Geometric Dimensioning
& Tolerancing
A comprehensive visual reference for GD&T based on ASME Y14.5 — covering symbols, modifiers, bonus tolerance, datum systems, feature control frames, and fundamental rules.
Feature Control Frame
The feature control frame (FCF) is the primary vehicle for communicating GD&T requirements on engineering drawings. Every FCF is read left to right.
Composite FCF vs. Multi-Single-Segment
One symbol spans both rows. Lower segment controls pattern spacing only.
Two separate FCFs. Each is fully independent with its own datum references.
GD&T Characteristic Symbols
14 geometric controls organized into 5 categories. Each symbol defines a specific tolerance zone that the feature must lie within.
Controls how round a cross-section of a feature is. The tolerance zone is two concentric circles — the surface must lie between them. No datum required.
Controls roundness, straightness, and taper of a cylinder simultaneously. Tolerance zone = two coaxial cylinders. Most stringent form control. No datum required.
Controls how straight a line element or axis is. Applied to a surface: two parallel lines. Applied to an axis (⌀ prefix): cylindrical zone. Can override Rule #1. No datum.
Controls how flat a surface is. Tolerance zone = two parallel planes. Often specified on sealing surfaces, mating faces, and gasket seats. No datum required.
Controls orientation of a feature at any angle other than 0° or 90°. Tolerance zone is two parallel planes at the specified basic angle to the datum. Datum required.
Controls orientation 90° to a datum. Applied to a surface: two parallel planes. Applied to an axis: cylindrical zone. Controls squareness. Datum required.
Controls orientation of a surface or axis parallel to a datum. Common for mating surfaces. Can be applied to planes, lines, or axes. Datum required.
Most commonly used GD&T control. Defines how far a feature's axis/center plane can deviate from its theoretically exact (basic) location. Enables bonus tolerance with MMC. Datum required.
Controls the median points of a feature to a datum axis. Tolerances the axis, not the surface. Extremely difficult to measure — replaced by runout or position in modern practice. Datum required.
Controls median points of a feature symmetric to a datum plane. Similar inspection difficulty as concentricity. Often replaced by position control. Removed in ASME Y14.5-2018. Datum required.
Controls surface variation measured at each cross-section as the part rotates 360° around the datum axis. A single-revolution measurement. Used on shafts, bearing seats. Datum required.
Controls all surface points simultaneously as part rotates and indicator traverses the full surface. Controls cylindricity + coaxiality together. More stringent than circular runout. Datum required.
Controls the shape of a cross-sectional profile. Tolerance zone is 2D — two curves offset from the true profile. Can be unequally disposed using U modifier. Datum may or may not be required.
3D control — most versatile GD&T symbol. Can simultaneously control form, orientation, and location of any surface. Universal control for complex shapes, stampings, castings. Datum may or may not be required.
Tolerance Zone Shapes
The shape of the tolerance zone depends on the symbol and whether a ⌀ prefix is used.
Modifiers
Modifiers refine how a tolerance applies. Material condition modifiers enable bonus tolerance and open up additional geometric relationships.
| Symbol | Name | Applies To | Effect / Description |
|---|---|---|---|
| Ⓜ | Maximum Material Condition (MMC) | Features of size only (holes, pins, slots, tabs) | Tolerance applies at MMC size. As feature departs from MMC toward LMC, additional (bonus) tolerance is earned. Most common modifier. Used for assembly fit. |
| Ⓛ | Least Material Condition (LMC) | Features of size | Tolerance applies at LMC. Bonus earned as feature departs toward MMC. Used where wall thickness or structural strength is critical (e.g., minimum material for casting bosses). |
| Ⓢ | Regardless of Feature Size (RFS) | Features of size | Default per ASME Y14.5-2018 (implied, rarely written). Tolerance applies regardless of actual size — no bonus tolerance earned. Used for functional requirements. |
| Ⓟ | Projected Tolerance Zone | Position of threaded holes, press fits | Extends the tolerance zone beyond the part surface to control the mating feature's alignment (e.g., stud projecting from a tapped hole). Eliminates interference from angular error. |
| Ⓕ | Free State (Non-rigid) | Non-rigid parts (gaskets, sheet metal, plastics) | Measurement taken in free state (unrestrained). Without modifier, non-rigid parts are measured in restrained/simulated assembly condition per drawing note. |
| ST | Statistical Tolerance | Any tolerance | Tolerance must be maintained using statistical process control (SPC). Allows wider individual tolerances while maintaining assembly-level requirements. Requires SPC plan. |
| CF | Continuous Feature | Profile, surfaces | Treat interrupted or offset surfaces as a single continuous feature. Both surfaces must lie within the same profile tolerance zone simultaneously. |
| U⌃ | Unequal Bilateral (Unequally Disposed) | Profile of a Line, Profile of a Surface | Distributes profile tolerance unequally: inside vs outside. Example: ⌓ 0.6 U 0.4 — 0.4 toward material, 0.2 away from material (total = 0.6). |
MMC vs LMC — Size Concept
Bonus Tolerance
When a material condition modifier (Ⓜ or Ⓛ) is applied, the geometric tolerance can increase as the feature departs from the specified condition — this additional allowance is called bonus tolerance.
