CNC / machinist reference

GD&T Symbols and Rules

The 14 geometric characteristic symbols of ASME Y14.5-2009 (the 2018 edition dropped two, leaving 12), grouped by their five categories, with whether each uses a datum and can take a material modifier, plus the modifiers, datums and how to read a feature control frame. A reference, sourced and kept honest about the 2018 revision.

The 14 geometric characteristics

Each control belongs to one of five categories. Form controls a feature against itself and never uses a datum; orientation and runout always reference a datum; location references datums; profile may use one or not. "FOS only" means the modifier applies only in the axis or center-plane (feature-of-size) form of that control.

Form (controls a feature against itself, never a datum)

Control	Datum	Modifier	What it controls
Straightness	No	FOS only	Straightness of a line element on a surface, or of an axis.
Flatness	No	No	How flat a surface is.
Circularity	No	No	Roundness of each individual cross-section of a round feature.
Cylindricity	No	No	The whole cylindrical surface at once: roundness, straightness and taper.

Orientation (angle to a datum; always uses a datum)

Control	Datum	Modifier	What it controls
Angularity	Yes	FOS only	A surface or axis held at a specified angle to a datum.
Perpendicularity	Yes	FOS only	A surface or axis held at 90 degrees to a datum.
Parallelism	Yes	FOS only	A surface or axis held parallel to a datum.

Location (where a feature sits relative to datums)

Control	Datum	Modifier	What it controls
Position	Usually	Yes	Location of a feature-of-size axis or center-plane. The main user of MMC/LMC and bonus tolerance.
Concentricity (removed in Y14.5-2018)	Yes	No	Median points of a feature about a datum axis. Use Position or Runout instead.
Symmetry (removed in Y14.5-2018)	Yes	No	Median points about a datum center-plane. Use Position instead.

Runout (variation as the part spins about a datum axis)

Control	Datum	Modifier	What it controls
Circular Runout	Yes	No	Variation at each cross-section as the part rotates about the datum axis.
Total Runout	Yes	No	Variation across the entire surface in one sweep about the datum axis.

Profile (a zone following the true form; datum optional)

Control	Datum	Modifier	What it controls
Profile of a Line	Optional	No	A 2D tolerance zone along individual line elements of a curved feature.
Profile of a Surface	Optional	No	A 3D zone wrapping a whole surface; the most versatile control.

Material condition modifiers and bonus tolerance

A material modifier can only be applied to a feature of size, a feature with a size dimension such as a hole or pin diameter or a slot width.

MMC (circle-M), maximum material condition: the size at which the most material exists, the smallest hole or the largest shaft. Earns bonus tolerance as the feature departs from it.
LMC (circle-L), least material condition: the opposite, the largest hole or smallest shaft. Used to protect minimum wall or edge distance.
RFS, regardless of feature size: the default when no modifier is shown. The tolerance applies at every size with no bonus.

bonus tolerance = departure from MMC; total tolerance = stated tolerance + bonus

Example: a hole with an MMC of 1.745 that actually measures at its LMC of 1.755 has departed 0.010, so it earns 0.010 of bonus positional tolerance on top of the stated value.

Datums and the feature control frame

A datum is a theoretically exact reference, a plane, axis or point, established from a real feature on the part. Datums are called out in order of precedence, primary then secondary then tertiary, and that order controls how the part is constrained and measured.

A feature control frame reads left to right like a sentence, in three compartments:

The geometric characteristic symbol, which of the 14 controls applies.
The tolerance zone: a diameter symbol for a cylindrical zone, the total tolerance value, and any material modifier.
The datum references, primary then secondary then tertiary.

Read it as: this feature is controlled within this much tolerance, referenced to these datums in this order. Form controls have no datum compartment.

What changed in ASME Y14.5-2018

The 2018 revision withdrew 2 of the characteristics in the table above: Concentricity and Symmetry. They are still legal on a drawing that invokes the 2009 standard, and you will meet them on prints for years, but they should not go on anything new.

