Guide
How do you calculate true position from CMM X and Y deviations?
True position is the exact location of a feature defined by basic dimensions from a datum reference frame, and the position deviation of a hole is calculated as two times the square root of (ΔX² + ΔY²), where ΔX and ΔY are the measured offsets of the hole axis from that exact location. The result is a diameter, so it compares directly with the diameter in the position feature control frame, plus any bonus tolerance allowed by an MMC or LMC modifier.
By Saola Manufacturing engineering team · Published · Updated
This guide gives the formula, a calculator that takes nominal and measured X and Y values, a worked four-hole example from a CMM report with the pass/fail call for each hole, and the cases where the plain formula gives the wrong answer: square coordinate zones, slots, tilted hole axes and datum shift. What position controls compared with concentricity and runout is covered in concentricity vs runout vs position.
On this page
What is the true position formula?
Position deviation = 2 × √(ΔX² + ΔY²), where ΔX = measured X − basic X and ΔY = measured Y − basic Y, both taken in the datum reference frame named in the feature control frame. The part conforms when that value is no larger than the stated diameter tolerance plus any bonus.
The square root gives the radial distance between where the axis is and where the basic dimensions say it should be. The factor of two converts that radius into a diameter, because ASME Y14.5-2018 defines the position zone for a cylindrical feature as a cylinder whose diameter equals the tolerance, centered on the true position. An axis can therefore move half the tolerance in any direction. Forgetting the factor of two is a frequent error in hand calculations and spreadsheets: the radial value looks like it passes with room to spare when the hole is actually out.
Three conditions sit behind the formula. The offsets must be measured from the datums, not from the edge of the CMM table or the first hole probed. The locating dimensions on the drawing must be basic (boxed), since a ± dimension makes the zone a rectangle instead of a circle; see the basic dimensions guide. And the formula as written is two-dimensional: it checks the axis at one depth. On ISO drawings, a position tolerance whose value is preceded by ⌀ also gives a circular or cylindrical zone for an axis (ISO 1101:2017), so the deviation arithmetic is the same; the Ⓜ (MMR) modifier there is governed by ISO 2692 rather than ISO 1101.
How do you use the true position calculator?
Enter the basic and measured X and Y of the feature, the position tolerance from the feature control frame, and, for an MMC or LMC callout, the size limit and the measured size. The calculator returns the position deviation, the allowed tolerance including bonus, and a pass or fail.
Use one unit throughout, inch or millimeter. The measured size for bonus should be the actual mating size the standard calls for, not a single caliper reading; the next sections explain why. The calculator runs in your browser and sends nothing anywhere.
What does a worked four-hole example from a CMM report look like?
Subtract basic from measured for each hole, apply the formula, then compare with the tolerance plus that hole’s own bonus. In the example below one hole passes only on bonus and one fails, even though all four would pass a square zone of the same nominal width.
The drawing calls out four holes at basic coordinates on a square pattern, sized .265–.272 with a position tolerance of ⌀.010 at MMC relative to datums A, B and C. The CMM aligned to A, B and C, measured each hole as a cylinder, and reported the axis location at the top face and the actual mating size. The values are an illustration of the arithmetic, not data from a real part.
| Hole (basic X, Y) | ΔX / ΔY | Position deviation ⌀ | Bonus (size − .265) | Allowed ⌀ | Result |
|---|---|---|---|---|---|
| 1 (1.000, 1.000) | +.0021 / −.0015 | .0052 | .0021 | .0121 | Pass |
| 2 (3.000, 1.000) | +.0040 / +.0031 | .0101 | .0005 | .0105 | Pass on bonus only (fails RFS) |
| 3 (3.000, 3.000) | −.0038 / +.0049 | .0124 | .0002 | .0102 | Fail |
| 4 (1.000, 3.000) | −.0007 / +.0012 | .0028 | .0040 | .0140 | Pass |
Hole 3 is the instructive one. Neither offset exceeds half the tolerance on its own, so a quick look down the X and Y columns of the report suggests the hole is fine. Combined, the axis sits outside the circle, in the corner of the square that the cylindrical zone does not include. Hole 2 shows the opposite case: it is outside the stated tolerance but legally inside the zone once its small bonus is added, which is exactly what the MMC modifier is for. How bonus grows with hole size is covered in the MMC bonus tolerance guide.
