Circularity in GD&T: The Roundness Tolerance, Its Symbol, and How to Measure It
Two concentric circles, one cross-section at a time, and no datum — circularity is the simplest form control on a drawing and one of the most mismeasured on the shop floor.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 16 min read
On this page
Quick Answer
Circularity — called roundness on the shop floor and in the ISO system — is a GD&T form tolerance that controls how close each cross-section of a cylindrical feature must be to a perfect circle. Its symbol is a circle, and its tolerance zone is two concentric circles separated radially by the tolerance value, applied independently at every cross-section along the feature. Because it is a form control, circularity never references a datum: it judges shape only, not position. It is the 2D sibling of cylindricity (whole surface), the datum-free cousin of runout (rotation about a datum axis), and the control you specify on bearing seats and seal surfaces where local ring shape drives function.
What Circularity Means: Symbol, Tolerance Zone, and Why No Datum
Under ASME Y14.5, circularity is one of the four form tolerances, alongside straightness, flatness, and cylindricity. Form tolerances control the shape of a single feature in isolation — no datum is ever referenced, and the feature control frame contains only the circle symbol and a tolerance value. That frame attaches to a cylindrical, conical, or spherical surface: a shaft journal, a bore, a tapered seat, or a ball. The tolerance zone is the radial gap between two concentric circles drawn in a plane perpendicular to the feature’s axis, and every point of the measured surface in that plane must fall inside the gap.
Two consequences follow from the definition, and both trip people up. First, the zone is evaluated independently at every cross-section. Slice the part anywhere along its length and that slice must be round to the callout — but the control says nothing about how the slices relate to each other. A shaft can pass circularity everywhere and still be tapered, bowed, or barrel-shaped, because those are axis-direction errors that a per-section control cannot see. Second, the zone floats: the pair of concentric circles centers itself on the measured data. A perfectly round section in the wrong place passes circularity, because position is not the control’s job.
The vocabulary deserves a note of its own. Circularity is the ASME drawing term; roundness is the ISO 1101 name for the identical control and the word every machinist, inspector, and gauge maker actually uses. A roundness measurement report from a form tester is exactly the evidence a circularity callout asks for. For the broader symbol system this callout lives in, see our GD&T symbols explained guide and the GD&T basics for CNC machining primer.
Circularity vs Cylindricity, Concentricity, and Runout
Four controls orbit the same round geometry, and drawings that confuse them are a daily source of quoting friction and inspection disputes. The clean way to keep them apart is to ask two questions: does the control judge one cross-section or the whole surface, and does it need a datum? Circularity judges one section with no datum — it is the minimal round-shape control. Cylindricity extends the same idea to the entire surface: two coaxial cylinders as the zone, capturing roundness, straightness, and taper in one callout, still with no datum. Our companion guides on cylindricity in GD&T and runout in GD&T go deeper on each.
| Control | Category | What It Controls | Datum Required? |
|---|---|---|---|
| Circularity (roundness) | Form — ○ | Roundness of each cross-section, checked independently of every other section | No |
| Cylindricity | Form — ⌭ | Roundness, straightness, and taper of the entire cylindrical surface at once | No |
| Concentricity | Location — ◎ (removed in ASME Y14.5-2018) | Derived median points of the feature relative to a datum axis | Yes |
| Circular runout | Runout — ↗ | Surface variation at each cross-section while the part rotates about a datum axis | Yes |
Concentricity and runout answer the second question differently: both require a datum axis, because they control where the feature is, not just its shape. Circular runout measures surface variation at each section while the part rotates about the datum, so it folds form, orientation, and location error into one dial reading — a runout failure can come from a bent axis even when every section is perfectly round. Concentricity, which compared derived median points to the datum axis, was removed from ASME Y14.5-2018 because it was nearly impossible to measure reliably; position and runout now do its work. The practical rule: reach for circularity when shape alone is the requirement, cylindricity when the whole surface must act as one cylinder, and runout when the part spins on a datum axis in service.
When a Circularity Callout Earns Its Place on the Drawing
Rule #1 of ASME Y14.5 — the envelope principle — already does quiet work on every feature of size: at maximum material condition, the surface must fit inside a boundary of perfect form. In plain terms, your diameter tolerance is already a crude roundness tolerance, and linear-dimension practice treats out-of-roundness as bounded by roughly the size tolerance range. A circularity callout is therefore only justified when the function demands form tighter than the size tolerance alone can guarantee. Calling out circularity looser than the size band adds nothing; calling it out blindly on every round feature adds cost everywhere it adds no value.
