Profile and Runout
Profile of a line and of a surface, zone styles, datums, all-around and between, composite profile, and circular and total runout, with worked examples.
Profile and runout are the two controls for surfaces. Profile is the most powerful of all the geometric controls: one frame can control the form, orientation, location and, for features of size, the size of a surface of any shape, flat or curved. Runout is the control for rotating parts: how much a surface wobbles as the part turns about an axis, measured with a dial indicator. This page covers both, with zones, datums, composite profile, worked examples and a guide to choosing between runout, position and profile. It is part of the GD&T guide and follows ASME Y14.5-2018.
What profile controls
A profile tolerance is a uniform band, or zone, around a true profile: the exact shape of the surface, defined by basic dimensions or by a CAD model. The actual surface must lie inside the band everywhere. A profile of a surface controls the whole three-dimensional surface; a profile of a line controls each cross-section on its own.
| Symbol | Characteristic | Zone | Controls |
|---|---|---|---|
| Profile of a surface | A 3D band around the true surface (a pair of offset surfaces) | The whole surface: flat, cylindrical, free-form | |
| Profile of a line | A 2D band around the true line in each cross-section | The shape of each section, not how the sections relate |
- Basic shape. The true profile is not toleranced by ±; its dimensions are basic (boxed), or the whole part is defined by a model that is declared the authority.
- One control for many things. A profile tolerance on a flat face can replace flatness, parallelism, perpendicularity or location of the face, depending on which datums it references. That is why it is so widely used on cast, molded, formed and machined shapes.
- It applies to the surface, not to an axis, so it is measured on the actual surface, which a CMM can scan directly.
What the datums change
The datum references in a profile frame decide how much the profile controls. Because the zone is a band around the true shape, the more datums that are named, the more degrees of freedom of the band are fixed, and the more things the single tolerance controls:
| Datum references | The band is… | Profile controls | Replaces |
|---|---|---|---|
| None | Free to float and tilt to fit the surface | Form (the shape only) | Flatness, circularity, cylindricity for a curved or flat shape |
| Primary datum only (A) | Held at the correct angle to A, free to slide | Form and orientation to A | Perpendicularity, parallelism, angularity |
| A full frame (A | B | C) | Fixed in position by the datum reference frame | Form, orientation and location | Position of a surface; size of a profile feature of size too |
The shape is the same in each case; only the freedom of the band changes. This is why a model-based drawing often has a general profile of a surface tolerance, say 0.5 to A | B | C for the whole part, with tighter local tolerances where the function needs them.
Equal, unilateral and unequal zones
- Equal bilateral is the default: a profile of 0.3 means 0.15 on each side of the true profile.
- Unilateral: the whole tolerance on one side of the true profile. It was originally shown by drawing a phantom line parallel to the surface. When the zone lies wholly on the outside of the material, the surface may never go below the true profile (inside the material), which preserves a minimum wall or a mating clearance.
- Unequally disposed (Ⓤ) is the general form: a total tolerance, and a value after Ⓤ that says how much of it lies outside the true profile (away from the material); the remainder lies inside. For example 0.3 Ⓤ 0.2 is a 0.3 zone, 0.2 outside and 0.1 inside. Check the standard’s figures for the exact meaning of the number on your edition.
- Choose a unilateral or unequal zone when the part has to be at or on one side of the nominal: a mating surface that needs clearance, a sealing face that must not be below a gasket line, a casting with a machining allowance.
All around, all over and between
A profile frame normally applies to the one surface that the leader points to. Three symbols extend it:
| Symbol on the drawing | Meaning | Example |
|---|---|---|
| All around: a small circle at the bend of the leader | The tolerance applies to every surface around the part’s outline in the view (a closed outline made of connected surfaces) | The outline of a plate or the cross-section of an extrusion |
| All over: a larger circle with a second circle inside | The tolerance applies to every surface of the part, in all views | A casting or molding, with a general profile tolerance |
| Between: a double arrow with two letters, for example A ↔ B | The tolerance applies only to the surfaces between the two points marked A and B | One section of a curved surface that needs a tighter tolerance than the rest |
These let one frame replace many. A cast housing, for example, can carry | profile of a surface | 1.5 | A | B | C | all over, with a tighter 0.3 | A | B | C between two points on a mating face.