Datums & the Datum Reference Frame
A datum is a theoretically exact point, axis, line, or plane from which measurements are made. The Datum Reference Frame (DRF) is the 3-2-1 constraint system that fully immobilizes a part in 3D space.
The 3-2-1 Rule — Degrees of Freedom
Datum Feature Types
| Datum Feature Type | Geometry | Degrees of Freedom Constrained | Common Application |
|---|---|---|---|
| Planar Datum | Flat surface | 1 translation + 2 rotations (3 DOF) | Bottom face, machined flange face |
| Cylindrical Datum | Hole or shaft | 2 translations (axis) — 4 DOF if primary | Bore, shaft OD, pilot feature |
| Width Datum | Slot or tab | 1 translation (center plane) | Keyed slots, symmetrical bosses |
| Point Datum | Sphere, apex | 3 translations | Precision spherical features |
| Line Datum | Axis from intersection of planes | 2 rotations | Compound datum features |
Fundamental Rules
ASME Y14.5 defines two fundamental rules that govern GD&T interpretation. These are not optional — they apply to all drawings unless explicitly overridden.
A pin of ⌀10.00±0.10 must fit through a perfect ⌀10.10 ring gauge, and each cross-section must be ≥⌀9.90.
This means no bonus tolerance is earned unless Ⓜ or Ⓛ is explicitly written.
Basic dimensions never appear without an FCF. The FCF contains all the tolerance for that feature.
A straight leader arrow pointing to a surface means the control applies to the entire surface, not a portion of it.
Virtual Condition & Resultant Condition
Two critical boundary concepts used in mating-part analysis and gauge design.
| Condition | External Feature (Pin) | Internal Feature (Hole) | Use |
|---|---|---|---|
| Virtual Condition (VC) | MMC + Geometric Tol = outer boundaryVC = ⌀10.10 + 0.25 = ⌀10.35 |
MMC − Geometric Tol = inner boundaryVC = ⌀9.90 − 0.25 = ⌀9.65 |
Gauge design (GO gauge), worst-case fit check |
| Resultant Condition (RC) | LMC − Geometric Tol = inner boundaryRC = ⌀9.90 − 0.45 = ⌀9.45 |
LMC + Geometric Tol = outer boundaryRC = ⌀10.10 + 0.45 = ⌀10.55 |
Edge distance, wall thickness, structural check |
Common Inspection Methods
Quick Reference — Datum Requirements
| Control Type | Symbol | Datum Required? | Bonus Tol (Ⓜ)? | Notes |
|---|---|---|---|---|
| Flatness | ⏥ | No | No | Self-referencing form control |
| Straightness | — | No | No* | *On axis (⌀): can override Rule #1 |
| Circularity | ○ | No | No | Per cross-section only |
| Cylindricity | ⌭ | No | No | Most stringent form control |
| Profile of a Surface | ⌓ | Optional | No | No datum = form only |
| Profile of a Line | ⌒ | Optional | No | 2D cross-section control |
| Angularity | ∠ | Yes | No | Orientation only, no location |
| Perpendicularity | ⊥ | Yes | No | 90° orientation control |
| Parallelism | ∥ | Yes | No | 0° orientation control |
| True Position | ⌖ | Yes | Yes (Ⓜ or Ⓛ) | Most versatile location control |
| Concentricity | ◎ | Yes | No (axis only) | Hard to measure; prefer position |
| Symmetry | ⊙ | Yes | No | Removed in Y14.5-2018 |
| Circular Runout | ↗ | Yes | No | Per cross-section |
| Total Runout | ⇗ | Yes | No | Full surface simultaneously |
Bonus Tolerance Calculator
Enter feature size limits and the stated position tolerance. Switch between MMC and LMC modes. The table auto-generates bonus tolerance for every step within the size range.
Virtual & Resultant Boundary Calculator
Calculates all four critical boundaries for mating part analysis, gauge design, and worst-case fit checks. Works for both internal (holes) and external (pins/bosses) features under MMC or LMC.
Feature Parameters
Calculate to see boundaries