Location Tolerances: True Position, Concentricity, and Symmetry

What Location Tolerances Control

Location tolerances tell you exactly where a feature — a hole, a boss, a slot — must be relative to a set of datums. Three GD&T controls fall under this category: true position, concentricity, and symmetry. True position is by far the most common in CNC machining and the one most likely to appear on shop drawings and NIMS credentialing assessments.

True Position

A true position callout defines a tolerance zone centered on the theoretically exact location of a feature. That exact location is set by basic dimensions (boxed dimensions on the drawing) from the specified datum reference frame.

For a round hole, the tolerance zone is a cylinder whose diameter equals the value in the feature control frame. The center axis of the actual hole must fall inside that cylinder. For a point feature in a plane, the zone collapses to a circle.

The feature control frame reads left to right: the position symbol (a target/crosshair circle), the total tolerance diameter, and any material condition modifier, then the datum references in order of precedence — primary, secondary, tertiary.

MMC and RFS Modifiers

MMC (Maximum Material Condition) — the modifier circle-M — means the stated tolerance applies when the feature is at its largest allowable material size (smallest hole, largest pin). As the feature departs from MMC toward LMC, the position tolerance is allowed to increase by the same amount as the size departure. This bonus tolerance only exists at MMC; it rewards the inspector for a feature that has "extra" material removed.

RFS (Regardless of Feature Size) — implied when no modifier is shown in current ASME Y14.5 practice — means the stated tolerance applies at every actual feature size. There is no bonus. The tolerance zone stays fixed.

Example: a hole is ⌀0.500 +0.002/−0.000 (MMC = 0.500 in.) with a position tolerance of ⌀0.010 at MMC. If the hole is actually measured at ⌀0.501, the bonus is 0.001 in., and the allowable position tolerance opens to ⌀0.011.

Calculating True Position from Coordinate Measurements

When you measure a hole's actual center with a caliper, height gauge, or CMM, you get an X and Y coordinate. Compare those to the basic (theoretically exact) X and Y from the drawing. The deviations are Δx and Δy.

The diametral position error (the diameter of the smallest circle centered on the true position that contains the measured center) is:

Position error = 2 × √(Δx² + Δy²)

The factor of 2 converts the radial error to a diametral tolerance zone so it can be directly compared to the diametral tolerance in the feature control frame.

If the calculated position error ≤ the allowable tolerance (stated tolerance + any bonus), the hole passes. If it exceeds the allowable tolerance, the hole fails — it is out of location.

Concentricity and Symmetry

Concentricity controls the median points of a diametrically opposed surface relative to a datum axis. All median points must lie within a cylindrical tolerance zone coaxial with the datum. Because establishing median points requires many cross-sectional measurements, concentricity is difficult and expensive to verify — it is rarely used in modern practice. Runout or position controls are preferred for most coaxial features.

Symmetry controls the median points of a feature relative to a datum plane, requiring them to fall within two parallel planes equally disposed about the datum. Like concentricity, it is measurement-intensive and is used infrequently. Many designers substitute position or profile controls.

Setting Up for Manual Layout Measurement

To measure hole positions manually:

1. Place the part on a surface plate (flat reference surface). Use an angle plate or V-blocks as needed to establish datum A (usually the bottom face) perpendicular and stable.

2. Zero your height gauge on the surface plate to establish the Z reference, then measure from the datum edge using a digital caliper or step measurement to establish X and Y coordinates of each hole center.

3. Record measurements carefully — repeat each reading twice and average to reduce error.

4. Calculate Δx and Δy by subtracting the basic dimension from your measured coordinate, then apply the formula.

Safety on the surface plate: burrs on the part or chips under the part will gouge the lapped surface and throw off all measurements. Deburr the part before placing it. Never slide steel parts; lift and set them. Keep the plate clean and covered when not in use.

CMM Verification

A coordinate measuring machine (CMM) uses a touch-trigger probe to capture feature coordinates with high accuracy and repeatability. The CMM software computes position errors automatically using the same formula, applies the datum reference frame, and generates a report showing each feature's deviation and pass/fail status.

When reconciling CMM output with hand calculations: small differences (within about 0.001 in.) are normal given surface plate setup limitations. Larger disagreements usually point to an error in your datum setup — the part was not seated squarely on the reference plane, or you measured from the wrong edge.

CMM safety: the probe tip is fragile and expensive. Never jog the ram at high speed near the part. Follow the instructor's directions for loading and fixturing. Wear safety glasses; a dropped probe or part can cause injury.