Skip to content

PRECIMORA / Resource

Concentricity, Runout, and Datums for Turned Parts

A turned part can measure right on every diameter and still fail in the assembly: the diameters are correct, the lengths are correct, and […]

A turned part can measure right on every diameter and still fail in the assembly: the diameters are correct, the lengths are correct, and the part wobbles — because the diameters are not on the same axis. A shaft whose two diameters are each perfectly round but offset by 0.05 mm will vibrate, wear unevenly and load its bearings on one side. Size tolerance alone does not catch this. This post explains the geometric tolerances that do — concentricity, circular runout, total runout and datums — what each one controls, when to use it, and how inspection proves it.

A long shaft being checked for runout with a dial indicator on a lathe.

The problem: diameters on different axes

Turning produces round features, but it does not automatically produce features that share an axis. Each time a part is re-clamped, each time a tool is changed, each time a long part flexes, the axis can shift slightly. The result is a part where the bore is round, the outside diameter is round, and the two are not coaxial. The functional consequence depends on the part. For a bushing, a bore that is off-axis from the outside diameter means the wall is thin on one side and the shaft sits off-centre. For a shaft, diameters that are off-axis from each other mean the shaft runs with a wobble. For a threaded insert, a thread that is off-axis from the outside means the mating screw enters at an angle.

The size tolerance alone does not catch this. A bore of 10.00 mm and an outside diameter of 20.00 mm can both be within their size tolerances while being offset from each other. The drawing needs a geometric tolerance to control the relationship between the features, not just their sizes. That is what concentricity and runout are for.

Concentricity: what it controls, and why it is rarely the right call

Concentricity controls the position of one feature’s axis relative to a datum axis. In its strict definition, it controls the derived median line of a cylindrical feature: every cross-section’s centre must fall inside a cylindrical tolerance zone around the datum axis. Precimora lists bore and outside-diameter concentricity typically 0.02 mm for its turned parts, which is the value to use as a reference when the drawing needs it.

But concentricity has a problem: it is hard to inspect. Measuring a derived median line requires measuring many cross-sections and computing their centres, which in practice means a coordinate measuring machine (CMM) and a careful measurement program. A dial indicator cannot measure concentricity directly. A buyer who calls out concentricity and then asks the supplier to verify it with a dial indicator is asking for something the instrument cannot do.

For that reason, most experienced designers now specify runout instead of concentricity for turned parts. Runout controls the same practical problem — the axis relationship — in a way that can be measured with a dial indicator on the shop floor. If the function is that the part must run true, runout is almost always the better callout. Concentricity remains appropriate where the standard or the mating requirement specifically demands it, but it should be the exception, not the default.

Circular runout: the practical control

Circular runout controls how much a surface varies as the part rotates about a datum axis. The part is mounted on its datum — usually a shaft held between centres, or a bore mounted on a mandrel — and a dial indicator touches the surface being controlled. As the part is rotated one full turn, the indicator shows the total variation. That variation is the circular runout, and it captures two things at once: whether the surface is round, and whether it is coaxial with the datum axis.

Circular runout is the workhorse geometric tolerance for turned parts. It is easy to specify, easy to inspect, and it controls the problem that matters — whether the part runs true. A typical value for a turned part is 0.02 mm, matching the concentricity value Precimora lists, but the value should be set by the function: a bearing surface needs tighter runout than a non-functional outside diameter. State the runout only on the surfaces that must run true, and state the datum — the axis the runout is measured against — explicitly. A runout callout without a datum is meaningless, because there is nothing to rotate about.

A machinist measuring a turned shaft with a Starrett micrometer.

Total runout: when circular runout is not enough

Total runout extends circular runout along the whole length of a surface. Where circular runout is measured at one cross-section, total runout is measured as the indicator is moved along the entire surface while the part rotates. It controls not only roundness and coaxiality but also straightness, taper, and cylindricity along the length.

Total runout is the right callout for a long bearing surface, where the shaft must run true along its whole length, not just at one cross-section. It is a tighter and more expensive requirement than circular runout, because it controls more, and it should be used only where the function demands it — a long bearing journal, a sealing surface that must stay in contact along its length, a shaft that carries a seal. For most turned parts, circular runout on the functional surfaces is enough, and total runout is over-specification.

Datums: the reference everything hangs on

A geometric tolerance is meaningless without a datum, and the datum choice is the most common source of confusion on turned-part drawings. The datum is the reference axis (or plane) that the tolerance is measured against, and it should be the feature that matters in the assembly. For a shaft, the datum is usually the bearing journal — the surface the shaft actually runs on. For a bushing, the datum is usually the bore or the outside diameter, whichever locates the part in the housing.

The mistake is to choose a datum that is convenient to measure rather than one that matters in the assembly. A datum on a non-functional surface produces a tolerance that controls the wrong relationship, and the part can pass inspection and still fail in the assembly. Choose the datum from the assembly: which feature locates the part, and which features must be true relative to it. State the datum on the drawing with the standard datum feature symbol, and make sure the inspection plan uses the same datum — a tolerance measured against a different datum is a different tolerance.

