GD&T Runout: Circular vs Total Runout, FIM, and How to Measure It

Runout is one of the two runout controls in the ASME Y14.5 geometric tolerancing system, and it is fundamentally a composite tolerance: a single runout callout captures the combined effect of a surface’s form error (roundness) and its location error (eccentricity or coaxiality) relative to a datum axis. The definition is operational — runout is what a dial indicator shows. The part is rotated a full 360° about the datum axis while an indicator contacts the controlled surface, and the total swing of the needle, the full indicator movement, must not exceed the value in the feature control frame. If you are new to the framework, our guide to GD&T basics for CNC machining covers the system, and the GD&T symbols explained page decodes every feature control frame character.

The symbol tells you which version applies. Circular runout uses a single diagonal arrow (↗); total runout uses a double diagonal arrow (↗↗). Both always reference at least one datum — unlike pure form controls such as circularity, runout is meaningless without the datum axis the part rotates around. Both apply to surfaces of revolution: external and internal cylinders, cones, and planar faces perpendicular to the datum axis. And both always apply on a regardless-of-feature-size (RFS) basis — the tolerance value is a fixed FIM limit and cannot be modified with material boundary modifiers the way a position callout can.

Why does this matter so much in practice? Because the two errors runout bundles together are exactly the errors that make rotating hardware fail. A shaft that is perfectly round but eccentric whips its bearings; a shaft that is centered but lobed chatters its seals. Size tolerances and form controls alone catch neither condition reliably. Runout catches both with a measurement any shop can perform in minutes — which is why it has been the workhorse callout for rotating parts for as long as piston ring grooves and motor shafts have been made.

Runout measurement is beautifully simple in concept, and nearly all of its errors come from the setup. The procedure: mount the part so it rotates about the datum axis, bring a dial indicator into contact with the controlled surface perpendicular to it, rotate the part through one full revolution, and record the difference between the highest and lowest readings. That difference is the FIM, and it is compared directly against the value in the feature control frame.

The datum axis is the part that matters. Three setups dominate. Precision centers on the datum journals are the classic choice — the part spins on its own functional centers, just as it will in service. Precision V-blocks under the datum diameters work for parts without center holes, at the cost of folding the datum feature’s own roundness error into the reading. A chuck or collet gripping the datum feature is fastest and is how most shaft inspection actually happens on the shop floor. NEMA standards for motor shafts describe exactly this: indicator held stationary, contact at the end of the finished shaft surface, maximum-minus-minimum reading. Parts that turn about a finished bore — pulleys, gear blanks, spacers — take a close-fitting arbor through it and read against the axis that bore defines, so how that bore was reamed is part of the measurement too. Whatever the fixture, the rotation axis must be the datum axis — spinning the part about anything else measures something that is not runout. Our GD&T datums guide covers how datum features establish these axes.

Details that keep the reading honest: use an indicator with resolution at least 5–10× finer than the tolerance (a 0.001 mm or 0.0001 in indicator for tenths-class work); mount it rigidly, because flex in the stand reads as runout; apply light preload so the contact never leaves the surface; and rotate slowly and steadily. For circular runout, re-zero at each section and measure every section the drawing implies. For total runout, traverse the indicator along the surface in a smooth helical path without re-zeroing — the overall swing across the whole traverse is the result. A CMM can compute runout from scanned points with a best-fit datum axis, but the dial indicator setup remains the functional reference and the method every machinist trusts.

Runout shows up anywhere something spins, seals, or registers on a centerline. Shafts, spindles, rotors, bearing journals, gear seats, hydraulic spools, and sealing faces are the classic applications. Motor and gearbox builders call out shaft runout because misalignment and eccentricity are leading causes of bearing failure and vibration; turbomachinery controls rotor runout to hold blade-tip clearances; hydraulic valve bodies need spool runout to keep annular clearances even.

On values, the honest answer is that runout tolerance follows the process, not wishful thinking. General CNC turning on a journal commonly holds 0.025–0.1 mm of runout without special effort. Below about 0.025 mm (0.001 in), shops typically move to precision grinding on hardened, stabilized material — and the 0.001–0.005 mm band of precision spindles and instrument shafts is grinding-and-lapping territory. Since runout includes the surface’s roundness error, the callout can never be tighter than the circularity your process can actually hold — a 0.005 mm runout on a surface you can only turn to 0.01 mm circularity is scrap by definition.

If you are setting limits against general machining capability rather than a dedicated grinding operation, our CNC machining tolerances guide maps what each process tier holds, and the IsoCNC tolerances capability page shows the levels we inspect against, with reports.