GD&T Symbols and Geometric Tolerances

Controls the actual location of a feature of size (hole, shaft, slot, median plane) relative to a datum reference frame, comparing its actual location with its true (theoretically exact) position defined by basic dimensions. The tolerance zone is normally a cylinder (with ⌀, for holes or shafts) or two parallel planes (for slots or median planes) centered exactly on the basic position. It is a clear improvement over the classic ± coordinate tolerancing method: it defines a real (circular) acceptance zone rather than a square one, giving more usable area for the same functional control.

Controls that a feature (face, axis or median plane) is at 90° to the referenced datum. It is an orientation tolerance: it says nothing about the form of the feature itself (a face can be perfectly perpendicular on average and still not be flat, which is why flatness should also be specified where it applies). With ⌀ in front of the value, the tolerance zone is a cylinder around the theoretically perpendicular axis; without it, it is two parallel planes oriented at 90° to the datum.

Controls that a feature (face, axis or median plane) stays parallel to the datum, with no theoretical angle other than 0°. The tolerance zone is two planes (or a cylinder, if ⌀ is specified) parallel to the datum, separated by the stated value. As with perpendicularity, it does not control the feature's own form: a face can be parallel to its datum on average and still not be flat.

Limits the variation of an actual surface relative to two theoretical parallel planes separated by the tolerance value: the entire surface must fit between the two planes, regardless of its orientation to other faces of the part (which is why it takes no datum). Passing flatness does not guarantee that the face is square or parallel to another one — that is controlled separately by perpendicularity and parallelism.

Combines into a single requirement the circularity of every cross section, the straightness of the surface elements (longitudinal lines) and taper along the entire cylindrical surface. The tolerance zone is two coaxial cylinders separated radially by the stated value, within which the entire actual surface must lie. Because it requires no datum, it is the most complete cylindrical form tolerance and also the most expensive to achieve and inspect.

Limits the radial variation of a circular cross section from a perfect circle, evaluated in a plane perpendicular to the axis at a given location — not along the whole part (that is what cylindricity is for). The tolerance zone is two concentric circles separated radially by the stated value; the actual section must lie between them. It needs no datum: it is the circularity of that section relative to itself, not relative to an external reference axis.

Limits the deviation of an actual line (a surface element, an edge or the axis of a cylinder) from a theoretically perfect straight line. The tolerance zone is the space between two parallel lines separated by the stated value, and it is evaluated point by point along that line. It is a pure form tolerance: by default it takes no datum, and it controls only the specific line called out on the drawing (an edge, a surface element seen in profile), not necessarily the whole axis of the part — that is what axis straightness is for.

Controls the orientation of a feature at a theoretical angle (a basic dimension, shown in a box) other than 0° or 90° to a datum — for those two specific cases, parallelism and perpendicularity are used. The tolerance zone is a band oriented exactly at the basic angle: the tolerance value is always expressed in linear units (mm), like every other GD&T tolerance, never in degrees or minutes.

Requires the midpoint of every cross section of the controlled feature (not the whole surface, but the center of each section) to coincide with the datum axis. It is one of the most demanding and hardest-to-verify tolerances in the entire GD&T system, because it requires evaluating the center of an infinite number of sections rather than the surface as a whole.

Controls how closely the derived axis of a cylindrical feature coincides with the axis of a datum that is also cylindrical. Unlike concentricity (which compares the centers of individual sections), coaxiality compares the full axis of the feature with the datum axis, treating both as derived straight lines.

Controls that a median feature (slot, tab, median plane) is centered on the median plane of the datum. The tolerance zone is two parallel planes, equidistant from the datum median plane, within which the actual median plane of the controlled feature must fall.

Two or more rows within a single feature control frame, sharing the symbol and datums but with different values: the upper row (PLTZF, pattern-locating tolerance zone framework) controls the location of the whole pattern relative to the datum reference frame; the lower row (FRTZF, feature-relating tolerance zone framework) controls only the geometric relationship of the pattern features to one another, usually with a tighter tolerance. They are not two independent requirements: the lower-row zone must fall within the upper-row zone for each feature.

Indicates, by means of the numeric prefix (4×, 6×, etc.) or the note “PATTERN”, that the geometric tolerance in the feature control frame applies to the complete set of repeated features as a single pattern, not to each feature in isolation with its own dimensional tolerance. All the features in the pattern share the same datum reference frame and the same theoretical tolerance zone framework.

At the feature's maximum material condition (MMC), the permitted geometric deviation is exactly zero: the feature must be perfectly at its theoretical location when it is at its worst-case size limit. The available geometric tolerance only appears (grows) as the actual size of the feature departs from MMC toward LMC — hence the “0” next to the symbol in the feature control frame instead of a fixed value.

Controls, at a specific cross section, the total variation (combining form and location) of a circular feature or a face as it rotates 360° about the datum axis. Unlike circularity (which requires no datum), circular runout does depend on how the part is held on the reference axis: eccentricity, ovality and misalignment are mixed into a single reading, without distinguishing which of the three causes the error.

Controls the combined variation of form, orientation and location of an entire surface (not just one section) as it rotates about the datum axis, with the indicator traversing the full length or face at the same time as the part rotates. It is more demanding than circular runout because it accumulates the error of every section into a single reading: a part can pass circular runout section by section and still fail total runout if the error pattern changes progressively along the part (for example, a slight taper).

Controls the form of a complete surface (not just one section) relative to the theoretical three-dimensional model (CAD or basic dimensions), and can replace several form, orientation and location tolerances with a single requirement if the drawing explicitly says so (profile as a composite tolerance). The tolerance zone is an envelope of constant thickness around the entire nominal surface.

Controls the form of a line (the outline seen in a specific cross section) relative to the theoretical profile defined by basic dimensions or by the CAD model, without comparing the whole 3D surface (that is what profile of a surface is for). The tolerance zone is a band that follows the theoretical outline, with a width equal to the stated value; it can be split equally on both sides of the nominal profile or unequally disposed (with the ⊕/⊖ modifier) toward one side.

Extends the scope of a profile tolerance (line or surface) so that it automatically applies to the ENTIRE closed outline shown in that view, without having to dimension each segment separately. It is indicated by a small circle at the elbow of the feature control frame leader ("all around"). This is different from applying profile only to a segment marked with a thick line: without the circle, profile controls only the segment explicitly indicated.

Straightness applied to the derived median line (the theoretical center) of a cylindrical feature, not to its surface. With ⌀ in front of the value, the tolerance zone is an imaginary cylinder of that diameter within which the actual axis must lie along its entire length — not a pair of planes as in line straightness. It is the correct way to control the full axis of a rod or stud; because it applies to a feature of size, it is the only form of straightness that accepts Ⓜ or Ⓛ.