GD&T Symbols Chart: All 14 Symbols per ASME Y14.5
ASME Y14.5-2018 defines 14 geometric characteristic symbols across five categories: form, profile, orientation, location, and runout. This chart covers every symbol with its tolerance zone shape, datum requirement, typical CNC-achievable value, and inspection method.
Quick Answer
ASME Y14.5-2018 defines 14 geometric characteristic symbols organized into five categories: form (4), profile (2), orientation (3), location (3), and runout (2). Each symbol specifies a tolerance zone shape and may or may not require a datum reference. Form controls (flatness, straightness, circularity, cylindricity) never need datums. All orientation, location, and runout controls require at least one datum. Position is the most commonly used symbol; concentricity and symmetry are recommended against for new designs.
GD&T Symbol Categories
The 14 symbols in ASME Y14.5-2018 are not arbitrary. They map to a hierarchy of geometric control. Understanding the category tells you what the symbol controls and whether it needs a datum, before you even read the feature control frame.
For a full introduction to GD&T concepts including datum reference frames, feature control frame anatomy, and when to use GD&T vs ± dimensions, see the GD&T guide. For a worked example of position calculation with MMC bonus, see true position tolerance.
All 14 GD&T Symbols: ASME Y14.5-2018
Typical tolerance ranges are achievable under standard CNC machining conditions on aluminum and steel alloys. Tighter values may require secondary operations (grinding, honing) or specialized inspection. All values are per-feature ranges; actual achievability depends on feature size, aspect ratio, and material.
| Symbol | Name | Category | Tolerance Zone Shape | Datum? | Typical CNC Range | Inspection |
|---|---|---|---|---|---|---|
| ⏥ | Flatness | Form | Two parallel planes | No | 0.001″–0.005″ (0.025–0.13 mm) | Surface plate + indicator, CMM |
| ⏤ | Straightness | Form | Two parallel lines (surface) or cylinder (axis) | No | 0.001″–0.005″ (0.025–0.13 mm) | V-block + indicator, CMM |
| ◯ | Circularity (Roundness) | Form | Two concentric circles (annular ring) | No | 0.001″–0.003″ (0.025–0.08 mm) | V-block + indicator, roundness tester |
| ⌭ | Cylindricity | Form | Two concentric cylinders | No | 0.001″–0.003″ (0.025–0.08 mm) | CMM (multi-section scan), roundness tester with Z-axis |
| ⌒ | Profile of a Line | Profile | Two offset curves (bilateral, unilateral, or unequally disposed) | Optional (with datum = form + orientation + location) | 0.002″–0.010″ (0.05–0.25 mm) | CMM, optical comparator |
| ⌓ | Profile of a Surface | Profile | Two offset surfaces (bilateral, unilateral, or unequally disposed) | Optional (with datum = form + orientation + location) | 0.002″–0.010″ (0.05–0.25 mm) | CMM (3D surface scan), structured light scanner |
| // | Parallelism | Orientation | Two parallel planes (or cylinder for axis) | Yes | 0.001″–0.005″ (0.025–0.13 mm) | Surface plate + indicator, CMM |
| ⟂ | Perpendicularity | Orientation | Two parallel planes (or cylinder for axis) | Yes | 0.001″–0.005″ (0.025–0.13 mm) | Square + indicator, CMM |
| ∠ | Angularity | Orientation | Two parallel planes at the specified angle to datum | Yes | 0.001″–0.005″ (0.025–0.13 mm) | Sine bar + indicator, CMM |
| ⌖ | Position | Location | Cylinder (for holes/pins), two parallel planes (for slots/tabs) | Yes | 0.005″–0.014″ (0.13–0.36 mm) | CMM, functional gage (at MMC) |
| ◎ | Concentricity | Location | Cylinder centered on datum axis | Yes | 0.002″–0.005″ (0.05–0.13 mm) | CMM (median-point algorithm) |
| ⌯ | Symmetry | Location | Two parallel planes centered on datum center plane | Yes | 0.002″–0.005″ (0.05–0.13 mm) | CMM (median-point algorithm) |
| ↗ | Circular Runout | Runout | Two concentric circles at each cross-section | Yes (axis) | 0.001″–0.005″ (0.025–0.13 mm) | V-block + dial indicator (single rotation) |
| ⌰ | Total Runout | Runout | Two concentric cylinders (entire surface simultaneously) | Yes (axis) | 0.002″–0.008″ (0.05–0.20 mm) | V-block + dial indicator (traverse full length) |
Form: Flatness, Straightness, Circularity, Cylindricity
Form tolerances control the shape of a single feature without referencing any datum. They answer: “Is this surface flat enough? Is this bore round enough?” Because no datum is involved, form controls describe the feature in isolation, so the surface can be tilted or displaced, and the form tolerance only constrains its shape. Per ASME Y14.5 Rule #1, the form of a feature of size is already bounded by its size tolerance; a separate form callout is only needed when the form requirement is tighter than what the size tolerance controls.
Flatness
Entire surface must lie between two parallel planes separated by the tolerance value.
Straightness
Each line element on a surface, or the derived median line / axis, must lie within the specified zone.
Circularity (Roundness)
Each cross-section of a cylindrical or spherical feature must lie between two concentric circles separated by the tolerance.
Cylindricity
Combined control of roundness, straightness, and taper over the full length of a cylinder. The surface must lie between two coaxial cylinders.
Profile: Line and Surface
Profile controls are the most versatile GD&T tools. Profile of a surface can replace separate flatness, parallelism, perpendicularity, and position callouts with a single feature control frame. When used with datums, it simultaneously controls form, orientation, and location. Modern practice increasingly favors profile for complex surfaces and 5-axis CNC freeform features. The tolerance zone can be bilateral (equally disposed about the true profile), unilateral (entirely inside or outside), or unequally disposed (per the “UZ” modifier in ASME Y14.5-2018).