How inspection proves it

The inspection method follows the callout. Circular runout is checked with a dial indicator while the part rotates on its datum — a simple, fast check that Precimora’s final inspection can perform with the same instruments it uses for dimensions. Total runout needs the same setup with the indicator moved along the surface. Concentricity needs a CMM, which Precimora lists as available on critical features where specified.

The buyer’s job is to agree the inspection method before production. If the drawing calls out concentricity, the inspection plan must say CMM, and the cost and time of CMM inspection must be in the quote. If the drawing calls out circular runout, the inspection is a dial-indicator check, and the buyer can reasonably ask to see the runout reading. State the callout, the datum, and the inspection method together, so the supplier quotes the right inspection and the buyer knows what the number on the report means.

A micrometer clamped on a freshly machined metal shaft.

Buyer questions, answered

Should I call out concentricity or runout?

Runout, in almost every case. Concentricity controls the derived median line of a feature and is hard to inspect — it needs a coordinate measuring machine (CMM) and a careful measurement program, and a dial indicator cannot measure it directly. Circular runout controls the same practical problem — whether the part runs true — and can be checked on the shop floor with a dial indicator. Reserve concentricity for where the standard or the mating requirement specifically demands it.

What is the difference between circular runout and total runout?

Circular runout is measured at one cross-section as the part rotates about its datum axis; it captures roundness and coaxiality at that section. Total runout is measured as the indicator moves along the entire surface while the part rotates, so it also controls straightness, taper and cylindricity along the length. Total runout is the right callout for a long bearing surface; for most parts, circular runout is enough and total runout is over-specification.

How do I choose the datum?

From the assembly, not from convenience: the datum should be the feature that locates the part — usually the bearing journal for a shaft, or the bore or outside diameter for a bushing, whichever locates the part in the housing. A datum on a non-functional surface controls the wrong relationship, and the part can pass inspection and still fail in the assembly.

What runout value should I put on the drawing?

Set it by function, not by habit. A typical value for a turned part is 0.02 mm — matching the concentricity value Precimora lists — but a bearing surface needs tighter runout than a non-functional outside diameter. State runout only on the surfaces that must run true, and state the datum explicitly: a runout callout without a datum is meaningless, because there is nothing to rotate about.

Common pitfalls and how to avoid them

The most common pitfall is calling out concentricity when runout would do. Concentricity is hard to inspect and rarely needed; runout controls the same practical problem and can be checked on the shop floor.

The second is a runout callout with no datum. Without a datum, runout cannot be measured. State the datum feature explicitly.

The third is choosing a datum that does not matter in the assembly. The datum should be the feature that locates the part, not the easiest feature to measure.

The fourth is specifying total runout where circular runout would do. Total runout controls more and costs more; use it only on long functional surfaces.

The fifth is a tolerance value copied from another part. A runout of 0.02 mm is typical for Precimora’s turned parts, but the value should come from the function — a bearing surface needs it, a non-functional outside diameter does not.

The sixth is agreeing the callout but not the inspection method. A concentricity callout without a CMM plan, or a runout callout without a stated datum setup, will be inspected differently by different people. Agree the method in the inspection plan.

The geometry callout chooser

A decision table built from this post. Find the job, then the callout:

JobCalloutHow inspection proves it
Part must run true at one cross-sectionCircular runoutDial indicator while the part rotates on its datum
Long bearing surface must run true along its whole lengthTotal runoutIndicator moved along the surface while the part rotates
Standard or mating requirement specifically demands itConcentricityCMM — cost and time must be in the quote
No axis relationship is functionally criticalNo geometric toleranceSize tolerances are enough

In every case: name the datum — the feature that locates the part in the assembly, stated with the datum feature symbol — and state the inspection method together with the callout, so the supplier quotes the right inspection and the buyer knows what the number on the report means. A tolerance measured against a different datum is a different tolerance.

Buyer checklist

  1. The features that must share an axis are identified, and the consequence of misalignment is understood.
  2. Runout is specified instead of concentricity unless the standard or mating requirement demands concentricity.
  3. The runout value is set by the function, and only on surfaces that must run true.
  4. Total runout is used only on long functional surfaces, not as a default.
  5. The datum is the feature that locates the part in the assembly, stated with the datum symbol.
  6. The inspection method matches the callout: dial indicator for runout, CMM for concentricity.
  7. The inspection plan names the datum setup, so the measurement is repeatable.
  8. The geometric tolerance and its inspection are visible in the quote before production.

Send the drawing and state the datums and the runout your assembly actually needs in the RFQ at https://precimora.com/request-a-quote/ — the quote is promised in 24–48h.

Drawing-led production

Have a part ready for production?

Send your drawing and requirements for engineering review.

Upload DrawingTalk to an Engineer
WhatsApp