GD&T (Geometric Dimensioning and Tolerancing) is the engineering language that defines part geometry with mathematical precision — understanding all 14 geometric tolerance symbols is essential for anyone who designs, manufactures, or inspects mechanical components.
Coordinate tolerancing with ±XY dimensions worked adequately for simple parts, but it breaks down on complex assemblies where form, orientation, and location of features must be controlled simultaneously. GD&T, standardized in ASME Y14.5-2018 and ISO 1101:2017, provides a complete, unambiguous framework. This article covers all 14 geometric tolerances, organized by the five categories defined in the standards, with drawing callout examples and practical applications for each.
How to Read a Feature Control Frame
Every GD&T callout uses a rectangular feature control frame (FCF). Reading left to right: the first compartment contains the geometric characteristic symbol; the second contains the tolerance value (preceded by ∅ if the zone is cylindrical, followed by material condition modifiers like Ⓜ or Ⓛ); subsequent compartments contain datum references (primary, secondary, tertiary) with optional modifiers.
Example: ⊕ | ∅0.1 Ⓜ | A | B Ⓜ | C reads as: “True position, cylindrical tolerance zone diameter 0.1 at MMC, primary datum A, secondary datum B at MMC, tertiary datum C.”
Form Tolerances (No Datum Required)
Form tolerances control the shape of a single feature in isolation, without reference to any datum. They answer the question: “How perfect must this surface or line be, on its own?”
1. Straightness (—)
Straightness controls how straight a line element or axis must be. Applied to a surface, it controls individual line elements in one direction — each line must lie within two parallel planes separated by the tolerance value. Applied to a feature of size (e.g., a shaft diameter), it controls the derived median line and the tolerance zone is cylindrical: the median line must lie within a cylinder of the stated diameter.
Drawing callout example: A 30mm shaft with a feature control frame — | 0.05 — placed below the diameter dimension means each longitudinal line element of the shaft surface must lie within two parallel planes 0.05 mm apart.
2. Flatness (◻)
Flatness controls how flat an entire surface must be. The tolerance zone is the space between two parallel planes. The entire surface must lie within these planes simultaneously — this is a three-dimensional control, not just a line-by-line check. Flatness is commonly specified on sealing surfaces, machine table interfaces, and base plates.
Example: A mounting face with | ◻ | 0.02 | means the entire surface must fall within two parallel planes 0.02 mm apart. Note that flatness must always be less than the size tolerance on that feature per ASME Rule #1.
3. Circularity (○)
Also called roundness, circularity controls a single cross-sectional slice of a cylindrical, conical, or spherical surface. Each circular cross-section must lie within an annular zone defined by two concentric circles with a radial difference equal to the tolerance value. Circularity is measured perpendicular to the axis of the feature at each cross-section independently.
Example: | ○ | 0.01 | on a journal bearing surface means each circular cross-section must lie between two concentric circles 0.01 mm apart in radius — approximately equivalent to saying the out-of-roundness must not exceed 0.01 mm in any cross-section.
4. Cylindricity (⌭)
Cylindricity is the most comprehensive form control for cylindrical features. The tolerance zone is the annular space between two coaxial cylinders of radial difference equal to the tolerance value. The entire surface — all cross-sections and all longitudinal elements simultaneously — must lie within this zone. Cylindricity simultaneously controls circularity, straightness, and taper of a cylinder.
Example: | ⌭ | 0.015 | on a precision bearing bore means the entire bore surface must lie between two coaxial cylinders 0.015 mm apart in radius. This is significantly harder to measure than circularity alone and is typically reserved for critical fits.
Profile Tolerances
Profile tolerances control the shape of any line or surface — including complex curves and free-form surfaces — relative to a theoretically exact (true) profile defined by basic dimensions. They can be used with or without datums.
5. Profile of a Line (⌒)
Controls the shape of individual cross-sectional slices of a surface. The tolerance zone is the area between two curves offset equally (bilateral) or unequally from the true profile. Applied to 2D cross-sections only — each slice is evaluated independently. Used on complex cam profiles, airfoil cross-sections, and non-circular contours.
6. Profile of a Surface (⌓)
The most powerful GD&T control, profile of a surface controls the entire 3D surface simultaneously relative to datums. The tolerance zone is the volume between two surfaces offset from the true profile. When applied all-around (indicated by a circle at the leader line elbow) or all-over (two concentric circles), it can replace many individual tolerances. This is covered in depth in a dedicated article in this series.
Orientation Tolerances (Datum Required)
Orientation tolerances control how a feature is angled relative to a datum. They always require at least one datum reference.
7. Perpendicularity (⊥)
Controls how close to 90° a surface or axis is relative to a datum. For a surface, the tolerance zone is two parallel planes perpendicular to the datum. For an axis (cylindrical tolerance zone, indicated by ∅ before the value), the zone is a cylinder perpendicular to the datum.
Example: A threaded hole with | ⊥ | ∅0.1 | A | means the axis of the hole must lie within a cylinder of diameter 0.1 mm that is perfectly perpendicular to datum plane A. This ensures the fastener will not be cocked relative to the mating surface.
8. Angularity (∠)
Controls how close a surface or axis is to a specified basic angle relative to a datum. The true angle is always a basic dimension (in a rectangle box). The tolerance zone is two parallel planes at the true angle from the datum, separated by the tolerance value. Angularity applies to any angle other than 90° (use perpendicularity for 90°) or 0° (use parallelism for 0°).
Example: An angled face at a basic 45° to datum A with | ∠ | 0.05 | A | means the face must lie within two parallel planes 0.05 mm apart, both oriented at exactly 45° to datum A.
