GD&T Concentricity: Definition, Application and Measurement

Concentricity controls the median points of a feature relative to a datum axis. It evaluates material distribution rather than the actual surface, which makes it harder to understand, apply, and measure than most other tolerances. Consider a shaft that must rotate smoothly inside a bearing. A designer might conclude that the outer and inner races must be concentric and apply a concentricity callout. The same functional result, however, can be achieved with position and runout controls, which are easier and less costly to manufacture and inspect.

While concentricity is rarely specified on modern drawings, older drawings and a large share of the manufacturing workforce still reference earlier standards. Understanding how the tolerance zone is defined and how concentricity compares to its alternatives remains useful for interpreting legacy prints correctly.

What Is Concentricity in GD&T?

Engineering drawing example showing a concentricity feature control frame applied to a stepped shaft, referencing datum A.

Concentricity is the condition where the median points of all diametrically opposed elements of a surface of revolution, or the median points of correspondingly located elements of two or more radially disposed features, are congruent with a datum axis or center point.

Concentricity resembles axis straightness in that it also evaluates derived median elements rather than the actual surface. It is more demanding than straightness, since the median points must be measured relative to a separate datum axis, whereas straightness is checked against itself.

Concentricity is often mistaken for a tolerance that controls circular form. It only controls some aspects of form, not all of it. An oval, peanut, square, or any symmetric polygon can still pass a concentricity check, since the median points of diametrically opposed elements can land at the center within tolerance for any cross-section along the feature’s length. A D-shaped feature would not pass, since the median points on its flat side fall outside the tolerance zone. Any feature with symmetry at diametrically opposed points has a chance of passing concentricity, even when its shape is not circular at all.

Five symmetric cross-sections, including a circle, square, ellipse, peanut shape, and hexagon, each capable of passing a concentricity check.

Concentricity Tolerance Zone

The tolerance zone limits a feature’s permissible variation in location, form, and orientation. For concentricity, the tolerance zone is a cylinder whose axis coincides with the datum axis. The derived median points of the controlled feature must fall within this cylinder along the entire length of the feature.

Unlike several other GD&T controls, concentricity has only one tolerance zone shape. There is no equivalent to parallel planes, circles, or spheres, since concentricity always controls the location of a feature’s derived median line relative to a datum axis in three-dimensional space. The tolerance value stated in the callout is the diameter of that tolerance zone cylinder.

Concentricity Feature Control Frame

GD&T tolerances are denoted on engineering drawings through feature control frames, connected to the controlled feature by a leader arrow. A feature control frame has three blocks.

Geometric symbol block

The first block holds the GD&T symbol for the applied tolerance. Concentricity uses two concentric circles (◎).

Tolerance block

The tolerance block defines the shape, magnitude, and material condition of the tolerance. For concentricity, the zone is cylindrical, denoted with a diameter symbol, followed by the diameter magnitude of the cylindrical zone. A part passes as long as every median point along the feature’s length falls inside that cylinder.

Concentricity is always applied at RFS (regardless of feature size), so the tolerance block never carries a material condition modifier. Since no modifier applies, concentricity never allows bonus tolerance. The tolerance zone stays the same size no matter where the feature’s actual size falls between its maximum and least material conditions.

Datum block

The datum block holds the reference axis used as the concentricity datum, typically the axis of the primary cylindrical feature that drives the part’s alignment or rotation. A concentricity callout usually references a single datum feature, though multiple datums appear in two cases: when multiple coaxial features together define the datum axis end to end, forming a common datum written as two datum letters joined by a hyphen, or when a primary plane and a separate cylindrical bore are both needed to fully define the datum reference frame. Either way, the controlled median axis is ultimately evaluated against one derived datum axis.

Concentricity vs. Other Callouts

Concentricity overlaps in function with position and the two runout controls. Selecting the right callout depends on understanding exactly what each one governs and what it ignores.

Callout	Controls	Tolerance Zone	Handles Non-Round Shapes	Ease of Inspection	Use Instead of Concentricity When
Concentricity	Median point distribution about a datum axis	Cylinder	Yes, if symmetric	Very difficult	Rarely, legacy drawings only
Position	Feature axis location (actual mating envelope)	Cylinder around true position	No, needs an added form control	Moderate	Standard hole or pin location control
Circular runout	Surface deviation at one cross-section	Two concentric circles (2D)	No	Easy	Dynamic rotation at a single cross-section
Total runout	Surface deviation across the full feature length	Cylindrical (3D)	No	Moderate	Rotating shafts needing full-length control

Concentricity vs. Position

Position evaluates the axis of a feature’s related actual mating envelope, the smallest cylinder that fits around an external feature or the largest cylinder that fits inside an internal one, oriented and located relative to the datum reference frame. A D-shaped pin can pass a position inspection if its derived axis falls within the stated tolerance, which is one of the classic reasons position alone is insufficient and why controls such as concentricity and symmetry were introduced.