The reason is measurement, not theory. Both controlled the location of derived median points, the set of midpoints between opposing surface elements, rather than the surfaces themselves. That is an elegant definition of what a designer usually means by concentric, and it is expensive and slow to verify: an inspector has to probe opposing points all around the feature and compute the midpoints, where a runout gauge gives an answer in seconds. In practice the symbols were also widely misapplied, used where a simple coaxiality requirement was meant, so a control that was hard to measure was frequently not even the one intended.

What to use instead, in order of how often it is the right answer:

Position for coaxiality of an axis or centre-plane. This is the direct replacement and it accepts material condition modifiers, so it can carry bonus tolerance where the old controls could not.
Circular or total runout when the part rotates and what actually matters is how much the surface moves. Cheap to check and usually what the function requires.
Profile of a surface when the requirement is really about the surface rather than a derived axis.

The 2018 revision also added rules for numbering continuous features. The withdrawal of these two symbols is the change most likely to affect a drawing you are reading today.

Which control to reach for

More than one characteristic will technically work on most features, and the table above will not tell you which to pick. The split that decides it is what the control is measured against. 4 of the characteristics take no datum at all and check a feature against itself; 7 always require one; the profile controls take one only if the requirement needs it.

Working from the function rather than the symbol:

Does the feature only need to be well made in itself? A form control, and no datum. Flatness on a mating face, cylindricity on a bearing journal.
Does it need to sit at an angle to something else? An orientation control. Perpendicularity and parallelism are the same idea as angularity at 90 and 0 degrees.
Does it need to be in the right place? Position, and this is where 5 of the 14 that accept a material modifier earn their keep: at maximum material condition a hole that comes out smaller than its limit hands the extra back as bonus tolerance, which is free manufacturing latitude that costs nothing in function.
Does the part spin? Runout, because it measures the thing the assembly actually feels.
Is the surface a curve or a shape rather than a plane or a cylinder? Profile of a surface, which is the most general control in the set and can stand in for most of the others.

A useful rule when two controls both fit: pick the one that is cheaper to inspect. The tolerance that is never checked is not a tolerance, and the one that needs a CMM programme where a dial indicator would do adds cost to every part for the life of the drawing.

Frequently asked questions

What does the circle-M modifier mean in GD&T?

It is MMC, maximum material condition. It says the stated tolerance applies when the feature is at its maximum-material size, and that bonus tolerance is earned as the feature departs from MMC. It can only be used on a feature of size.

What is the difference between Position and Concentricity?

Position locates the axis or center-plane of a feature of size and can use MMC and bonus tolerance, so it is manufacturable and easy to inspect. Concentricity controlled median points about a datum axis, was hard to measure, and was removed in ASME Y14.5-2018 in favor of Position or Runout.

When is a datum required in a feature control frame?

Form controls (straightness, flatness, circularity, cylindricity) never use a datum. Orientation and runout controls always require a datum. Location controls reference datums, and profile controls can be used with or without a datum.

What is a feature of size, and why does it matter for modifiers?

A feature of size has a size dimension, such as a hole or pin diameter or a slot width. Material condition modifiers like MMC and LMC and their bonus tolerance only apply to features of size, because they are defined relative to the size limits. A plain surface cannot take a modifier.

How do I calculate bonus tolerance?

Bonus tolerance is the departure from the material condition modifier. At MMC it equals the difference between the actual mating size and the MMC size, and it is added to the stated geometric tolerance. So the total allowable tolerance is the stated tolerance plus the bonus.

What is the difference between circular and total runout?

Both are measured as the part rotates about a datum axis and neither takes a modifier. Circular runout checks variation at each individual cross-section, while total runout checks the entire surface in one pass, so it also captures taper and profile error along the axis and is the tighter control.

Sources

This page follows ASME Y14.5. The 2009 edition defines these 14 symbols across five categories; the 2018 edition removed Concentricity and Symmetry, leaving 12, and keeps the same five categories.

These calculators are for planning and as a starting point. Recommended speeds and feeds are published starting values that vary with your specific tool, coating, machine rigidity, workholding and coolant. Always start conservative, listen to the cut, and follow your tool maker data sheet.