Composite profile
Like composite position, a composite profile frame has two rows that share one symbol: an upper row for the overall location of the surface, and a lower, tighter row for its shape and orientation.
| Row | Controls | Datums | Example |
|---|---|---|---|
| Upper (pattern-locating) | Location of the surface from the datum reference frame, together with its form and orientation | Full datum reference frame | Profile 1.5 to A | B | C |
| Lower (feature-relating) | Form and orientation only, at a tighter value | Usually the primary datum (or primary and secondary); location is not controlled | Profile 0.3 to A |
Use composite profile for a cast or molded surface whose position on the part is loose (1.5) but whose shape must be tight (0.3), such as a sealing groove or a mating contour. The shape band can float within the large location band.
Profile of a line
Profile of a line controls the shape of each cross-section separately, in the plane of the view, so each section must lie inside a thin band around the true line, but the bands in different sections need not line up. It is for shapes whose section matters more than the 3D surface:
- Extrusions and rolled sections whose profile is constant along the length, where bending along the length is separately controlled by straightness.
- Aerofoil and blade sections that are measured at specified stations.
- Cams and templates where the outline in one plane is what counts.
- A cheaper way to control a section than the whole surface, for instance where twist or taper along the length is allowed.
Runout: circular and total
Runout controls how much a surface moves, as measured by an indicator, when the part is rotated about a datum axis. It combines form and location of the surface relative to the axis into one number that is easy to measure on a lathe, between centers, or on V-blocks.
| Symbol | Control | What the indicator reads | Where |
|---|---|---|---|
| Circular runout | The indicator stays in one place on the surface (a circular element), and the part turns one revolution. The full movement must not exceed the tolerance. It is checked separately at each position along the part. | Cylinders and cones (a radial or conical element); a face (an axial circular element) | |
| Total runout | The indicator moves along the whole surface while the part turns (a straight line parallel to the axis for a cylinder, or radially across a face). The full movement over all of it must not exceed the tolerance. | Cylinders and faces; a stricter control that includes taper and bow |
- A datum axis is required, normally from a pair of journals or centers (A-B) or from a bore. Runout is measured about that axis, so the datum feature itself must be good.
- Radial and axial. On a cylinder the indicator is perpendicular to the axis (radial runout). On a flat face it is parallel to the axis (axial runout, also called face runout, and on a face total runout is like perpendicularity to the axis).
- It is the sum of two things: how far the surface’s axis is from the datum axis (eccentricity), and how out of round (and straight) the surface is. A surface offset by e gives a reading of 2e, so a perfectly round surface with a circular runout of 0.05 has its axis within 0.025 of the datum axis.
- Circular runout is a cheaper control than total runout, and total is cheaper to write than a series of position and form controls.
Runout, position or profile?
| The need | Use | Why |
|---|---|---|
| A rotating surface must not wobble (a pulley, a gear journal, a brake rotor) | Total runout | It reads exactly what causes vibration, and it is easy to measure |
| A diameter must line up with another (a bearing seat to a shaft journal) | Circular runout or position | Runout when the surface is round and quick checks matter; position to control the axis, with bonus tolerance and gages |
| A flat face must be square to the axis of a rotating part (a flange, a gear’s back face) | Total runout of the face (axial) | It combines flatness and squareness to the axis in one reading |
| A surface of any shape must be where the model says | Profile of a surface | It controls location and shape in one frame |
| Only the shape of each cross-section matters | Profile of a line | Each section floats |
| An axis (not a surface) must be in a precise place, with clearance | Position (Ⓜ) | Runout cannot use bonus tolerance and does not distinguish the axis from the surface form |
Worked examples
Example 1: checking points against a profile band
A curved surface has a profile of a surface of 0.3 to A | B | C. A CMM measures the distance of five points from the CAD surface, in mm, with a positive sign for outside the material:
| Point | Deviation | Equal zone (±0.15) | Unequal zone 0.3 Ⓤ 0.2 (−0.10 to +0.20) |
|---|---|---|---|
| Point 1 | +0.12 | pass | pass |
| Point 2 | −0.08 | pass | pass |
| Point 3 | +0.19 | fail | pass |
| Point 4 | −0.04 | pass | pass |
| Point 5 | +0.21 | fail | fail |
- Equal zone: the limits are ±0.15. Points 3 (+0.19) and 5 (+0.21) are outside, so the surface fails.
- Unequal zone 0.3 Ⓤ 0.2: 0.2 outside and 0.1 inside gives limits of −0.10 to +0.20. Point 5 (+0.21) is just outside; points 3 (+0.19) and 2 (−0.08) are inside. The surface still fails, by 0.01.
- The moral: the same surface can pass or fail depending on how the zone is disposed, so the drawing’s zone style has to say which side matters.
