TLDR
Orientation tolerances (perpendicularity, parallelism, angularity) control the angular relationship of a feature to a datum. Location tolerances (true position, concentricity, symmetry) control where a feature sits relative to datums. Runout tolerances (circular and total) control surface variation during rotation. Together, these are the most frequently used GD&T controls on engineering drawings.
This guide covers each tolerance with its symbol, definition, datum requirements, measurement approach, and common applications, plus a comparison table for quick reference.
Beyond Form: The Tolerances That Control Relationships
Form tolerances (flatness, straightness, circularity, cylindricity) control the shape of individual features. They are the simplest GD&T (Geometric Dimensioning and Tolerancing) controls because they work in isolation, with no reference to other features.
But parts don’t function in isolation. Holes must be perpendicular to mounting faces. Surfaces must be parallel to reference planes. Bolt patterns must be in the right position. Shafts must not wobble.
That is where orientation, location, and runout tolerances come in. These controls define the relationships between features, and they appear on drawings far more often than form tolerances alone.
Orientation Tolerances
Orientation tolerances control the angular relationship between a feature and a datum reference. All three orientation tolerances require at least one datum. They also inherently control form within the orientation tolerance zone.
Perpendicularity (⟂)
Definition: Controls how close a feature (surface, axis, or median plane) is to being exactly 90 degrees relative to a datum.
Tolerance zone: For a surface, the zone is two parallel planes perpendicular to the datum, separated by the tolerance value. For an axis, the zone is a cylinder (if preceded by ⌀) perpendicular to the datum.
Datum requirement: Always requires at least one datum reference.
Measurement approach: For surfaces, set the part on the datum feature (or simulate the datum with a surface plate), then sweep an indicator across the controlled surface. The total indicator variation is the perpendicularity error. For axes, measure multiple points along the feature and evaluate the axis deviation from perfect perpendicularity using a CMM (Coordinate Measuring Machine).
Common applications: Dowel pin holes that must be square to a mounting face. Walls that must be at right angles to a base. Press-fit bosses that locate components perpendicularly. Threaded holes where bolt alignment depends on the hole being perpendicular to the mating surface.
Key point: Perpendicularity refines form. A perpendicularity tolerance of 0.05 mm means the surface must also be flat within 0.05 mm. You do not need a separate flatness callout unless flatness must be tighter than perpendicularity.
Parallelism (∥)
Definition: Controls how close a feature is to being exactly parallel to a datum. The controlled feature must maintain a consistent distance from the datum within the specified tolerance.
Tolerance zone: Two parallel planes (or a cylinder for an axis) that are parallel to the datum, separated by the tolerance value.
Datum requirement: Always requires at least one datum reference.
Measurement approach: Place the datum surface on a surface plate. Sweep an indicator across the controlled surface. The total indicator variation represents the parallelism error. On a CMM, take points on both the datum feature and the controlled surface, then calculate the angular and distance deviation.
Common applications: Top and bottom surfaces of a machined block. Rails that must stay equidistant. Shaft axes that must remain parallel to a reference surface. Valve body faces where parallel mating surfaces prevent leaks.
Key point: Like perpendicularity, parallelism inherently controls form. If you specify parallelism of 0.03 mm, the surface must also be flat within 0.03 mm.
Angularity (∠)
Definition: Controls how close a feature is to a specified angle (other than 0° or 90°) relative to a datum. The basic angle is stated on the drawing; the angularity tolerance controls how tightly the feature must conform to that angle.
Tolerance zone: Two parallel planes oriented at the basic angle to the datum, separated by the tolerance value.
Datum requirement: Always requires at least one datum reference.
Measurement approach: Set up the datum reference on an angle plate or fixture that orients the part so the basic angle aligns with the measurement axis. Sweep an indicator across the controlled surface. Alternatively, use a CMM to take points and calculate the angular deviation from the basic angle relative to the datum.
Common applications: Chamfers, tapered surfaces, V-block features, angled mounting faces, and any feature specified at an angle other than 0° or 90° to a reference.