9. Parallelism (∥)
Controls how close a surface or axis is to 0° (parallel) relative to a datum. For a surface, the zone is two parallel planes parallel to the datum. For an axis, the zone can be two parallel planes or a cylinder (with ∅) parallel to the datum axis.
Example: A top face with | ∥ | 0.03 | A | where A is the bottom face means the top surface must lie within two planes 0.03 mm apart, both parallel to datum A. This is common on precision spacers and shims.
Location Tolerances (Datum Required)
Location tolerances control where a feature is located relative to datums and/or other features.
10. True Position (⊕)
Position is the most widely used GD&T symbol. It controls the location of features of size (holes, pins, slots, tabs) relative to datums and to each other. The tolerance zone for a hole is typically a cylinder (∅ specified) centered on the true (theoretically exact) position, defined by basic dimensions from datums.
Position uniquely allows material condition modifiers (Ⓜ for MMC, Ⓛ for LMC) that provide bonus tolerance — as the actual mating size departs from the modifier condition, the geometric tolerance zone increases by the same amount. This is detailed in a dedicated article on position and bonus tolerance.
Example: Four M8 holes on a bolt circle with | ⊕ | ∅0.3 Ⓜ | A | B | C | means each hole axis must lie within a cylinder of at least ∅0.3 mm diameter (growing as hole size departs from MMC) at the true position defined by basic dimensions from datums A, B, C.
11. Concentricity (◎) — Legacy Symbol
Concentricity controls all median points of a diametrically opposed surface element pairs relative to a datum axis. The tolerance zone is a cylinder about the datum axis within which all derived median points must lie. This is extremely difficult and expensive to measure because it requires finding the median of opposed points — not simply measuring the surface. ASME Y14.5-2018 removed concentricity; position or runout is the recommended replacement in most applications.
12. Symmetry (≡) — Legacy Symbol
Similar to concentricity but for planar features: controls all median points of a feature relative to a datum plane. The tolerance zone is a space between two parallel planes equally disposed about the datum plane. Also removed from ASME Y14.5-2018 due to measurement difficulty; position is the recommended alternative.
Runout Tolerances (Datum Axis Required)
Runout tolerances control surfaces that revolve about an axis. They always require a datum axis, typically an important bearing surface.
13. Circular Runout (↗)
Circular runout controls the variation of a surface in any single cross-section as the part is rotated 360° about the datum axis. The tolerance value is the total indicator reading (TIR) at each cross-section. The gauge is not moved along the axis during measurement — each position is measured separately. Circular runout simultaneously controls circularity and coaxiality at each cross-section.
Example: | ↗ | 0.05 | A-B | means at any single cross-section, when the part is rotated 360° about the axis established by datum features A and B, the total indicator movement must not exceed 0.05 mm.
14. Total Runout (⇗)
Total runout is the most comprehensive surface control for rotating parts. The indicator traverses the entire surface (both rotational and axial movement) while the part rotates 360° about the datum axis. The total indicator reading across the entire surface must be within the tolerance value. Total runout simultaneously controls cylindricity, straightness, circularity, taper, and coaxiality of the entire surface — a single total runout callout replaces many individual controls.
Example: | ⇗ | 0.03 | A | on a shaft journal means over the entire journal surface, total indicator movement during full rotation about datum axis A must not exceed 0.03 mm.
GD&T Symbol Quick Reference
| Category | Symbol Name | Symbol | Datum Required | Modifier Allowed |
|---|---|---|---|---|
| Form | Straightness | — | No | Yes (on FOS) |
| Form | Flatness | ◻ | No | No |
| Form | Circularity | ○ | No | No |
| Form | Cylindricity | ⌭ | No | No |
| Profile | Profile of a Line | ⌒ | Optional | No |
| Profile | Profile of a Surface | ⌓ | Optional | No |
| Orientation | Angularity | ∠ | Yes | Yes |
| Orientation | Perpendicularity | ⊥ | Yes | Yes |
| Orientation | Parallelism | ∥ | Yes | Yes |
| Location | True Position | ⊕ | Yes | Yes |
| Location | Concentricity | ◎ | Yes | No |
| Location | Symmetry | ≡ | Yes | No |
| Runout | Circular Runout | ↗ | Yes | No |
| Runout | Total Runout | ⇗ | Yes | No |
Choosing the Right Symbol
Selecting the appropriate GD&T symbol requires understanding what the functional requirement actually is. Ask: “What must this feature do in the assembly?” A sealing face needs flatness. A bearing bore needs cylindricity or circular runout. A bolt hole pattern needs true position with MMC modifier. A cam profile needs profile of a surface. Using the wrong symbol — for example, specifying concentricity when total runout would suffice — creates unnecessary inspection burden without functional benefit.
The trend in ASME Y14.5-2018 is away from concentricity and symmetry (expensive to verify) and toward position and profile (geometrically clear, measurable on CMM or with functional gauges). When reviewing older drawings that use concentricity or symmetry, consult with the design engineer about whether the functional requirement is better served by a more modern callout.
Conclusion
The 14 geometric tolerance symbols cover every type of geometric control a designer could need — from the shape of a single surface element to the location of a complex hole pattern. Mastering what each symbol means, what its tolerance zone geometry looks like, and when it requires a datum is the foundation of competent GD&T practice. The subsequent articles in this series explore each major symbol category in depth, including worked examples of bonus tolerance calculation, datum reference frame setup, and measurement strategies for production inspection.
コメント