Concentricity Tolerance: GD&T, Measurement, and Inspection
Need Custom Components?
Looking for a direct China factory for plastic or hardware parts?
Your Direct China Manufacturer
In-house production for custom plastic and hardware parts.
A concentricity problem often starts before a part reaches production. A drawing calls for concentricity, the supplier checks the part with a dial indicator, and the customer evaluates it using a different geometric calculation. Both inspection reports may look reasonable, yet they do not necessarily measure the same requirement.
The consequence is more than a rejected sample. Tooling adjustments, additional machining, repeated measurements, and delayed approval can follow a requirement that was never clearly defined. Avoiding that situation means agreeing on the functional need, the drawing standard, the datum, and the inspection method before committing to tooling or production.

For buyers and engineers sourcing molded plastic components or hardware parts, concentricity tolerance should therefore be treated as a drawing-and-verification decision, not simply a tighter number beside a circular feature.
What Is Concentricity Tolerance?
In everyday manufacturing language, concentricity means that circular features share a common center, or that cylindrical features share a common axis. A bore positioned centrally within an outside diameter is a familiar example. However, this everyday meaning is not enough to define a formal acceptance requirement.
Under the legacy ASME Y14.5 definition, concentricity controls the derived median points of diametrically opposed surface elements relative to a datum axis. For a cylindrical application, those median points must lie within a cylindrical tolerance zone centered on the datum axis.
This is more specific than checking whether a fitted bore axis and a fitted outside-diameter axis appear aligned. It is also different from checking how much an external surface moves under an indicator as the part rotates.
The essential distinction is between controlling derived geometry and controlling the actual surface. A part can have acceptable median-point alignment while still having surface-form errors that affect its performance.
How to Read the Tolerance Zone

Consider an illustrative legacy ASME callout specifying a cylindrical concentricity zone of diameter 0.05 mm relative to datum A. Assuming the drawing establishes A as the relevant datum axis, the controlled median points must remain inside a cylinder 0.05 mm in diameter centered on that axis.
The radial allowance from the datum axis is therefore 0.025 mm, not 0.05 mm. Confusing a diametrical tolerance zone with a radial allowance can result in accepting a part outside the specified limit.
This geometric tolerance does not replace the bore or outside-diameter size tolerance. Size, surface form, orientation, and location requirements must be considered together.
Confirm the Drawing Standard Before Interpreting the Symbol
The phrase “concentricity GD&T” can lead engineers to explanations based on different standards and editions. Those explanations should not be treated as interchangeable.
ASME Y14.5-2018 removed concentricity as a supported geometric characteristic. For new drawings using that edition, engineers normally select another control, such as position or runout, according to the actual functional requirement.
That change does not automatically invalidate an older drawing. A drawing explicitly governed by ASME Y14.5-2009 can still contain a valid concentricity requirement under that edition. Suppliers should not silently reinterpret it as runout or position.
ISO GPS drawings require their own review. Concentricity and coaxiality terminology and specifications must be interpreted under the applicable ISO standards, including ISO 1101 where referenced. An ASME legacy median-point explanation should not be transferred automatically to an ISO callout.
- Confirm the governing standard and edition in the drawing notes or technical agreement.
- Check the complete feature control frame, datum references, and applicable modifiers.
- Resolve conflicts between the drawing, purchase specification, and inspection instructions before quotation approval.
- Document any replacement of a legacy control through an authorized drawing revision or written deviation.
Choose the Control That Matches the Functional Risk
Many concentricity disputes arise because the designer needs one outcome but specifies another. A rotating surface that must not wobble, a bore that must align for assembly, and a wall that must remain sufficiently thick are different engineering problems.
The following comparison provides a starting point. The final choice still depends on the governing standard, feature geometry, and assembly requirements.
| Control | Primary purpose | Typical inspection approach | Important limitation |
|---|---|---|---|
| Legacy ASME concentricity | Control derived median points relative to a datum axis | Suitable coordinate measurement with a defined sampling and evaluation method | Does not directly limit every surface variation or replace size control |
| Position | Locate a feature of size, including an applicable axis or derived median line, within its specified zone | Coordinate measurement or appropriate functional gauging, depending on the specification | Does not by itself provide complete surface-form or running-surface control |
| Circular runout | Limit surface variation during rotation at individual circular sections | Indicator or equivalent measurement while rotating about the datum axis | Does not control the full surface collectively along its length |
| Total runout | Limit combined variation over the controlled surface during rotation | Rotational inspection covering the specified surface extent | May impose broader surface requirements than an alignment-only function needs |
| Circularity | Control roundness of individual circular sections | Roundness measurement or suitable coordinate evaluation | Uses no datum and does not establish alignment with another feature |
For example, a molded sleeve may need a bore positioned relative to its mounting geometry so a mating pin can enter reliably. Position may address that requirement more directly than legacy concentricity. A rotating outside diameter whose surface movement matters may instead need runout control.
If the actual concern is minimum wall thickness, specify and verify that requirement directly where necessary. Neither a general concentricity note nor a comparison of fitted centers guarantees adequate wall thickness at every location.
Concentricity, Eccentricity, and Runout Are Not Interchangeable
Eccentricity generally describes the offset between centers or axes. Concentricity is a specified relationship, while runout is a measured surface variation relative to a rotation axis established from the datum.
For an ideal circular section with no form error, tilted-axis effects, or setup error, total indicator variation is twice the center offset. An eccentricity of 0.02 mm would therefore produce 0.04 mm of indicator variation in that simplified case.
Real parts rarely satisfy all those assumptions. Out-of-roundness, taper, surface texture, datum error, and fixture movement can affect the indicator reading. A dial indicator therefore cannot generally separate axis offset from surface-form error.