Key point: Angularity does not control the angle itself (that is defined by the basic dimension). It controls how tightly the surface conforms to that angle. The basic dimension is exact; the angularity tolerance defines the allowable variation.
Location Tolerances
Location tolerances control where a feature is positioned relative to a datum reference frame. They are about placement, not angular relationship.
True Position (⊕)
Definition: Controls how close the actual location of a feature (typically its axis or center plane) is to its theoretically exact position, defined by basic dimensions from datum references. This is the most frequently used GD&T symbol.
Tolerance zone: Typically a cylinder (when preceded by ⌀) centered on the theoretically exact position. Can also be two parallel planes for features like slots.
Datum requirement: Always requires datum references to establish the coordinate system from which the theoretically exact position is measured.
Measurement approach: Measure the actual location of the feature (hole center, pin center, slot center) relative to the datum reference frame. Calculate the deviation from the theoretically exact position. For cylindrical tolerance zones, the positional deviation is calculated as:
Positional deviation = 2 × √(ΔX² + ΔY²)
where ΔX and ΔY are the deviations in each axis from the basic dimensions. The result is compared to the diametrical tolerance zone.
Common applications: Bolt hole patterns, pin locations, slot centers, connector mounting holes, and virtually any feature whose position relative to a datum reference frame determines whether the part assembles correctly.
Key point: True position is almost always used with basic dimensions (theoretically exact, no tolerance applied to the dimension itself). The tolerance lives entirely in the feature control frame. Material condition modifiers (MMC, LMC) are commonly applied to true position, enabling bonus tolerance.
Concentricity (◎) and Symmetry (⌯)
Concentricity controls the relationship of the median points of a feature of size to the axis of a datum feature. Symmetry does the same for the median points of a feature relative to the center plane of a datum feature.
Both are rarely used in practice because they require deriving median points, which is time-consuming and expensive to inspect. In most applications, true position or runout provides the same functional control with simpler measurement methods. Many experienced practitioners recommend avoiding these symbols unless the design specifically requires median-point control.
Runout Tolerances
Runout tolerances control how much a surface varies during a full 360-degree rotation about a datum axis. They combine elements of form, orientation, and location control in a single measurement.
Circular Runout (↗)
Definition: Controls the surface variation at each individual circular cross-section as the part makes one full rotation about a datum axis. Each cross-section is evaluated independently.
Tolerance zone: At each cross-section, the Full Indicator Movement (FIM) must not exceed the specified value.
Datum requirement: Always requires a datum axis (often established by centers, a bearing journal, or a datum diameter).
Measurement approach: Mount the part on its datum axis (between centers, in a chuck on the datum feature, or on V-blocks). Place an indicator on the controlled surface. Rotate the part one full turn. Record the FIM. Repeat at multiple cross-sections.
Common applications: Bearing journals, pulley grooves, gear ODs, and any rotating surface where eccentricity at individual cross-sections would cause vibration or uneven contact.
Key point: Circular runout does not detect taper because it checks each cross-section independently. A shaft that is perfectly round at every cross-section but tapers along its length would pass circular runout but fail total runout.
Total Runout (↗↗)
Definition: Controls the surface variation of the entire feature simultaneously as the part rotates. An indicator sweeps across the full surface during rotation, and the total FIM across all positions must not exceed the tolerance.
Tolerance zone: The total variation across the entire surface during rotation must not exceed the specified value. This captures eccentricity, taper, waviness, and out-of-round simultaneously.
Datum requirement: Always requires a datum axis.
Measurement approach: Mount the part on its datum axis. Place an indicator on the surface and sweep it axially across the feature while rotating the part. The total FIM across the entire surface is the total runout value.
Common applications: Precision shafts, print rollers, spindles, and any cylindrical surface where the combined effect of eccentricity, taper, and surface irregularity must be controlled.
Key point: Total runout is more restrictive than circular runout. It captures taper and axial variation that circular runout misses. Use total runout when the entire surface must function as a single, consistent reference.
