Engineering
GD&T Reference
Look up what each geometric control actually controls, whether it needs a datum, and what it does not say - which is where drawings usually go wrong.
Straightness
FormHow much a single line or axis may bow. Applied to a surface, it controls the line elements; applied to a size dimension, it controls the axis.
Datum: none - the feature is compared to itself
What it does not say: It says nothing about where the line is. A perfectly straight feature in the wrong place passes a straightness callout.
Flatness
FormHow much a surface may deviate from a plane, with no datum - the surface is compared to itself.
Datum: none - the feature is compared to itself
What it does not say: A flat face is not a parallel face. If the requirement is that two faces stay the same distance apart, the control is parallelism, and flatness alone will not hold it.
Circularity (roundness)
FormHow far a cross-section departs from a true circle, measured in one plane.
Datum: none - the feature is compared to itself
What it does not say: A part can be round at every cross-section and still be banana-shaped along its length. That is cylindricity, or straightness of the axis.
Cylindricity
FormBoth roundness and straightness of a cylinder at once - every point of the surface inside two coaxial cylinders.
Datum: none - the feature is compared to itself
What it does not say: The strictest form control there is, and the hardest to measure. It is applied when a bore has to seal or carry a bearing along its whole length, not as a general upgrade to roundness.
Perpendicularity
OrientationHow far a surface or axis may tilt from 90° to a datum.
Datum: yes - the result depends on the datum
What it does not say: The result depends on the datum being real. A perpendicularity callout off a datum that is itself unmachined transfers the roughness of the casting into the measurement.
Parallelism
OrientationHow far a surface or axis may depart from parallel to a datum.
Datum: yes - the result depends on the datum
What it does not say: It controls orientation, not separation. Parallelism does not set the distance between the faces - that is still the size dimension, and it still has a tolerance.
Angularity
OrientationHow far a surface or axis may depart from a specified angle to a datum.
Datum: yes - the result depends on the datum
What it does not say: Angularity is orientation at an angle other than 0° or 90°. Using it for a right angle works, but perpendicularity is the conventional and clearer callout.
Position
LocationWhere a feature is allowed to be, as a zone around its true position. Applied to a hole, it controls both location and, through the size, the clearance the bolt needs.
Datum: yes - the result depends on the datum
What it does not say: The most useful and most misused control. Its value is a diameter, not a radius, and it works with the feature size to determine whether a bolt fits - which is why it is quoted with a projected tolerance zone or at MMC on real assemblies.
Concentricity
LocationWhether the median points of all diametrically opposed elements of a surface are coaxial with a datum axis.
Datum: yes - the result depends on the datum
What it does not say: Difficult to measure and hard to justify. In most drawings where it appears, runout or position would express the requirement and be measurable on a lathe or a CMM with a fraction of the effort.
Symmetry
LocationWhether the median points of opposed features are centred on a datum plane.
Datum: yes - the result depends on the datum
What it does not say: Same measurement problem as concentricity, and the same advice: where the real requirement is balance or fit, a positional or profile tolerance usually says it better.
Profile of a line
ProfileHow far a cross-section of a curved surface may depart from its true profile, in one plane.
Datum: optional, depending on how it is applied
What it does not say: It controls the shape at each cross-section but not the consistency along the length - a surface can be right in every slice and still twisted.
Profile of a surface
ProfileHow far a curved surface may depart from its true profile in all directions at once, controlling size, form, orientation and location together.
Datum: optional, depending on how it is applied
What it does not say: The broadest control on this page, which is why it is used on sculpted surfaces where nothing else describes the requirement. Because it controls everything, it is also the most expensive to meet - apply it where it is needed rather than to a whole part.
Circular runout
RunoutThe full indicator movement at one cross-section while the part turns about a datum axis - form and location error combined.
Datum: yes - the result depends on the datum
What it does not say: It measures a composite of everything wrong with that section, so it cannot tell you which fault caused it. That is a strength when the requirement is "it must not vibrate" and a weakness when it is not.
Total runout
RunoutThe same indicator movement, swept along the whole surface as the part turns - roundness, straightness and coaxiality together.
Datum: yes - the result depends on the datum
What it does not say: Much stricter than circular runout because it also catches taper and bow. Specifying total runout where circular would do roughly doubles the process requirement, which is why the distinction is worth getting right.
Modifiers, and why they matter
At MMC (maximum material condition)
The tolerance applies when the feature is at its maximum material size - the smallest hole, the largest shaft.
Why it is used: It gives away tolerance as the feature departs from MMC, which is the bonus tolerance the fit can actually absorb. Common on positional callouts, because a larger hole genuinely does allow more position error with the same bolt.
At LMC (least material condition)
The tolerance applies at the least material size - the largest hole, the smallest shaft.
Why it is used: Used when minimum wall thickness matters more than fit: a hole that drifts towards a thin wall is the failure being guarded against.
RFS (regardless of feature size)
The stated tolerance applies whatever the feature measures. This is the default when no modifier is given.
Why it is used: The strictest reading, and correct when the requirement does not depend on the feature size - a bore that must be centred regardless of how the size lands.
Projected tolerance zone
Extends the tolerance zone beyond the feature, typically the thickness of the mating part.
Why it is used: Used on a tapped or clearance hole where a bolt or stud passes through another part: the position error that matters is where the bolt ends up, not where the hole starts.
Free state / restrained
Whether the tolerance is measured on the part unrestrained, or as clamped in the assembly.
Why it is used: Matters on thin and flexible parts: a plate can meet a flatness callout bolted down and fail it on the bench. The drawing has to say which one applies.
How to use this reference
- Definitions follow the ASME Y14.5 family of standards. Nothing here is a tolerance value: the numbers come from the standard, the function of the part and the process that will make it - and the shop reads them from your drawing, not from a reference page.
A reference for what each control means and what it does not say. It contains no tolerance values and it is not a drawing review - an engineer reads the callouts against the function of the part.
What you provide
- Form, orientation, location, profile or runout
Other tools