$$TP=2\sqrt{\Delta X^2+\Delta Y^2}$$

With a basic location of 1.000, 2.000 in and a measured axis at 1.002, 1.997 in, the offset is 0.0036 in and the true position is ø0.0072 in. That fits inside a ø0.010 in callout before any bonus is counted.

Mixing up radius and diameter is an easy reporting slip. As one CMM programmer put it in a Hexagon PC-DMIS forum thread, true position is a diameter by default unless the drawing calls for a radial value, so check which one your software prints before comparing it to the callout. The True Position Calculator always reports the diameter.

True Position With MMC Bonus

With an MMC modifier, the position tolerance grows as the feature moves away from its tightest size. For a hole, MMC is the smallest allowed diameter, and GD&T Basics gives the bonus as the measured hole size minus that MMC size.

$$B_{hole}=D_{actual}-D_{MMC}$$

A pin works the other way, since its MMC is the largest size, so a smaller pin earns more bonus. LMC mirrors both: a hole gains bonus as it shrinks toward its smallest size, and a pin as it grows. RFS earns no bonus at all.

The example hole has 0.250 to 0.260 in limits and measures 0.254 in, so it earns 0.004 in. The allowed zone becomes ø0.014 in, and the measured ø0.0072 in uses 51.5% of it.

In the True Position Calculator, the Bonus Across the Size Range table steps from MMC to LMC and shows where this part would pass or fail at each size. A feature outside its size limits fails before position is checked, and the tool says so instead of granting bonus.

Above 80% of the zone used, the verdict turns amber. That threshold is the tool's own flag, because gauge and CMM uncertainty can push a part that close to the edge either way.

Virtual Condition and the Gauge Pin

At MMC, the hole's worst case for assembly is a fixed boundary called the virtual condition. A functional gauge uses a pin at that size, placed at the basic location.

$$V{C}_{hole}=D_{MMC}-T_{pos}$$

For the example, 0.250 in minus 0.010 in gives a ø0.240 in gauge pin. A pin feature uses its MMC plus the tolerance for a ring gauge instead, and at LMC the boundary moves to the other size limit.

Holes from a Bolt Circle Calculator layout drop straight in here, since its hole coordinates are the basic X and Y values the position check needs. For the hole size side of the fit, the Clearance Hole Calculator sizes the opening the fastener passes through.

Which Way the Axis Drifted

The offset card gives the radial distance and an angle measured counterclockwise from +X. The example axis sits 0.0036 in off at 303.7°, down and to the right, with ΔX of +0.0020 in and ΔY of -0.0030 in.

To correct it, move the setup or work offset the opposite way. The card also shows how much room is left in the drift direction, 0.0034 in here, before the axis reaches the edge of the allowed zone.

The sketch shows that example to scale. The solid circle is the ø0.014 in allowed zone, and the dashed box is the largest ± square that fits inside it.

What a ± Tolerance Would Have Allowed

The fourth card turns the round zone into its nearest ± equivalent. The largest square that fits inside the ø0.014 in zone is ±0.0049 in, while a single axis can shift up to ±0.007 in when the other axis is perfect.

That gap is the reason position tolerancing exists. GD&T Basics notes that a round zone holds 57% more area than the matching square, so parts that would fail a ± check in the corners still pass a position check.

True Position in 3D for X, Y and Z

Most holes and pins are checked in X and Y, because their tolerance zone is a cylinder running along the axis. Depth does not move the axis sideways, so Z stays out of the calculation.

The 3D mode adds ΔZ and treats the zone as a sphere. That matches a spherical position callout, written Sø on the drawing, such as the center of a ball or a spherical seat.

$$T{P}_{3D}=2\sqrt{\Delta X^2+\Delta Y^2+\Delta Z^2}$$

Using 3D on an ordinary hole makes the result larger than the drawing intends, so a good part can read as a reject. Leave the mode on 2D unless the callout carries the Sø symbol, or use Projected Zone when it carries a circled P.

Projected True Position for Tapped Holes

A tapped hole can sit in the right spot at the surface and still lean. The bolt follows that lean, so it can hit the clearance hole in the mating part even though the hole itself passes.

A projected tolerance zone, the circled P in the feature control frame, moves the check up to where the fastener sits. Tec-Ease's ASME Y14.5-2018 tip notes it is mainly used on threaded holes and holes that take a press-fit pin, that the projection is usually the maximum thickness of the mating part or the pin height, and that the tolerance applies only to the projected portion.

The True Position Calculator's Projected Zone mode takes the axis at the surface plus a second reading a known depth down the hole. The two points set the axis line, and the tool extends that line up by the projection height h, where d is the depth between readings.

$$\Delta X_{top}=\Delta X_s+\frac{X_s-X_d}{d}\times h$$

Y works the same way, and the position at the top comes from the usual 2√(ΔX² + ΔY²). Because the axis is a straight line, the worst point of the projected portion is at one of its two ends, so the tool checks the surface and the top and reports the larger.

With the default readings, the axis leans about 0.081°, 0.001 in per inch on each axis. At the surface it sits at ø0.0072 in, but 0.75 in above the part it reaches ø0.0093 in, which still passes the ø0.014 in zone at 66% used.

When a hole passes at the surface but its leaning axis leaves the zone above the part, the alert reads Fails Only in the Projection. That is exactly the case a plain position check would wave through.

True Position Calculator in Excel

The same 2D formula works in a spreadsheet. With basic X and Y in A2 and B2 and measured X and Y in C2 and D2, enter =2*SQRT((C2-A2)^2+(D2-B2)^2) to get the diameter.

Excel will not add bonus, check size limits or size the gauge pin unless you build those columns yourself. The True Position Calculator does those steps for one feature at a time, including the bonus table for the full size range.

What This Tool Does Not Cover

The result assumes fixed datums and a single feature. It does not add datum feature shift from datums referenced at MMB, and it does not evaluate a composite pattern callout across several holes.

CMM software or a functional gauge can account for datum shift and pattern requirements. For those callouts, use the full evaluation and treat this tool as a quick cross-check on each feature.