Comparison Table: Orientation, Location, and Runout Tolerances
| Tolerance | Symbol | Category | What It Controls | Datum? | Controls Form? |
|---|---|---|---|---|---|
| Perpendicularity | ⟂ | Orientation | 90° to datum | Yes | Yes |
| Parallelism | ∥ | Orientation | Parallel to datum | Yes | Yes |
| Angularity | ∠ | Orientation | Specified angle to datum | Yes | Yes |
| True Position | ⊕ | Location | Feature placement | Yes | Yes |
| Concentricity | ◎ | Location | Median points to axis | Yes | Yes |
| Symmetry | ⌯ | Location | Median points to plane | Yes | Yes |
| Circular Runout | ↗ | Runout | Surface per cross-section | Yes (axis) | Yes (at each section) |
| Total Runout | ↗↗ | Runout | Entire surface | Yes (axis) | Yes (entire surface) |
How These Tolerances Work Together
On a typical part drawing, you will often see multiple types of tolerances applied simultaneously. A bolt hole might have true position controlling its location, while the surface it passes through has perpendicularity controlling the hole’s angular relationship to the mounting face.
The hierarchy of GD&T controls is worth understanding: location controls inherently refine orientation, and orientation controls inherently refine form. A true position tolerance of 0.5 mm also limits the feature’s orientation and form to within that 0.5 mm zone. Adding a separate perpendicularity or flatness callout only makes sense when the tighter control is needed.
Runout is often chosen as an alternative to position or orientation for rotating parts because it is simple to measure with an indicator and captures multiple types of geometric error in a single check.
Stay Current on Automotive Quality
PPAP updates, GD&T guidance, and practical quality resources delivered to your inbox. No spam, just what quality professionals need to know.
SubscribeFrequently Asked Questions
What is the difference between perpendicularity and true position?
Perpendicularity controls the angular relationship of a feature to a datum (specifically 90 degrees). True position controls where a feature is located relative to a datum reference frame. A hole could be perfectly perpendicular but in the wrong location, or in the right location but tilted. They control different aspects of a feature’s geometry.
When should you use runout instead of true position?
Use runout when the part rotates in service and the primary concern is surface variation during rotation. Runout is easier to measure (indicator on a rotating part) and captures eccentricity, out-of-round, and taper in a single check. Use true position when the concern is the location of a feature’s axis relative to a datum reference frame, regardless of rotation.
Do orientation tolerances control form?
Yes. Orientation tolerances (perpendicularity, parallelism, angularity) inherently control the form of the feature within the orientation tolerance zone. If parallelism is specified as 0.03 mm, the surface must also be flat within 0.03 mm. A separate form tolerance is only needed when form must be tighter than the orientation tolerance.
What is the difference between circular runout and total runout?
Circular runout checks surface variation one cross-section at a time during rotation. Total runout checks the entire surface simultaneously during rotation. Total runout is more restrictive because it captures taper, waviness, and eccentricity across the whole feature, not just at individual sections.
Can true position be applied without MMC?
Yes. When no material condition modifier is specified, the default condition is RFS (Regardless of Feature Size) per ASME Y14.5-2009 and later. The tolerance value applies at any produced size of the feature, with no bonus tolerance. MMC is commonly applied to true position for assembly-fit applications, but RFS is used when the tolerance must be maintained regardless of size.
Why are concentricity and symmetry rarely used?
Both require deriving median points from measured data, which is expensive and time-consuming. The results are often difficult to reproduce between different measurement setups. In most applications, true position (for location control) or runout (for rotating parts) achieves the same functional result with simpler, more repeatable measurement methods.
How does the GD&T tolerance hierarchy work?
Location tolerances are the broadest; they inherently refine both orientation and form. Orientation tolerances refine form but do not control location. Form tolerances control only shape. This means a true position tolerance of 0.5 mm also limits orientation and form to 0.5 mm. You only add a tighter orientation or form tolerance when that specific aspect needs stricter control than the location tolerance provides.
Leave a Comment