True Position Calculator
Calculate a measured feature’s diametral X/Y position deviation and optionally check its GD&T position tolerance with MMC or LMC bonus.
Informational coordinate-based check only; not a complete datum or feature-axis inspection. Terms and Conditions.
For a circular position zone; coordinates must already be expressed in the correct datum reference frame.
Enter measured coordinates
Basic and actual X/Y values must use the same datum frame. Updates are automatic.
Calculated position
Diametral deviation, optional tolerance comparison, and independent size check.
Inspection details
Show calculation stepsCoordinate offsets, formula, bonus and acceptance checks
- Enter valid coordinates to view the calculation.
Position tolerance zone
Basic center, measured center, and specified circular position boundary. Diagram auto-scales.
Nominal center at the axis intersection. Coordinates assume a fixed, established datum frame.
Method, sources, and assumptions
A simplified coordinate-based check; not certification of complete GD&T conformance.
The calculation doubles the radial distance between measured and basic centers. When a position tolerance is supplied, the measured diametral deviation is compared with the stated tolerance plus an applicable MMC/LMC feature-size bonus.
- Coordinates are already in the drawing’s correctly established datum reference frame. A point-center check cannot evaluate axis tilt, form, datum mobility, composite position, or projected zones.
- A PASS is limited to the displayed, simplified checks and does not certify entire-part drawing conformance. Apply the drawing’s stated standard/edition and your inspection decision rule.
- The initial example uses basic (25, 40) mm and measured (25.03, 40.04) mm; example position tolerance is Ø0.12 mm at RFS.
Calculator guide
What Does True Position Measure?
True position describes how far a measured feature location departs from its theoretically exact, or basic, location. The calculator above uses basic and measured X/Y coordinates—or their direct differences—to report the diametral position deviation. If you enter a drawing’s position tolerance, it also compares the result with the available tolerance; optional MMC/LMC inputs account for feature-size bonus.
For the circular position zone modeled here, the calculator doubles the distance between the basic and measured centers. Its result is a coordinate-based check, not a complete inspection of a hole’s or pin’s entire axis, its datums, or every drawing requirement.
- Measured input
- Basic and actual X/Y coordinates, or direct X/Y deviations
- Primary output
- Diametral position deviation in mm or in
- Key prerequisite
- Both coordinates use the same correctly established reference frame
How to Use the True Position Calculator
Use your drawing’s basic location and a measurement of the same feature in the drawing’s reference frame. The initial example values are illustrative; replace them with your inspection data.
Choose how to enter location
Select Basic and measured X/Y to enter drawing and inspection coordinates, or Direct X/Y deviations when your inspection report already gives signed offsets from basic location. Changing modes preserves the represented offset.
Choose consistent length units
Use the length-units selector for millimeters or inches. Switching the selector converts the entered physical dimensions; it does not merely relabel the values.
Enter the measured values and optional limit
Enter the basic and measured coordinates (or direct deviations). The Position tolerance (diameter) field is optional: leaving it blank returns a measured position without a pass/fail comparison. If entered, use the drawing’s applicable diametral tolerance, not an independent ±X or ±Y limit.
Use Advanced Options only when the drawing calls for them
The default RFS — no bonus setting does not add feature-size bonus tolerance. When the controlled feature’s position callout specifies MMC or LMC, select the matching modifier, then enter the internal-hole or external-pin type, permitted size limits, and actual measured feature size. Review the separate size and position status.
True Position Formula and Tolerance Zone
The common two-dimensional circular-zone calculation starts with signed coordinate differences. The straight-line center offset is radial; doubling it expresses the required circular zone as a diameter.
Calculate the diametral deviation
In words: subtract each basic coordinate from its measured coordinate; square both differences; add them; take the square root; then multiply by two.
All coordinates must be in the same units and the same established frame. This computes a point-center deviation for a diametral circular zone, not the full geometry of a tilted feature axis.
- \(TP\)
- Diametral true positionDiameter of the smallest circle centered at basic location that contains the measured point.
- \(X_a\)
- Actual XMeasured feature-center X coordinate in the established reference frame.
- \(X_b\)
- Basic XTheoretically exact X coordinate specified by basic dimensions.
- \(Y_a\)
- Actual YMeasured feature-center Y coordinate in the established reference frame.
- \(Y_b\)
- Basic YTheoretically exact Y coordinate specified by basic dimensions.
- Basic center
- Blue point at the circle’s center; theoretical X/Y location.
- Measured center
- Green point displaced +0.030 mm in X and +0.040 mm in Y.
- Radial deviation
- 0.050 mm from basic to measured center (solid diagonal).
- Diametral position
- Ø0.100 mm, twice the radial deviation.
