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.
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.
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
- GD&T symbols and their meaning (GD&T Basics)
- Geometric dimensioning and tolerancing (Wikipedia)
- ASME Y14.5 Dimensioning and Tolerancing (ASME)
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.