Two decisions remain before hole 2 is signed off. The CMM result has measurement uncertainty, and a reading that close to the limit may need a decision rule agreed in advance; NIST’s guidance on expressing uncertainty is the usual reference for how that uncertainty is stated (NIST TN 1297), and ASME B89.7.3.1 covers how to turn it into an accept or reject rule. Second, hole 3 can still be accepted if the datum feature is referenced at MMB and its departure from MMB allows the whole pattern to shift; that is a pattern-level calculation, covered below, and not a per-hole bonus.
How do RFS, MMC bonus and a square tolerance zone change the result?
RFS allows only the stated tolerance, MMC and LMC add bonus as the feature departs from that size limit, and a ± coordinate tolerance gives a square zone whose corners reach farther than the matching diameter. The table gives the formula and limit for each case.
RFS is the default in ASME Y14.5 when no modifier is shown. For bonus, the standard measures the hole by its unrelated actual mating envelope, the largest perfect cylinder that fits inside it, and the pin by the smallest that fits around it. A least-squares diameter from a CMM, or a two-point bore gauge reading, can be larger than that envelope on an out-of-round or tapered hole, which overstates the bonus. When a reading passes only on bonus, check which size the report used.
| Callout | Conforms when | Hole 3 allowed | Hole 3 result |
|---|---|---|---|
| ⌀t, RFS (no modifier) | 2√(ΔX²+ΔY²) ≤ t | .0100 | Fail (.0124) |
| ⌀t at MMC, hole | 2√(ΔX²+ΔY²) ≤ t + (actual mating size − MMC) | .0102 | Fail |
| ⌀t at MMC, pin or boss | 2√(ΔX²+ΔY²) ≤ t + (MMC − actual mating size) | n/a | n/a |
| ⌀t at LMC, hole | 2√(ΔX²+ΔY²) ≤ t + (LMC − actual minimum material size) | .0168 | Pass |
| Plus/minus t/2 in X and Y (coordinate tolerancing) | |ΔX| ≤ t/2 and |ΔY| ≤ t/2 (square zone) | .005 each axis | Pass |
| Diameter that just contains that t-wide square | ⌀ = t × √2, area about 57 percent larger than the square | .0141 | Pass |
| Spherical zone S⌀t (point location) | 2√(ΔX²+ΔY²+ΔZ²) ≤ t | .0100 | Depends on ΔZ |
The last two rows explain an argument that comes up when a legacy ± drawing is converted to GD&T. Replacing ±t/2 with ⌀t keeps the circle inside the old square and rejects parts the old drawing accepted, as hole 3 shows. Replacing it with ⌀t×√2 accepts everything the square accepted plus the extra area of the circle beyond the square’s sides, which is why a converted drawing usually loosens rather than tightens the shop’s job. The LMC row uses the hole’s LMC of .272 and, for illustration, treats .2652 as the hole’s actual minimum material size; LMC bonus protects wall thickness rather than assembly, so it is rarer on clearance holes.
How do you calculate true position on a slot?
For a slot or tab, position controls the center plane, so only the offset across the width counts: deviation = 2 × |Δ| measured perpendicular to the slot, compared with a tolerance zone of two parallel planes. An elongated hole with tolerances in both directions is checked once per direction.
A width feature has no axis, so there is no ΔX² + ΔY² to combine. The zone defined in ASME Y14.5-2018 for a width-type feature is the space between two parallel planes centered on the true position, so the check is twice the offset of the measured center plane in that one direction. With an MMC modifier the bonus is the slot’s actual mating width minus its MMC width.
An elongated hole (a slot with rounded ends used for adjustment) is usually given two feature control frames, one for its length direction and one for its width, each with its own tolerance, and sometimes the word BOUNDARY under them. ASME Y14.5 treats this as a boundary requirement: the slot surface must stay outside a slot-shaped virtual condition boundary located at true position, which a functional gauge or a CMM boundary fit checks directly. A common shop approximation is to check each direction separately with 2 × |ΔX| and 2 × |ΔY| against its own value, with bonus from the slot length and width respectively; treat a marginal result from that shortcut as a reason for the stricter check. Do not run the diametral formula on an elongated hole: it mixes two tolerances that the drawing deliberately kept apart.