Example 2: reading runout on a shaft
A shaft ⌀40 has circular runout 0.05 to A-B on its middle diameter. In the V-block set-up the indicator’s full movement over one revolution is read at three places along it:
| Position | FIM (mm) | Result against 0.05 |
|---|---|---|
| Left end | 0.032 | pass |
| Middle | 0.036 | pass |
| Right end | 0.041 | pass |
- All three readings are below 0.05, so the shaft passes circular runout. Each position is judged separately.
- If the same readings had to meet a total runout of 0.05, the indicator would be traced along the surface and the largest overall range counted. The three readings (up to 0.041) differ in axis position too; the combined movement could be larger than any single section, so total runout may fail where circular passes.
- If the surface were perfectly round, an FIM of 0.041 would mean the axis is 0.041 ÷ 2 = 0.0205 from the datum axis. Any out-of-roundness is included in the reading.
Example 3: a composite profile on a cast contour
A cast sealing contour has a composite profile: upper 1.5 to A | B | C, lower 0.3 to A.
- The contour may sit anywhere inside a 1.5 band around the nominal location, because the cast part is located loosely in its housing.
- But its shape must be correct to a 0.3 band that is held square to A. The shape band floats inside the 1.5 band.
- A measured contour whose shape holds within a 0.2 band, and which sits 0.5 away from nominal at its worst point, passes: the 0.5 shift is inside the ±0.75 location band, and the 0.2 shape band fits inside the 0.3 refinement.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Profile tolerance is hard to inspect | There is no CAD model or the model is not the authority | State on the drawing that the model defines the true profile; give datum targets |
| Part passes profile but does not fit | A zone that is equal on both sides allows the surface to go inside the clearance | Use a unilateral or unequally disposed zone on the side that matters |
| Runout reading drifts as the part turns | The part is not held on its datum axis, or it floats on the supports | Use centers or a mandrel; hold it against an end stop |
| Runout fails but the part runs true in the machine | The datum journals have form error, so the datum axis is not the real axis | Control the journals’ circularity or cylindricity; use a common datum A-B |
| Total runout fails but circular passes | The surface is tapered or bowed along its length | Check straightness or taper; correct the set-up or the grinding |
| Cast profile fails everywhere | The datum targets are not where the foundry located the pattern | Agree the datum scheme with the foundry; use datum targets on the casting |
Related
- GD&T: the overview and quick reference.
- Datums and Datum Reference Frames: datum targets for castings and a common axis A-B.
- Position and Location: locating axes, and the coaxial alternative to concentricity.
- Form Tolerances: circularity and cylindricity of the journals that runout is measured from.
- Inspection and Tolerance Stack-up: how profile is scanned and runout is set up.
FAQ
What does “full indicator movement” (FIM) mean?
The total travel of the indicator needle from its lowest to its highest reading during the measurement. It is the difference between the highest and lowest values, not a ± value. Older drawings said TIR (total indicator reading) for the same thing.
Is runout the same as concentricity?
No. Runout reads the surface with an indicator and so includes the surface’s own out-of-roundness. Concentricity (removed in ASME 2018, still in ISO) is about the centers of cross-sections and is much harder to measure.
Do I have to give datums for profile?
No. With no datum, profile is a form control. With datum A only it also controls orientation, and with a full reference frame it also controls location. The choice is the whole point of the control.
Can profile be used on a feature of size?
Yes. A profile of a surface on a hole or slot controls its size, form, orientation and location together, if both sides of the feature are covered. It is common on molded parts and sheet-metal features.
What is the difference between “all around” and “all over”?
All around is for the surfaces that make up the outline in the view where the leader is shown. All over includes every surface of the part, in all views.
Which is better, circular or total runout?
Neither is better: total runout is stricter. Use circular runout for sections that matter independently, and total runout when taper, bow and overall wobble have to be limited too.
Why is the zone symmetrical by default?
Because the true profile is the middle of the tolerance, and most parts are equally happy with errors on either side. Where that is not true, use a unilateral or unequally disposed zone.
References
- ASME Y14.5-2018, Dimensioning and Tolerancing (profile, composite profile, runout, and the all-around, all-over and between symbols).
- ASME Y14.5.1M, Mathematical Definition of Dimensioning and Tolerancing Principles.
- ISO 1101, Geometrical tolerancing, and ISO 1660, Profile tolerancing.
- ASME Y14.41, Digital Product Definition Data Practices (model-based definition and profile).
- Meadows, J. D., Geometric Dimensioning and Tolerancing: Applications, Analysis, Gaging and Inspection, CRC Press.
Last reviewed: October 2026. Symbols and the meaning of the unequally-disposed value differ slightly between editions and between ASME and ISO: check the standard your drawing names.