Do not convert a runout reading into a concentricity result unless a technically justified, approved inspection method supports that conversion. A useful shop-floor screening check is not automatically a valid contractual acceptance test.
How Concentricity Measurement Should Be Planned
Concentricity measurement begins with datum establishment, not instrument selection. A high-resolution instrument can still produce misleading results if the part is aligned to the wrong feature or the evaluation software calculates a different characteristic.
Establish the Datum Correctly
The inspection setup must reproduce the datum definition required by the drawing. Depending on the specification, that involves an appropriate physical datum simulator or a mathematically established datum based on measured features.
An arbitrary best-fit cylinder is not automatically equivalent to the required datum. Likewise, holding a bore on an expanding mandrel may introduce clearance, contact-pattern, or deformation effects that must be understood.
With thin plastic components, excessive clamping force can change the geometry being measured. A setup that forces a distorted part into alignment can conceal the free-state condition rather than characterize it.
Measure the Required Geometry, Not a Convenient Substitute
A coordinate measuring machine can support concentricity inspection, but the equipment name alone does not establish a valid method. The probe access, point distribution, datum construction, and software evaluation must match the specified requirement.
For legacy ASME concentricity, simply reporting the distance between two least-squares fitted cylinder axes is not sufficient evidence that the required median-point evaluation has been performed.
The inspection plan should define how opposing surface data are obtained and evaluated, which axial sections are sampled, and how the measurement covers relevant form variation. More points do not automatically make a result correct if the underlying calculation is wrong.
Account for Uncertainty Near the Limit
Measurement uncertainty includes more than instrument resolution. Probe behavior, part temperature, fixture repeatability, surface texture, sampling, and data processing can all contribute.
If the result is close to the tolerance limit, the acceptance decision should follow an agreed decision rule. Reporting extra decimal places does not resolve uncertainty. For disputed parts, compare the datum setup and evaluation method before assuming that one instrument is inaccurate.
What Changes for Injection-Molded Plastic Components?
For molded parts, the tool geometry is only the starting condition. The finished relationship between a bore and an outside diameter can also be affected by material shrinkage, cooling imbalance, core movement, residual stress, and distortion after ejection.
A narrow concentricity tolerance should therefore be evaluated alongside the resin grade, wall sections, feature length, and intended measurement condition. A long bore formed by a slender core presents different risks from a short, well-supported feature.
- Core support: Assess whether the core arrangement can maintain the required relationship under molding pressure.
- Wall distribution: Review uneven sections that may create differential shrinkage or pull the part away from its intended geometry.
- Measurement timing: Agree when samples will be inspected, particularly if cooling, moisture uptake, or conditioning affects dimensions.
- Fixturing: Prevent measurement loads from deforming thin walls or flexible locating features.
- Cavity traceability: Where multiple cavities are used, retain cavity identification so variation is not hidden inside a combined result.
A practical mistake is approving one freshly molded sample and treating it as proof of stable production. Validation should cover the agreed production conditions and account for relevant material behavior. Where moisture-sensitive plastics are involved, the specified conditioning state can materially affect the result.
What Changes for Metal Components?
For metal parts, an important question is whether related diameters can be produced while maintaining a consistent manufacturing reference. Features machined in one setup may be easier to align than features requiring removal, reversal, and reclamping.
However, a common setup is not a guarantee. Workholding distortion, tool deflection, burrs, and thin-wall movement can still affect the finished relationship. A part that measures well while clamped may change after release.
Where heat treatment, coating, or another geometry-affecting operation is specified, clarify whether inspection applies before or after that operation. An intermediate result cannot automatically serve as final acceptance.
In an illustrative spacer design, a bore and outside diameter may need a close alignment relationship. Before tightening the tolerance, engineering should assess the machining references, reclamping strategy, and inspection access. A minor drawing change can sometimes reduce manufacturing risk more effectively than adding inspection.
Link the Requirement to Quotation, Tooling, and Approval
A tolerance becomes commercially meaningful only when the supplier can understand, produce, and verify it. The same nominal value can carry very different costs depending on feature length, material stability, datum accessibility, and required inspection coverage.
JATERSON is a Zhejiang-based manufacturer with more than 20 years of production experience in injection molding and hardware manufacturing. Within that scope, a useful engineering review connects geometric requirements with tooling, process feasibility, sample development, and production quality planning. Inspection resources and any outside measurement support should be confirmed for the specific project rather than assumed.
Before issuing a purchase order, buyers should request agreement on the following points:
- The controlled drawing revision, governing standard, and tolerance interpretation.
- The functional reason for the requirement and any related size or form limits.
- The manufacturing condition at which acceptance applies, including specified finishing or conditioning.
- The datum setup, measurement method, sampling approach, and reporting format.
- The distinction between sample approval measurements and routine production checks.
- The response plan for borderline results, nonconforming samples, and process changes.
Where measurement requires a complex setup, its effect on sample lead time and inspection cost should be visible in the quotation. Production quantity also matters: a detailed laboratory evaluation may suit initial approval, while ongoing production needs a practical control plan linked to the same acceptance requirement.
Final Judgment: Is Concentricity the Right Requirement?
Use concentricity tolerance only when its defined geometric meaning matches the required function and the drawing standard supports it. For legacy drawings, preserve the specified interpretation unless an authorized change is made. For new designs, evaluate whether position, circular runout, total runout, or a direct wall-thickness requirement better expresses the need.
A robust requirement has three parts: a functional justification, a producible specification, and a reproducible inspection method. If any part is missing, tightening the tolerance usually increases disagreement rather than improving quality.
The most useful review happens before tooling release: identify what must remain aligned, establish the correct reference, and agree how compliance will be demonstrated. That gives engineering, purchasing, manufacturing, and quality teams the same basis for approving the part.
Recent Comments (0) 0
Leave a Reply