How is true position measured on a CMM or with a gauge?
A CMM first builds the datum reference frame from the datum features in the order the feature control frame lists them, then measures each hole as a cylinder and reports the axis offset from basic. A functional gauge, used only with an MMC callout, checks the same thing as a pass or fail with fixed pins.
Alignment is where most disputed position results come from. If the CMM program aligns on the wrong datum, or on the right datums in the wrong order, the ΔX and ΔY it prints are offsets in the wrong coordinate system and the formula faithfully calculates the wrong number. The datum reference frame guide explains why the order changes the answer.
Depth matters too. Position applies to the whole axis over the full length of the feature, so a hole that is on location at the top but leaning will be out at the bottom. A CMM that probes one circle at the top face and runs the 2D formula misses that; measure at least two levels or fit a cylinder and report the worst end. Where a datum feature is called out at MMB, the pattern may shift as a group by the datum’s departure from MMB. That shift is evaluated for all holes together, by best-fitting the pattern inside the allowed shift or with a functional gauge built to ASME Y14.43 principles; it is never added to each hole as if it were bonus.
For position-toleranced holes milled into plates, housings and brackets on CNC milling, or cross holes and bolt circles on CNC turning parts, our engineers review the datum scheme on the drawing before quoting and raise questions where the datums cannot be held in one setup. On the RFQ, state which holes are critical, whether a CMM report with ΔX, ΔY, size and position is wanted for each one, and whether a functional gauge is acceptable instead. A drawing can be sent through the quote form.
What should a CMM report show so a buyer can check position?
For each controlled feature the report should show the basic X and Y, the measured X and Y, the deviations, the measured size used for bonus, the position deviation, the allowed tolerance including bonus, and the result. With those columns anyone can recompute the call with the formula above.
A report that prints only a single “TP” column and a pass mark cannot be checked: there is no way to tell whether the value is radial or diametral, which datums were used, or whether bonus was taken from a sensible size. Ask for the alignment to be stated by datum letter, for the measured size to be labeled as the actual mating size, and for tilted or deep holes to be reported at both ends. ASME Y14.45 covers measurement data reporting if a formal format is needed, and a ballooned drawing inspection report ties each line back to the drawing callout.
When you receive the report, paste the values for any hole within a few tenths of its limit into the calculator above. If your result and the report disagree, the usual causes are a radial value presented as diametral, bonus taken from a least-squares size, or offsets reported in machine rather than datum coordinates.
Frequently asked
Is true position a radius or a diameter?
The position tolerance in a feature control frame with a diameter symbol is a diameter, so the deviation is reported as a diameter too: twice the radial offset. Some CMM software can also print the radial value; check the report header before comparing it with the drawing.
Can a true position value be negative?
No. It is a distance, calculated from squared offsets, so it is zero or positive. The signed ΔX and ΔY tell you which direction the feature moved, which is what a machinist needs to correct an offset.
How do I calculate true position in Excel?
With basic X in A2, measured X in B2, basic Y in C2 and measured Y in D2, use
=2*SQRT((B2-A2)^2+(D2-C2)^2). For an MMC hole, add the bonus in another column as
measured size minus MMC size, floored at zero, and compare the two.
Is “true position” the same as “position”?
In practice, yes. ASME Y14.5 names the control “position” and uses “true position” for the theoretically exact location set by basic dimensions, but shops and CMM software use “true position” for the control and its measured value as well.
Does a hole at its MMC size get any bonus?
No. At exactly MMC the bonus is zero and the hole must meet the stated tolerance. Bonus only appears as the hole is made larger than MMC, up to its LMC, which is why tight-fitting holes gain little from the modifier.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ISO 1101:2017, Geometrical product specifications (GPS) — Geometrical tolerancing, ISO, 2017
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures, ASME, 2011 (reaffirmed 2020)
- NIST Technical Note 1297, Guidelines for Evaluating and Expressing the Uncertainty of NIST Measurement Results, B. N. Taylor and C. E. Kuyatt, NIST, 1994