Blog

Roundness and Concentricity: Reading the Tolerances That Stop Assembly

Roundness controls how far a circle's surface strays from a perfect circle; concentricity controls how far one circle's center sits from another's — and the part that fails assembly is usually the one whose centers drifted apart even though every diameter measured in spec. Size tolerance alone never guarantees geometry: a bore can be perfectly sized and still be oval, and a shaft can be perfectly sized and still spin off-center.

Two of the most misunderstood callouts on a machined drawing are roundness and concentricity. Both are geometric tolerances — they control form and location rather than size — and both show up on rotating assemblies, bearing seats, seals, and precision fits where a part that measures "to size" still fails in service. This guide defines each tolerance, explains what it actually controls, shows the numbers a CNC shop can hold, and covers how they are measured so you can read the inspection data instead of hoping.

Roundness: The Circle's Own Geometry

Roundness (also called circularity) controls how far the surface of a circle deviates from a perfect circle in a single plane. It is a form tolerance: it has no datum and no relation to anything else on the part. The tolerance zone is the annular band between two concentric circles, and the measured roundness is the radial distance between the innermost and outermost points of the actual profile. A roundness of 0.005 mm means the surface fits between two circles 0.005 mm apart in radius — the profile can be oval, lobed, or irregular, as long as it stays inside that band.

Roundness is not the same as diameter tolerance. A part can hold ±0.005 mm on diameter and still be oval by 0.01 mm if the clamping distorted it during the cut — the diameter readings average the lobes while the roundness reading exposes them. That is why rotating parts with seals or precision fits carry roundness callouts separately from size, and why a shop that only reports diameters is not proving the geometry.

Concentricity: Two Centers, One Axis

Concentricity controls how closely the center point (or axis) of one circular feature lies to the center point of another. Unlike roundness, it is a location tolerance that relates two features — the classic callout keeps a turned diameter's center within a small cylinder around the axis of a datum diameter. The old-style concentricity symbol, defined by measuring diametrically opposed points, has largely been replaced in modern GD&T practice by position (which controls the same center relationship with clearer rules) and by runout (which combines center offset with form error). Older drawings still call concentricity, and understanding it matters because legacy prints and customer specifications keep using it.

The practical distinction: runout is measured by spinning the part against a fixed indicator and catches both off-center and out-of-round in one number — which is why runout is usually the better production callout. Concentricity, measured statically as center-to-center distance, does not catch an oval part whose average center is perfect. When a drawing says "concentric within 0.01 mm," the shop should confirm whether the functional need is really runout, because a shaft that spins on off-center diameters fails a runout gage and might pass a static concentricity check.

What a CNC Shop Can Actually Hold

Realistic numbers depend on the process and the part's stiffness. A turned diameter between centers on a rigid setup holds roundness in the 2–5 µm range; grinding brings it to 0.5–2 µm; centerless grinding sits around 1–3 µm. Concentricity between diameters machined in one setup — the same clamping, no re-chuck — is excellent because the part never moved; the moment a part is re-chucked between operations, the new clamping error enters the concentricity budget. That single fact drives a lot of process design: critical concentric features are machined in one setup, or the second operation uses a reference diameter and a dial indicator to re-center before cutting.

The "0.005 mm class" figure is the honest production headline: collet-held turning on a stable machine holds concentricity in the 0.005 mm class when the features run in one setup, which is exactly the capability class we hold on CNC precision components and CNC turning work. Note the caveat that appears in every serious discussion: re-chucking is where concentricity dies. A drawing with concentricity between a bore and an outside diameter that must be machined in two setups should expect a looser number or a grinding operation — and a quote that ignores the re-chuck is a quote that will fail the first article.

How These Tolerances Are Measured

Roundness is measured on a roundness machine (a precision spindle with a probe) for the finest work, or estimated with a V-block and indicator for shop-floor checks — with the warning that a V-block cannot detect all lobe counts and can miss the exact error a 3-jaw chuck created. Concentricity and runout are measured on the machine or in inspection with the part rotating against an indicator, or on a CMM for center-to-center relationships. Each method has limits: a CMM measures a finite number of points around the circle, so it can miss lobing between measured points, while a roundness machine traces continuously.

For a buyer, the question is not which instrument the supplier owns — it is whether the measurement matches the risk. A seal seat needs true roundness measured with enough points or a continuous trace. A shaft that must spin true needs a runout check on centers. A bore that must align with another bore needs a CMM position check against the drawing datums. The discipline of reading these results is covered in our CMM inspection guide — the same rules apply: check datums, read deviations, and compare batch to batch rather than trusting a single pass stamp.

Drawing the Callouts So They Mean Something

Specify roundness only where the function needs it — seal seats, bearing journals, and uniform-wall applications — and give a number the process can hold without grinding unless you are paying for grinding. Call runout instead of concentricity for rotating features, because runout is what assembly actually feels. If a legacy drawing truly requires concentricity, define the datum clearly and tell the machinist which features must share a setup. And remember the re-chuck rule: features whose center relationship matters belong in one clamping, and the drawing should say when that is a functional requirement so the process engineer plans for it.

For holes, the same geometry logic applies one level down — a round hole is the precondition for every reamed or bored fit, and our hole tolerance by process article covers how drilling, reaming, and boring each deliver different roundness along with different size control. Geometry and size are two different promises; a drawing that calls both, and a shop that measures both, is what keeps assemblies from jamming on parts that "measured fine."

Frequently Asked Questions

Q: What is the difference between roundness and concentricity?

A: Roundness is a form tolerance — how far one circle's surface strays from a perfect circle, with no datum. Concentricity is a location tolerance — how far one circle's center sits from another's. A part can be perfectly round and off-center, or perfectly centered and out of round.

Q: Which is better to call on a drawing, concentricity or runout?

A: For rotating parts, runout is usually the better callout: it is measured by spinning the part against an indicator and catches both center offset and form error in one number. Concentricity measures center position only and can miss an oval part whose average center is perfect.

Q: What roundness can CNC machining hold?

A: Turned diameters on a rigid setup typically hold 2–5 µm roundness, grinding reaches 0.5–2 µm, and centerless grinding runs about 1–3 µm. Thin walls and long unsupported sections loosen these numbers — the part's stiffness sets the practical floor.

Q: Why does re-chucking ruin concentricity?

A: Every clamping introduces its own error — chip on a locating face, jaw wear, seating variation. Features machined in one setup share the same axis to the 0.005 mm class; once a part is re-chucked, that clamping error enters the concentricity budget and the number loosens.

Q: How is roundness actually measured?

A: The finest work uses a roundness machine with a precision spindle and continuous probe trace. Shop-floor V-block checks are faster but can miss even-lobe forms like the 3-lobe error a 3-jaw chuck creates. CMMs sample points and can miss lobing between measured points, so choose the method to match the risk.

Authored by the BQUQ Engineering Team. BQUQ is an ISO9001-certified source factory in Dongguan, China, running CNC machining, metal stamping, custom springs, heat sink and collet lines under one roof. Send drawings to sc@bquq.com or WhatsApp +86 13713157787 for a quote within 12 working hours. www.bquq.com