Guide
What is the difference between circular runout and total runout?
Circular runout is a geometric tolerance that checks a surface one cross-section at a time: as the part turns a full revolution about its datum axis, the indicator reading at each circle must stay inside the tolerance. Total runout applies the same check to the whole surface at once, so the reading may not exceed the tolerance anywhere while the part rotates and the indicator sweeps the full length of a diameter or the full width of a face.
By Saola Manufacturing engineering team · Published · Updated
Both controls are defined in ASME Y14.5-2018 in the US and in ISO 1101:2017 internationally, where they are written “circular run-out” and “total run-out”. On a drawing, circular runout uses a single arrow in the feature control frame and total runout uses a double arrow. This guide covers what each one limits, how each is inspected, which to put on shafts and faces, and which machining decisions decide whether a turned part meets it.
On this page
How do the circular and total runout tolerance zones differ?
Circular runout gives every cross-section its own tolerance zone, so each circle is judged separately, while total runout gives the whole surface one zone: two coaxial cylinders around the datum axis for a diameter, or two parallel planes square to the axis for a face.
On a diameter, the circular zone is a ring between two concentric circles in a plane perpendicular to the datum axis, centered on that axis. Each measuring position has its own ring, and the rings are not linked to one another. That is the whole difference in practice. A diameter that tapers slightly from one end to the other can be round and perfectly centered at every section, so it passes circular runout, yet the large end and the small end do not fit inside one common cylinder, so it fails total runout. A bowed or barrel-shaped diameter behaves the same way.
On a face, circular runout (sometimes called axial runout) is read at one radius at a time. It catches wobble, where the face is tilted to the axis, but a face that is evenly dished or crowned can read almost nothing at every radius and still pass. Total runout on the same face sweeps the indicator from the inside edge to the outside edge in one setting, so a dished face fails. That is why total runout on a face limits both flatness and squareness to the axis, and circular runout limits only the wobble.
| Question | Circular runout | Total runout |
|---|---|---|
| Symbol | Single arrow | Double arrow |
| Zone on a diameter | Two concentric circles at each cross-section, independent of the others | Two coaxial cylinders covering the whole surface |
| Zone on a face | Axial band at each measuring radius, independent of the others | Two parallel planes perpendicular to the datum axis |
| Indicator during the check | Fixed position; reset at each new position | Travels the full surface in one setting while the part rotates |
| Limits on a diameter | Circularity and coaxiality at each section | Also straightness, taper and cylindricity along the length |
| Limits on a face | Wobble at each radius | Wobble, flatness and squareness to the axis |
| Surfaces it can go on | Any surface of revolution, including cones, chamfers and curved profiles | Cylinders around the axis and flat faces square to it |
| Material condition modifier | None; applies regardless of feature size | None; applies regardless of feature size |
Is total runout stricter than circular runout?
Yes: a surface that meets a total runout tolerance also meets a circular runout tolerance of the same value, but a surface that meets circular runout can still fail total runout.
So there is no point in calling both on the same surface with the same value; the total runout frame already says everything the circular one does. What is legitimate is a looser total runout combined with a tighter circular runout on the same diameter. That pair says the surface as a whole may taper a little, but every section must spin very true, which is a reasonable description of a seal track on a long diameter.
Total runout also costs more, both to hold on a long diameter, since it polices straightness and taper, and to measure. Use it where the function needs the whole surface, not as a stronger-sounding default.
When should a shaft drawing use circular runout and when total runout?
Use total runout where the full length or full face of a surface does the work, such as a bearing journal, a press-fit hub seat or a shoulder a bearing is clamped against. Use circular runout where each section acts on its own, such as a lip-seal track, a chamfer, a cone or a diameter that only has to spin clear of its neighbors.
A common motor or gearbox shaft shows how the choice falls out. The two bearing journals are the features the shaft actually rotates on, so they become datum features A and B, and the other features are controlled to the common axis A–B. A typical set of callouts reads:
- Gear or pulley seat: total runout to A–B, because the hub bears along the whole seat length and taper would tip the gear.
- Bearing shoulder face: total runout to A–B, because the inner ring seats across the whole face and a dished or tilted face would cock the bearing.
- Seal track: circular runout to A–B plus a surface roughness callout, because a lip seal rides one narrow band and cares about how true that band spins.
- Chamfers, lead-in cones and clearance diameters: circular runout, or simply the general tolerance, since nothing mates along their length.
- Each journal to the other: total runout of A to B and B to A, or a cylindricity refinement, when the two bearings must line up closely.
A part that locates on a face and a short pilot, such as a flange hub, takes the face as primary datum and the pilot as secondary. Either way, pick the datum features the part runs on in its assembly, not the ones that are easiest to grip.
How are circular runout and total runout measured?
Both are read as full indicator movement (FIM) while the part rotates about an axis simulated from its datum features. For circular runout the indicator stays put and is reset at each measuring position; for total runout it keeps one setting and travels the whole surface.