What do real values look like? On precision turned parts, circularity callouts commonly land in the 0.005–0.02 mm band, with the tight end verified on a roundness tester and the loose end within reach of a good CMM. Bearing practice anchors the top of that range: bearing catalogs specify seat quality through ISO tolerance grades — a normal-class bearing typically wants an IT6 shaft seat and IT7 housing seat — and form error is expected to consume only a fraction of that grade. Seal contact bands, valve spools, and gauge features push tighter. For context on how these callouts stack with the rest of a tolerance scheme, see CNC machining tolerances and our tolerance capability page. Every geometric callout also carries an inspection cost — form verification is slower than a micrometer check — so specify circularity where function needs it and let Rule #1 carry the rest.
How Circularity Is Measured: Roundness Testers, CMMs, and the V-Block Trap
The reference instrument is the roundness tester. The part is centered on a precision rotary table — air-bearing spindles on lab-grade machines — while a stylus traces the cross-section through one full revolution. Software separates spindle error from part error, filters the profile into its harmonic components (oval shapes are the second harmonic, three-lobed shapes the third, and so on), and reports the radial deviation against a fitted reference circle. A dedicated roundness tester typically delivers five to ten times the accuracy of a CMM on form work, which is why tight circularity callouts route to the metrology lab.
A coordinate measuring machine is the flexible alternative: it samples discrete points around the section and fits a circle mathematically. Its limit is physics — volumetric accuracy of roughly 1.5–5 µm at typical working volumes is the same order as the form error a tight callout is trying to resolve — so CMMs serve comfortably for circularity above about 10 µm and strain below it. Point count and filtering choices also move the result, which is why CMM roundness programs should be agreed before a dispute, not after. The shop-floor V-block and dial indicator is the seductive shortcut, and it is a trap: a three-lobed part can spin in a V-block and show almost no indicator movement, because the lobes ride the block faces at nearly constant height. The two-point micrometer has the mirror-image blind spot, catching only even-lobed errors. Both are screening tools, never verification.
| Method | What You Actually Measure | Strengths | Limitations |
|---|---|---|---|
| Roundness tester | Radial deviation from a precision rotating reference axis | Highest accuracy available — typically 5–10× better than a CMM; the reference method for form | Dedicated instrument; checks one cross-section at a time; lab environment |
| CMM | Sampled points fitted to a reference circle by software | Flexible — size, position, and form in one setup; no dedicated instrument needed | Volumetric accuracy of roughly 1.5–5 µm limits fine form work; result depends on point count and filtering |
| V-block + dial indicator | Apparent radial change as the part rotates in the block | Cheap, fast, always available on the shop floor | Lobe- and angle-dependent; can read near zero on a badly lobed part; cannot verify a circularity callout |
| Two-point diameter (micrometer) | Local diameter between opposite contact points | Simple size check everyone knows | Only detects even-lobed errors; a three-lobed part can mic perfectly round — it is not a roundness measurement |
One process note for buyers: because circularity floats with no datum, a first-article report should state the instrument, the reference-circle method, the filter settings, and the number of sections measured. A single mid-length section tells you little about a long journal — ask for sections at both ends and the middle at minimum.
Where Circularity Does Real Work: Bearing Seats, Seals, and Rotating Parts
The classic application is the bearing seat. A ball or roller bearing is itself a precision round component, and it inherits the shape of whatever it is pressed onto: an out-of-round shaft journal elastically deforms the bearing ring into the same lobed shape, which shows up as vibration, noise, heat, and shortened fatigue life. That is why bearing catalogs prescribe ISO tolerance grades for seats and why drawings add circularity when the size grade alone cannot be trusted. Seal surfaces run a close second — a rotary lip seal tracks the shaft thousands of times per second, and lobing opens and closes the contact line with every revolution, pumping leakage past the lip.
Beyond those two, circularity shows up wherever a local ring of geometry carries the function: hydraulic and pneumatic spool lands that must meter flow without binding, piston-ring grooves, gauge pins and plug gauges, optical and encoder hubs, press-fit bands, and the register diameters that locate one part on another. The common thread is that the requirement is genuinely local — one band of the surface — which is exactly what a per-section form control describes better than cylindricity. Most of these parts come off lathes, and the process behind them is covered on our CNC turning page; where grinding enters the route, it is usually because the circularity target dropped below what turning holds reliably.
Specifying Circularity So the Shop Can Actually Hold It
Three habits make circularity callouts work instead of just decorating the print. First, put the value in proportion to the size tolerance. The callout must be tighter than the diameter tolerance to mean anything — a useful starting band is a third to a half of the size range, tightened only where bearing, seal, or metering function justifies it. Second, place the frame on the feature that matters. A leader to the bearing journal or seal band, not a blanket note across every diameter on the part; each extra callout is another form measurement on the inspection report and another line on the quote.