A perfectly circular surface with a single high point could fail a position check, since that high point can shift the derived axis enough to violate tolerance.

Three-panel diagram comparing a circular feature with no high point, one high point, and two opposing high points, showing which pass position and concentricity checks.

The same surface could pass a concentricity check if a corresponding high point exists 180 degrees away, since the two would balance and pull the median point back to center.

Concentricity vs. Circular runout

Circular runout controls a surface’s circularity and axis alignment directly, through a two-dimensional tolerance zone at a specific cross-section, and is measured with a dial indicator rotated against the part at a fixed datum axis. It suits applications where dynamic assembly performance depends on minimizing off-axis wobble at a specific cross-section.

Unlike concentricity, circular runout checks the actual surface at that cross-section rather than a derived median point, which is what makes it far easier to inspect with standard shop equipment.

Concentricity vs. Total runout

Total runout extends circular runout’s control along the full feature length, governing circularity, straightness, taper, and axis alignment together in a three-dimensional zone. Total runout is common on high-speed rotating parts, such as shafts and flanges, where smooth rotation and dynamic balance matter along the entire length.

A feature that passes total runout will typically also pass concentricity. The reverse does not hold: a feature can fail runout and still pass concentricity, since concentricity does not require a circular form. A square whose central axis coincides with the datum axis passes concentricity at every cross-section, since a square is symmetric at diametrically opposed points, but the same square would fail any runout inspection. The same logic extends to other symmetric non-circular shapes, including ellipses and hexagons.

Concentricity controls the balance of a feature’s mass distribution. Runout controls the form of the surface and its location relative to an axis.

How to Measure Concentricity

Concentricity is measured cross-sectionally by building a cloud of median points for each section and checking them against the tolerance zone. Inspection begins by establishing the datum axis and constraining the part.

Using a dial indicator or CMM probe, readings are taken perpendicular to the datum axis. The part is rotated 180 degrees, and the median point is calculated from the opposing readings. This process repeats at 5 to 10-degree intervals around the circumference and along the feature’s length. A part passes only if all median points fall within the tolerance cylinder.

Close-up of a dial indicator probe measuring a shaft held in a rotating chuck for a manual concentricity check

Engineers often use total runout as a proxy for concentricity, as it typically implies compliance. However, this is not universal. A hollow pipe with a perfect outer surface may pass runout checks while failing a specific concentricity requirement due to internal wall thickness variations.

Measurement Method Comparison Table

Method	Accuracy	Setup Cost	Operator Skill Needed	Best Use Case
Dial indicator (manual)	Low	Low	Low	Simple parts, low volume
Coordinate measuring machine (CMM)	High	High	High	Complex parts, high-precision verification

Manual dial indicator inspection involves fixing the datum axis on a chuck to measure diametrically opposed points by hand across the feature’s length. While inexpensive and requiring minimal training, it has lower accuracy and a high operator calculation burden.

Conversely, a CMM defines a reference plane to probe internal and external circles, calculating values automatically. Although setup and equipment costs are higher, CMMs offer faster, highly accurate, and repeatable results.

Standard Reference

ASME Y14.5 Version	Concentricity Status	Typical Use Today
2009 and earlier	Included as a location tolerance	Found on legacy drawings
2018 (current)	Removed	Replaced by position or runout

Conclusion

Concentricity remains one of the most misunderstood and misapplied GD&T tolerances, which is why the current standard removed it entirely. Calculating and positioning a cloud of median points around a datum axis makes it notoriously difficult to inspect.

The GD&T technical library on Xometry Pro covers parallelism, circularity, flatness, cylindricity, and more.

The same functional intent can usually be achieved with a combination of runout and position controls, which are easier and less costly to manufacture and inspect. Since a large share of existing drawings, and a significant portion of the workforce, still reference the older standard, understanding concentricity remains valuable for interpreting legacy drawings correctly and avoiding measurement errors.