GD&T Symbols Explained
Geometric Dimensioning and Tolerancing (GD&T) is the language that controls how features relate to each other, not just how big they are. A simple dimension says "this hole is ⌀10 ±0.05". GD&T says "this hole must be within ⌀0.05 of the exact theoretical location, relative to datums A and B." That difference is what makes parts actually fit and function.
The Feature Control Frame
Every GD&T callout appears as a rectangular box divided into cells. Reading left to right:
| Cell | Meaning |
|---|---|
| Symbol | Which geometric characteristic (position, flatness, etc.) |
| ⌀ (optional) | Tolerance zone is cylindrical (for position of holes). Without it, zone is two parallel planes. |
| Tolerance value | Size of the tolerance zone. If preceded by ⌀, it's the diameter of a cylindrical zone. |
| Ⓜ / Ⓛ / Ⓡ | MMC, LMC, or RFS modifier (explained in next article) |
| Datums (A|B|C) | The datum reference frame — order matters |
The 14 GD&T Symbols — Grouped by Type
Form Controls (no datums needed)
Form controls describe the shape of a single feature independently. They don't reference datums because they say "this surface itself must be flat/straight/round" regardless of where it sits.
| Symbol | Name | Controls | Typical use |
|---|---|---|---|
— | Straightness | Line element — must lie within a tolerance zone | Straightness of a shaft, no bow |
▱ | Flatness | Surface — all points within two parallel planes | Mating surfaces, fixture surfaces |
○ | Circularity (roundness) | Each cross-section must be within two concentric circles | Shaft diameters, bore circularity |
⌭ | Cylindricity | Entire surface — combined roundness + straightness + taper | Precision bearing journals, hydraulic bores |
Flatness vs parallelism: flatness says the surface itself is flat (no datum). Parallelism says the surface is parallel to datum A (a relationship). A surface can be flat but tilted — parallelism catches that, flatness doesn't.
Orientation Controls (need datums)
Orientation controls describe the angle between a feature and a datum.
| Symbol | Name | Controls | Typical use |
|---|---|---|---|
// | Parallelism | Surface/axis parallel to datum plane/axis | Parallel faces, slot walls |
⟂ | Perpendicularity | Surface/axis at 90° to datum | Square shoulders, hole axes vs face |
∠ | Angularity | Surface/axis at a specified angle to datum | Wedges, chamfers, angled faces |
Location Controls
| Symbol | Name | Controls | Typical use |
|---|---|---|---|
◉ | Position | Location of features (holes, pins) from datums | Bolt hole patterns — the most common GD&T callout |
◎ | Concentricity | Axes of features around a datum axis | Rotating parts — spindles, bearing journals |
⫛ | Symmetry | Feature centered about a datum centerplane | Slots symmetric about a centerline |
Position is the workhorse. On most machined parts, 80% of GD&T callouts are position. It controls hole location in a cylindrical tolerance zone. Instead of checking X=25±0.05 and Y=15±0.05 separately, position says the hole center must lie within a ⌀0.1 cylinder at the true position. This is more functional and allows bonus tolerance (explained next article).
Profile Controls
| Symbol | Name | Controls | Typical use |
|---|---|---|---|
⌒ | Profile of a line | 2D cross-section shape along one line | Cam profiles, contoured edges |
⌒ (filled) | Profile of a surface | 3D surface shape over the entire feature | Complex cast/machined surfaces, molds |
Profile is the most flexible control — it can simultaneously control size, form, orientation, and location. It's widely used on castings and contoured parts where no single dimension captures the shape.
Runout Controls
| Symbol | Name | Controls | Typical use |
|---|---|---|---|
↗ | Circular runout | Each individual cross-section during rotation | Shafts, bearing surfaces — catches lobing, eccentricity per revolution |
| Total runout | Entire surface during rotation (cumulative) | Entire shaft surface — catches taper, ovality, and cumulative error |
Runout in practice: to check runout, mount the part between centers or in a fixture on a rotary axis, place a dial indicator on the surface, and rotate. The total indicator variation is the runout. Circular runout checks one cross-section at a time; total runout sweeps the indicator along the whole surface.
Practical Example: A Bolt Hole Pattern
Consider a flange with 4 holes on a 50 mm bolt circle. The drawing shows:
Without GD&T:
Hole positions dimensioned as X=25±0.1, Y=25±0.1 for each hole. This creates square tolerance zones that accumulate — a hole could be at the corner of the square and still "pass", but the mating bolt wouldn't fit.
With GD&T position:
◉ ⌀0.15 Ⓜ A B C
Each hole's center must lie within a ⌀0.15 cylindrical tolerance zone at the true (basic) position. This is functionally correct — if a bolt fits the tolerance zone, it will assemble. Plus, with MMC, you get bonus tolerance when the hole is larger than its minimum size.
Which Control to Use — Quick Reference
| If you need to control... | Use |
|---|---|
| A flat surface is flat (no reference) | Flatness |
| A surface is flat AND parallel to another | Parallelism |
| A surface is square to another | Perpendicularity |
| Hole location relative to datums | Position |
| A shaft doesn't wobble when turned | Circular runout |
| A whole turned surface is straight and round | Total runout / cylindricity |
| A complex curved surface shape | Profile of a surface |
| A hole axis is perpendicular to a face | Perpendicularity (of axis) or position |
Next: learn how MMC, LMC, and bonus tolerance give you extra tolerance when the feature deviates from maximum material condition — MMC / LMC / Bonus Tolerance.