Why a circular zone differs from independent X/Y limits
Independent ±0.100 mm limits in X and Y create a square. Their corner, at deviations (+0.100, +0.100) mm, is permitted by both separate coordinate limits but has Ø0.2828 mm diametral position, outside a Ø0.200 mm circular zone. The visual below compares those acceptance regions using the same center and scale.
Worked Example: Hole Position
A hole’s basic center is (25.000, 40.000) mm. An appropriately datum-aligned measurement reports its center at (25.030, 40.040) mm. The drawing calls for Ø0.120 mm position tolerance at RFS. Calculate the measured position and compare it with the specified limit.
Calculate the offsets and substitute
ΔX = 25.030 − 25.000 = +0.030 mm; ΔY = 40.040 − 40.000 = +0.040 mm. All inputs already use millimeters, so no unit conversion is needed.
Result
Measured position: Ø0.100 mm
The center-position check is within the example Ø0.120 mm limit, leaving 0.020 mm of diametral position margin. This is not an independent conclusion about the whole hole axis or the part’s other requirements.
How to Interpret Position and Pass/Fail
A smaller calculated position means the measured center lies closer to its basic location. With an applicable diametral tolerance entered, compare the unrounded measured position with the allowed diameter: a value at or below the limit meets this simplified center-position check, while a larger value exceeds it.
Position margin
Allowed position minus calculated position gives the remaining diametral margin. A negative margin indicates an exceeded center-position limit. The calculator’s result panel also distinguishes a feature-size failure when MMC/LMC size data have been entered.
Effect of larger offsets
Holding the other signed offset constant, increasing the magnitude of either deviation increases or maintains the position result. Doubling both offsets doubles the calculated diametral position; reversing both signs leaves its magnitude unchanged.
Fast sanity check
Position should be at least twice the magnitude of either individual coordinate deviation. For example, a 0.040 mm Y offset alone requires at least Ø0.080 mm position, regardless of the X offset.
MMC, LMC, and Bonus Tolerance
Material-condition modifiers can link a feature’s permitted geometric variation to its actual size. On the controlled feature, MMC is the condition containing the most material: the smallest hole or largest pin. LMC is the largest hole or smallest pin. RFS provides no size-derived bonus in this calculator.
| Modifier | Internal feature: hole | External feature: pin |
|---|---|---|
| MMC | Actual diameter − minimum permitted diameter | Maximum permitted diameter − actual diameter |
| LMC | Maximum permitted diameter − actual diameter | Actual diameter − minimum permitted diameter |
| RFS | No size-derived bonus | No size-derived bonus |
Worked MMC bonus example
Suppose a hole is permitted from 10.000 to 10.200 mm in diameter, measures 10.120 mm, and has a position callout of Ø0.180 mm at MMC. MMC is the 10.000 mm minimum hole size. Size-derived bonus is 10.120 − 10.000 = 0.120 mm; total allowed diametral position is 0.180 + 0.120 = Ø0.300 mm. A measured center-position value of Ø0.240 mm is within this simplified limit, assuming the size and reference-frame inputs are valid.
Worked LMC bonus example
For a hole with size limits 10.000–10.200 mm, LMC is the largest permitted hole, 10.200 mm. If the actual hole is 10.080 mm and the drawing states Ø0.100 mm position at LMC, the size-derived bonus is 10.200 − 10.080 = 0.120 mm. Total available diametral position is Ø0.100 + Ø0.120 = Ø0.220 mm. The actual feature must still satisfy its independent size requirement.
Virtual condition at MMC
For a simple cylindrical hole at MMC, the theoretical virtual-condition boundary is the MMC hole diameter minus the stated diametral position tolerance. For a Ø10.000 mm MMC hole with Ø0.200 mm position tolerance at MMC, the internal virtual-condition diameter is Ø9.800 mm. This theoretical boundary is not an actual measured hole diameter or a substitute for complete functional-gage inspection.
Read the Drawing and Datum References
Before using measured coordinates, identify the position control’s tolerance-zone shape, applicable modifier, basic dimensions, and datum references. The basic location represents the intended exact location; it is not a measured coordinate or an independent plus/minus tolerance.
Example: reading the feature control frame
Consider an illustrative position frame containing the position symbol, a diametral tolerance of 0.20 mm with the MMC modifier on the controlled feature, followed by datum references A, B, and C. The corresponding drawing also provides the hole’s basic X/Y dimensions and its size limits.
Position symbol and diameter
The position symbol ⌖ specifies a location control. A diameter symbol before the tolerance value identifies a diametral zone for the applicable cylindrical or circular interpretation. Enter that diameter as the stated tolerance, not its radius.
Datums establish the frame
Basic X/Y coordinates and inspection coordinates must be referenced to the same appropriately established frame. Simply typing datum labels into a report does not establish the frame or justify a best-fit translation or rotation of measured points.
Controlled feature versus datum modifier
An MMC or LMC modifier on the controlled feature concerns its size-derived geometric allowance. A material boundary modifier after a datum letter affects how that datum is established; do not add it as ordinary feature-size bonus.
