Geometric Dimensioning and Tolerancing is a system for communicating design intent through engineering drawings. Instead of just saying "this surface should be flat to within 0.005 inches," GD&T specifies exactly what "flat" means, how it is measured, and what reference features establish the measurement frame. The result is clearer drawings, fewer arguments between design and manufacturing, and parts that function correctly even when individual dimensions are not all at nominal.
\nThis guide covers the 14 geometric tolerance symbols defined in ASME Y14.5-2018, organized by the five tolerance categories. The explanations use plain shop language, not the abstract definitions from the standard. If you can understand what the symbol controls and how the inspector checks it, you can machine the part correctly.
The Five Tolerance Categories
Form (4 symbols): Straightness, Flatness, Circularity, Cylindricity. These control the shape of a single feature without reference to any other feature. No datums are required. Form tolerances answer the question: "Is this feature the correct shape, regardless of where it is or how it is oriented?"
\nProfile (2 symbols): Profile of a Line, Profile of a Surface. These control the shape of a feature relative to its true profile (the theoretically perfect shape from the CAD model). Profile tolerances can be used with or without datums, depending on whether the profile must also be located and oriented relative to other features.
\nOrientation (3 symbols): Angularity, Perpendicularity, Parallelism. These control the orientation of a feature relative to a datum. They require at least one datum reference. Orientation tolerances answer: "Is this feature at the correct angle relative to the reference feature?"
\nLocation (3 symbols): Position, Concentricity, Symmetry. These control the location of a feature relative to datums. They always require datum references. Position is the most commonly used GD&T symbol overall. Concentricity and Symmetry are legacy symbols in Y14.5-2018.
\nRunout (2 symbols): Circular Runout, Total Runout. These control the form and location of a surface relative to a datum axis, measured with the part rotated. Used primarily for rotating components (shafts, bores, cylindrical surfaces). Always require a datum axis.
1. Position — Controls hole and feature locations
2. Flatness — Controls mating surface quality
3. Perpendicularity — Controls squareness to datums
4. Profile of Surface — Controls complex 3D shapes
5. Circular Runout — Controls rotating part surfaces
These five cover roughly 90% of GD&T callouts on typical machined parts.
GD&T Quick Reference
Interactive GD&T reference for all 14 geometric tolerances per ASME Y14.5. Plain-English explanations, feature control frames, inspection methods, and common mistakes.
Reading a Feature Control Frame
The feature control frame is the rectangular box on the drawing that contains the GD&T callout. Read it left to right, compartment by compartment:
\nFirst compartment: The geometric tolerance symbol. This tells you what type of tolerance is being applied (flatness, position, perpendicularity, etc.).
\nSecond compartment: The tolerance value. If preceded by a diameter symbol (ø), the tolerance zone is cylindrical. Otherwise it is two parallel planes (width zone). The number is the total tolerance zone width or diameter in the drawing units.
\nOptional modifier after tolerance: A circled M means MMC (Maximum Material Condition), a circled L means LMC (Least Material Condition). If no modifier is shown, the default is RFS (Regardless of Feature Size) in Y14.5-2018.
\nRemaining compartments: Datum references, listed in order: primary (most important), secondary, tertiary. Each datum letter may also have a material condition modifier. Not all tolerance types require datums — form tolerances have no datum references.
[Symbol] | [ø] [Tolerance] [Modifier] | [Datum A] [Mod] | [Datum B] [Mod] | [Datum C] [Mod]
Example: Position | ø 0.010 (M) | A | B | C
Reads: "The true position of this feature shall be within a cylindrical zone of 0.010 diameter at MMC, relative to datums A (primary), B (secondary), and C (tertiary)."
MMC, LMC, and RFS: When Size Affects Tolerance
MMC (Maximum Material Condition): The condition where the feature contains the most material. For a shaft, MMC is the largest diameter. For a hole, MMC is the smallest diameter. When MMC is specified in a feature control frame, the tolerance zone gets larger (bonus tolerance) as the feature departs from MMC. The logic: if the hole is bigger than the minimum, you have more room for position error and the parts will still assemble.
\nLMC (Least Material Condition): The opposite of MMC. For a shaft, LMC is the smallest diameter. For a hole, LMC is the largest diameter. LMC bonus tolerance is used when the concern is maintaining minimum wall thickness or minimum material between features. It is much less common than MMC.
\nRFS (Regardless of Feature Size): The tolerance zone stays the same size no matter what the actual feature size is. No bonus tolerance. RFS is the default in ASME Y14.5-2018 — if no modifier is shown after the tolerance value, RFS is assumed. Use RFS when the tolerance must be maintained at all possible feature sizes.
\nThe practical impact: MMC is most commonly applied to position tolerance on bolt patterns. If every hole in the pattern is at minimum size (MMC), the position tolerance is as stated on the drawing. If the holes are drilled oversize (within their size tolerance), the position tolerance gets a "bonus" equal to the amount of departure from MMC. This means parts that would technically fail a position check at RFS might pass at MMC — because the larger holes compensate for the position error.
Available position tolerance = Stated tolerance + (Actual size - MMC size)
Example: ø0.010 position at MMC, hole size tolerance 0.500-0.510
At MMC (0.500): available tolerance = 0.010
At 0.505: available tolerance = 0.010 + 0.005 = 0.015
At LMC (0.510): available tolerance = 0.010 + 0.010 = 0.020
Tolerance & Fit Calculator
ISO 286 tolerance zone calculator for shaft/hole fits. Calculates clearance, transition, and interference fits with visual tolerance zone diagram and common fit presets (H7/g6, H7/h6, H7/p6, etc.).
Datums: The Reference Frame for Everything
Datums are the reference features that establish the coordinate system for measuring geometric tolerances. Without datums, you cannot define where a feature should be or how it should be oriented. The datum reference frame is a set of three mutually perpendicular planes (like an XYZ coordinate system) established by contacting the datum features on the part.
\nThe primary datum is the most important reference surface. It establishes the first plane of the datum reference frame and constrains 3 degrees of freedom (a flat surface eliminates translation in one axis and rotation about two axes). In the feature control frame, the primary datum is listed first (closest to the tolerance value).
\nThe secondary datum constrains 2 additional degrees of freedom (typically another surface perpendicular to the primary). The tertiary datum constrains the last degree of freedom (typically a hole or edge perpendicular to both primary and secondary).
\nThe order matters. Datum A | B | C means the part is first seated on datum A (primary), then aligned to datum B (secondary), then located by datum C (tertiary). Changing the order changes how the part is fixtured for inspection and machining — which can change whether the part passes or fails geometric tolerances.
The primary datum should be the surface the part sits on during machining. The secondary datum should be the surface it pushes against for alignment. The tertiary datum should be the feature that locates it in the remaining direction.
If the inspection datums match the machining datums, the part will measure well. If they do not match, you may machine a good part that fails inspection due to datum shift.
GD&T Quick Reference
Interactive GD&T reference for all 14 geometric tolerances per ASME Y14.5. Plain-English explanations, feature control frames, inspection methods, and common mistakes.