Third, think about how the part will be verified before you finalize the value. Anything below roughly 10 µm pushes the supplier toward a roundness tester and away from the CMM already on their floor; single-digit micrometer values may push the manufacturing route from turning to grinding. Neither is wrong — precision bearing seats genuinely live there — but the drawing should spend that money on purpose. If you are unsure whether a feature needs circularity, cylindricity, or runout, describe the function in a note and let the shop propose the control; a good machining partner flags an under- or over-specified callout at quote time rather than at the CMM. That is exactly the review our engineers run on every drawing that comes through the instant quote portal.
FAQ: Circularity and Roundness in GD&T
What is circularity in GD&T?
Circularity — also called roundness — is a form tolerance in ASME Y14.5 that controls how closely each cross-section of a cylindrical, conical, or spherical feature must approach a perfect circle. Its symbol is a simple circle. The tolerance zone is two concentric circles in the measurement plane, separated radially by the tolerance value; every point on the measured surface must fall between them. Circularity is evaluated independently at every cross-section along the feature, so it says nothing about taper or straightness along the axis — only about the shape of each slice. Because it is a form control, it never references a datum.
Is roundness the same thing as circularity?
Yes. Circularity is the term ASME Y14.5 uses on engineering drawings; roundness is the everyday shop term and the name used in the ISO system (ISO 1101) for the same control. Both describe the identical tolerance zone: two concentric circles, radially separated by the tolerance value, applied to one cross-section at a time. You will hear machinists, inspectors, and gauge manufacturers say roundness almost exclusively, while drawing callouts and GD&T coursework say circularity. When a supplier’s inspection report shows roundness results from a form tester, that data is exactly what verifies a circularity feature control frame — the vocabulary differs, the geometry does not.
Does circularity need a datum?
No. Circularity is a form tolerance, and form tolerances never reference datums. This is the single most common point of confusion, because runout — which also involves a round cross-section on a rotating part — always requires a datum axis. The distinction is logical: circularity judges only the shape of the feature itself, wherever it happens to sit in space. A cross-section can be perfectly round and in completely the wrong place, and it still passes circularity. Position, orientation, and coaxial relationships are separate requirements that need their own controls with datums. That is why the circularity feature control frame contains only the symbol and the tolerance value — there is no datum compartment.
What is the difference between circularity and cylindricity?
Circularity controls one cross-section at a time; cylindricity controls the whole cylindrical surface simultaneously. A shaft can pass circularity at every measured slice and still fail cylindricity, because circularity cannot see taper, bowing, or barrel shape along the axis — each section is judged on its own. Cylindricity’s tolerance zone is two coaxial cylinders, and passing it implies roundness, straightness, and taper control in a single callout, which is why it is the tighter, more expensive specification. Use circularity when only the local ring shape matters — a seal contact band, for example. Use cylindricity when the entire surface must function as one precision cylinder, such as a hydraulic spool or a gauge pin.
How do you measure circularity on a machined part?
The reference method is a dedicated roundness tester: the part sits on a precision rotary table or spindle while a stylus traces the cross-section, and software fits a reference circle and reports the radial deviation, complete with harmonic analysis that reveals lobing. A CMM is the flexible alternative — it samples points around the section and fits a circle, and it is adequate for tolerances above roughly 10 µm, though its 1.5–5 µm volumetric accuracy limits finer work. On the shop floor, a V-block and dial indicator gives a quick screening signal, but its reading depends on lobe count and block angle, so it can pass a badly out-of-round part and should never be used to verify a callout.
Can you check roundness with a V-block and dial indicator?
Only as a rough screen, never as verification. The method’s weakness is geometry: a part with three-lobed (or any odd-lobed) out-of-roundness can sit in a V-block and show almost no dial movement, because the lobes ride the block faces at a nearly constant height. The reading depends on the V-angle, the number of lobes, and where the indicator contacts the part, so the same component can measure differently from one setup to the next. The two-point micrometer check has the mirror-image problem — it catches even-lobed errors but reads a three-lobed part as perfectly round. For any drawing that carries a circularity callout, verify with a roundness tester or a carefully programmed CMM.
Related Resources
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
Passivation of Stainless Steel: Process, Specs, and When Parts Need It
Passivation of stainless steel explained for machined parts: the chemistry, ASTM A967 and AMS 2700 methods, nitric…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Tight Roundness on Turned Parts? Send the Drawing.
IsoCNC machines bearing seats, seal surfaces, and precision journals in steels, stainless, aluminum, titanium, and brass — with CMM and roundness verification, full material certs, and inspection reports on every lot. Not sure whether your feature needs circularity, cylindricity, or runout? An engineer reviews every RFQ, typically within 1–2 business days.