How the datum axis is simulated decides whether the reading means anything. Holding the part in a chuck or collet on the actual datum journals, or on a pair of precision rollers under them, reproduces the drawing. Running it between centers is only valid when the center holes are the datum, or when they were made in the same setup as the journals. V-blocks are quick, but a journal that is slightly lobed rises and falls in the V as it turns, and that form error shows up in the reading, so V-block results are best treated as a screen rather than a final acceptance.
Total runout also needs the indicator to traverse along a slide aligned with the datum axis, or a coordinate measuring machine or form instrument that scans the surface. Ask the supplier which method they will use before the first article, and ask for the FIM value of each controlled surface in the inspection report, not just a pass mark.
Which machining step decides runout on a turned part?
Mostly the number of times the part is gripped. Features finished in one clamping share one spindle axis, while any feature finished after the part is turned around or re-chucked inherits the locating error of the second grip.
So the process plan matters more than the lathe. When both ends need work, the usual answers are to finish the critical features last, together, in one clamping; to grip the second operation in soft jaws bored in place on the finished diameter; to turn or grind between centers made in the first operation; or to use a lathe with a sub-spindle. A sub-spindle hand-off is still a re-grip.
Total runout adds length effects that circular runout does not see. A slender shaft deflects away from the tool as the cut moves from the chuck, which leaves taper; a long finishing pass can wear the insert enough to change the diameter from one end to the other. Heat treatment after turning can bow a shaft, so hardened journals with tight total runout are commonly finish-ground afterward, and plating or anodizing adds a layer that is never perfectly even, so state whether the runout value applies before or after the coating. The surface finishing step should be planned with that in mind.
For reference, the CNC turning page covers how turned diameters are quoted at Saola. A size tolerance is not a runout value; runout depends on the setup plan and the datum scheme, so it is reviewed drawing by drawing.
How does runout relate to concentricity and ISO 2768-K?
Runout is the practical replacement for concentricity, which ASME Y14.5-2018 removed along with symmetry, because runout checks the surface itself instead of derived median points that are hard to measure. On ISO drawings, the K in “ISO 2768-mK” also sets a default circular runout for features without their own callout.
Runout is a composite reading. On a diameter it combines the out-of-roundness of the surface with its offset from the datum axis, so a part can fail runout because it is lobed even when its center sits exactly on the axis. When only location matters and the feature is a non-rotating bore or pin, position at a material condition may be the cheaper callout.
| Tolerance class | General circular run-out (mm) |
|---|---|
| H | 0.1 |
| K | 0.2 |
| L | 0.5 |
The general class is a fallback, not a design tool. It covers circular runout only, and it leaves the choice of datum to the rules of the standard rather than to the drawing. Any diameter or face whose runout affects fit or function deserves its own feature control frame with a named datum. The ISO 2768 and NADCA tolerances guide covers the rest of the general tolerance note and the status of ISO 2768-2.
What should a runout callout sent to an overseas turning shop include?
A clearly identified datum axis, the symbol that matches the function, a value on each surface that needs one, and a note on whether the value applies before or after coating. With those four items a shop in Vietnam, Mexico or anywhere else can plan setups and inspection from the drawing alone.
- Datums the part runs on. Label the bearing journals or the seating face and pilot, and write the common axis as A–B where two journals share it.
- Total only where it earns its cost. Journals, hub seats and bearing shoulders; circular runout or the general class for everything else.
- Coating state. One note saying whether runout is checked before or after plating, anodizing or painting.
- Inspection expectation. Ask for FIM readings per controlled surface in the first article report, and agree the datum simulation method in advance so both sides measure the same thing.
- Critical features flagged in the RFQ. A supplier who sees tight total runout at the quote stage can plan the part in fewer grips, which is where both cost and yield are decided.
The RFQ package guide lists the rest of what to send with a drawing. When it is ready, send it for a quote, and any runout callout that affects the setup plan is raised in the reply before production.
Frequently asked
Can MMC or LMC be applied to a runout tolerance?
No. ASME Y14.5 applies runout regardless of feature size, and the datum features in a runout frame are also referenced regardless of size. If a bonus tolerance is what you need, position is the control that allows it.
Is total runout the same as cylindricity?
No. Cylindricity is a form control with no datum; it only asks whether the surface is a good cylinder. Total runout asks the same and also whether that cylinder is centered on the datum axis, so it is the stronger of the two for a rotating journal.
Can total runout be applied to a cone or a chamfer?
Circular runout is the usual control for cones, chamfers and curved surfaces of revolution. Where a whole cone matters, profile of a surface to the datum axis is the common alternative.
Does a runout tolerance control the diameter size?
No. Runout is read as indicator movement, so a diameter that is uniformly oversize can show zero runout. The size tolerance is checked separately, with a micrometer, bore gauge or ring gauge.
Why do two inspectors get different runout readings on the same part?
Almost always because they simulated the datum differently: one in V-blocks, one between centers, one in a collet on the journal. Agree the method before the first article.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ISO 1101:2017, Geometrical product specifications (GPS) — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017 (confirmed)
- ISO 2768-2:1989, General tolerances — Part 2: Geometrical tolerances for features without individual tolerance indications, ISO, 1989 (withdrawn)
- ISO 22081:2021, General geometrical specifications and general size specifications, ISO, 2021