Profile of a Line
Each cross-sectional line element must lie within the profile tolerance band around the true profile. Without datum, controls form only; with datum, also controls orientation and location.
Profile of a Surface
The entire surface must lie within the profile tolerance band. This is the most versatile GD&T control because it can replace multiple form, orientation, and location callouts in a single FCF.
Parts Machined to GD&T Spec
MakerStage machines to ASME Y14.5 with position tolerances as tight as ø0.002 in. (0.05 mm), flatness to 0.001 in. (0.025 mm), and full CMM verification on request. Upload your drawing with GD&T callouts and get engineer-reviewed pricing. After order confirmation, DFM can flag callouts that drive unnecessary cost and suggest tolerance-for-cost trade-offs before production starts.
Get a QuoteOrientation: Parallelism, Perpendicularity, Angularity
Orientation controls relate a feature to a datum. They describe the angular relationship without constraining the feature’s location. Parallelism constrains a surface to be parallel to a datum; perpendicularity constrains it to be 90° to a datum; angularity constrains it to a specified basic angle. All three inherently control the form of the toleranced feature: a parallelism tolerance of 0.003 in. (0.076 mm) means the surface must also be flat within 0.003 in. (0.076 mm). The tolerance zone is two parallel planes.
Parallelism
The controlled surface or axis must lie between two planes (or within a cylinder) that are parallel to the datum. Inherently controls flatness per ASME Y14.5 Rule #1.
Perpendicularity
The controlled surface or axis must lie between two planes (or within a cylinder) that are perpendicular to the datum.
Angularity
The controlled surface or axis must lie between two planes that are at the specified basic angle to the datum. The basic angle is stated separately; the tolerance controls only the variation around that angle.
Location: Position, Concentricity, Symmetry
Location controls define where a feature is relative to datums. Position is by far the most common because it uses a cylindrical zone for holes and pins, giving 57% more area than the equivalent ± square zone. Position supports MMC/LMC modifiers for bonus tolerance and functional gaging.
Concentricity and symmetry require measuring median points, which is expensive and unreliable. ASME Y14.5-2018 explicitly recommends using position or runout instead for new designs. Reserve concentricity for the rare case where median-point balance is critical (e.g., high-RPM rotating shafts where mass distribution matters).
Position
The axis or center plane of a feature must fall within the specified zone centered on the true (basic) position. The most commonly used GD&T control. Supports MMC/LMC modifiers for bonus tolerance.
Concentricity
The median points of all diametrically opposed elements must lie within a cylindrical zone centered on the datum axis. ASME Y14.5-2018 recommends position or runout for most applications; concentricity requires expensive median-point measurement.
Symmetry
The median points of all opposed elements must lie between two parallel planes equally disposed about the datum center plane. Like concentricity, ASME Y14.5-2018 recommends position as the preferred alternative.
Runout: Circular and Total
Runout controls apply to surfaces of revolution (shafts, bores, flanges) and always reference a datum axis. Circular runout checks one cross-section at a time during a full 360° rotation. Total runout checks the entire surface simultaneously as the indicator traverses the full length during rotation.
Total runout is the stricter control because it captures taper and axial straightness that circular runout misses. Inspection is simple: V-block and dial indicator on most features. For a deeper comparison of runout types and when to choose each, see the GD&T guide.
Circular Runout
At each individual cross-section, the surface must lie between two concentric circles (centered on the datum axis) separated by the tolerance. Controls circularity and coaxiality per cross-section, but not surface straightness along the axis.
Total Runout
The entire surface must lie between two coaxial cylinders centered on the datum axis. It controls circularity, straightness, coaxiality, and taper simultaneously, making it a more comprehensive check than circular runout.
How to Read a GD&T Symbol on a Drawing
Every GD&T symbol appears inside a feature control frame (FCF). Reading the FCF is a mechanical, left-to-right process. Once you identify the symbol from this chart, you know the type of control; the remaining compartments tell you the tolerance magnitude, material condition modifier, and datum references.
Identify the symbol
The first compartment of the FCF contains the geometric characteristic symbol. Use this chart to identify what it controls (form, profile, orientation, location, or runout) and whether it requires datums.
Read the tolerance value
The second compartment states the tolerance magnitude. A ⌀ prefix means a cylindrical (diametral) zone. No prefix means a width (two parallel planes). The unit matches the drawing’s unit system.
Check for material condition modifiers
Look for Ⓜ (MMC) or Ⓛ (LMC) after the tolerance value. If present, bonus tolerance applies as the feature departs from the specified material condition. No modifier means RFS (Regardless of Feature Size) — the default in ASME Y14.5-2018.
Read the datum references
The remaining compartments list datum letters (A, B, C) in order of precedence. Primary datum constrains 3 degrees of freedom, secondary adds 2, tertiary adds 1. If no datums are listed, the control is a form control and applies to the feature in isolation.
Reading template
Read any FCF aloud: “The [symbol name] of this feature shall be within [tolerance value] [zone shape] [at material condition], referenced to datum [A], [B], [C].” For a detailed walkthrough with 5 annotated examples and compartment-by-compartment reading help, see the feature control frame guide. For broader context on datums, basic dimensions, and how the symbols fit together, see our GD&T guide.
GD&T Symbols FAQ
Related Resources
Need Parts Machined to GD&T Specs?
Upload your drawings with GD&T callouts. We machine to ASME Y14.5 with position tolerances as tight as ø0.002 in. (0.05 mm) and provide CMM inspection reports on request. Free DFM starts after order confirmation.
Get Free Quote Fast