Hole-pattern checks
For several holes, calculate the individual center deviations relative to the correctly established common datum frame and use the applicable tolerance for each. This basic procedure cannot independently establish compliance with composite position or permitted pattern mobility.
Four-hole pattern: independent center checks
Suppose a drawing controls four hole centers with Ø0.120 mm position at RFS relative to one correctly established common datum frame. The basic positions are H1 (0, 0), H2 (50, 0), H3 (0, 30), and H4 (50, 30) mm. The table evaluates the corresponding signed measured offsets. No best-fit pattern movement or composite position evaluation is applied.
| Hole | Actual X, Y | ΔX, ΔY | TP (Ø mm) | Margin (mm) | Center check |
|---|---|---|---|---|---|
| H1 | 0.020, 0.030 | +0.020, +0.030 | 0.0721 | +0.0479 | Within limit |
| H2 | 49.960, 0.010 | −0.040, +0.010 | 0.0825 | +0.0375 | Within limit |
| H3 | 0.060, 30.040 | +0.060, +0.040 | 0.1442 | −0.0242 | Outside limit |
| H4 | 49.990, 29.980 | −0.010, −0.020 | 0.0447 | +0.0753 | Within limit |
H3 exceeds the individual center-position limit; the other three centers are within it. The values are displayed to four decimal places, while an actual acceptance comparison should use unrounded calculated values and the applicable inspection decision rule. This example does not certify a complete hole pattern or inspect the entire axes.
For a broader explanation of feature control frames, basic dimensions, and datum symbols, see the Turn2Engineering GD&T guide.
Common Inspection Mistakes
Most misleading results come from mismatching the measurement to the drawing requirement, not from the square-root arithmetic.
Using radial distance as diametral position
A center offset of 0.050 mm corresponds to Ø0.100 mm position in the circular-zone calculation. Check whether the inspection report displays radial distance or already reports diametral position before multiplying by two.
Using different origins or mixed units
Coordinates in mismatched datum frames cannot be subtracted meaningfully. Likewise, 0.004 in must not be entered as 0.004 mm. Align the coordinate basis and check the unit selector before interpreting the result.
Counting an axis midpoint as the entire axis
An inclined feature may pass at one inspected cross-section yet extend outside the applicable cylindrical zone elsewhere. Obtain suitable axis or surface measurements when the drawing controls an entire derived axis or related geometry.
Rounding before checking the boundary
Do not treat a calculated position of 0.12004 mm as equal to a 0.12000 mm limit merely because a display rounds both to 0.120 mm. Retain measurement precision and use your inspection decision rule.
Doubling an already diametral CMM result
A CMM report may show signed ΔX/ΔY offsets, an actual feature center, a radial center distance, or an already computed diametral position. Enter signed offsets or actual coordinates as appropriate; do not multiply a reported diametral true-position value by two again. Check whether the CMM fitted a center at one section or evaluated the full controlled feature axis.
What This Calculator Cannot Verify
The calculator applies a closed-form two-dimensional center-offset relationship. Its simplified PASS/FAIL comparison is useful only when the underlying drawing and measured-feature interpretation are appropriate for that model.
Whole-axis and form evaluation
A single X/Y center location does not establish whether every relevant point along an actual hole or pin axis lies inside its cylindrical positional zone. Axis tilt, extraction of a derived feature, and form require additional metrology.
Advanced position controls
The tool does not construct or optimize datum frames, assess datum shift, solve composite position, evaluate projected tolerance zones, or inspect a spherical or specially shaped tolerance zone. Those requirements need suitable geometry and standard-specific procedures.
Complete part and assembly acceptance
A favorable simplified position comparison does not override size, surface, other geometric controls, or functional assembly requirements. Verify the full drawing and relevant part characteristics independently.
Uncertainty and drawing edition
The calculator does not determine measurement uncertainty or enforce a specific organization’s acceptance rule. Interpret borderline results under the specified drawing standard, inspection method, and governing quality procedure.
Standards and Method References
The numerical examples use the circular-zone coordinate relationship and are independently checked by calculating radial offset first, then doubling it. The references below provide context for interpreting the geometrical requirements; this page does not reproduce their complete normative rules.
- ASME Y14.5-2018 (R2024), Dimensioning and Tolerancing — ASME drawing interpretation, position controls, datums, and geometric tolerance conventions. Use the edition specified by the actual drawing or contract.
- ISO 1101:2017, Geometrical Tolerancing — ISO GPS symbolic geometrical specifications; ISO and ASME interpretation cannot be assumed identical.
- ISO 5459:2024, Datums and Datum Systems — ISO datum establishment and interpretation.
- ISO 2692:2021, Material Requirements — ISO maximum-material and least-material requirements and their applicability.