GD&T — Geometric Dimensioning & Tolerancing
GD&T controls the form, orientation, location and runout of features with clear symbols and a datum system. For fixtures, the drawing datums should define the locating scheme.
Datum System
A datum is a theoretically exact reference established by contacting the datum feature with the datum simulator (the fixture locator).
- Primary datum (A): 3 contact points — a plane.
- Secondary datum (B): 2 contact points — an axis/line.
- Tertiary datum (C): 1 contact point — a point.
- Order matters: datum precedence A-B-C matches how the part is located.
Maximum Material Condition (MMC)
MMC (⬸) allows a bonus tolerance: as a hole grows from its MMC size, the positional tolerance increases by the same amount. This is a functional, cost-saving callout for holes and pins.
Common GD&T Symbols
| Symbol | Characteristic | Controls |
|---|---|---|
| Position | True position of a point, axis or plane | |
| Concentricity / coaxiality | Common axis of two features (location) | |
| Symmetry | Median points equally disposed about a datum | |
| Parallelism | Orientation parallel to a datum | |
| Perpendicularity | Orientation perpendicular to a datum | |
| Angularity | Orientation at a specified angle to a datum | |
| Flatness | Uniform plane of the surface (form) | |
| Straightness | Straight line of an axis or surface (form) | |
| Circularity (roundness) | Uniform circle of a cross-section (form) | |
| Cylindricity | Uniform cylinder of the surface (form) | |
| Circular runout | Variation of a circular element during rotation | |
| Total runout | Total surface variation during rotation | |
| Profile of a line | Cross-section profile in a plane | |
| Profile of a surface | Surface profile in three dimensions | |
| Datum feature | Reference feature (A, B, C…) | |
| Datum target | Specific point, line or area on a datum | |
| Maximum material condition | Bonus tolerance at largest material size | |
| Least material condition | Bonus tolerance at smallest material size | |
| Regardless of feature size | No bonus tolerance |
ISO 1101 — Recommended Position Tolerance Values
For locating holes, dowel holes and pins, position tolerance values in common design practice follow the feature size. The drawing's specified tolerance always overrides these typical starting points.
| Nominal size (mm) | Fine | Medium | Coarse |
|---|---|---|---|
| ≤ 3 | 0.05 | 0.08 | 0.12 |
| > 3–6 | 0.05 | 0.10 | 0.16 |
| > 6–10 | 0.06 | 0.12 | 0.20 |
| > 10–18 | 0.08 | 0.16 | 0.25 |
| > 18–30 | 0.10 | 0.20 | 0.32 |
| > 30–50 | 0.12 | 0.25 | 0.40 |
| > 50–80 | 0.16 | 0.30 | 0.50 |
| > 80–120 | 0.20 | 0.40 | 0.60 |
| > 120–180 | 0.25 | 0.50 | 0.80 |
| > 180–250 | 0.30 | 0.60 | 1.00 |
ISO 2768-1 — General Tolerances (Untoleranced Dimensions)
When no tolerance is written next to a dimension, ISO 2768-1 applies. It covers linear and angular dimensions in tolerance classes f, m, c and v.
Linear dimensions — permissible deviations (± mm)
| Nominal size (mm) | Fine (f) | Medium (m) | Coarse (c) | Very coarse (v) |
|---|---|---|---|---|
| 0.5–3 | ±0.05 | ±0.1 | ±0.2 | — |
| > 3–6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| > 6–30 | ±0.1 | ±0.2 | ±0.5 | ±1.0 |
| > 30–120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| > 120–400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| > 400–1000 | ±0.3 | ±0.8 | ±2.0 | ±4.0 |
| > 1000–2000 | ±0.5 | ±1.2 | ±3.0 | ±6.0 |
Angular dimensions — permissible deviations
| Nominal length of the shorter side (mm) | f / m | c / v |
|---|---|---|
| ≤ 10 | ±1° | ±1°30′ |
| > 10–50 | ±0°30′ | ±1° |
| > 50–120 | ±0°20′ | ±0°30′ |
| > 120–400 | ±0°10′ | ±0°15′ |
| > 400 | ±0°5′ | ±0°10′ |
ISO 2768-2 — General Geometrical Tolerances
ISO 2768-2 sets default geometrical tolerances (form, orientation, location and runout) for features without individual indication, in classes H, K and L.
| Characteristic | H | K | L |
|---|---|---|---|
| Straightness and flatness | 0.02 | 0.05 | 0.1 |
| Perpendicularity | 0.05 | 0.1 | 0.2 |
| Symmetry | 0.05 | 0.1 | 0.2 |
| Circular and total runout | 0.1 | 0.2 | 0.5 |
Applying the Numbers in Fixture Design
- Hold locator features to 1/3–1/5 of the part position tolerance so the fixture does not consume the drawing budget.
- Use ISO 2768-1 class f or m for precise fixture dimensions; reserve class c and v for non-functional faces.
- Where the ISO 2768-2 default runout (0.1 mm, class H) is too coarse, specify the fixture's own GD&T and its wear limits.
Using GD&T in Fixture Design
- Locate on the drawing datums — fixture datums must match A, B, C.
- Use the datum features (holes, planes) as locating surfaces, not arbitrary edges.
- Align fixture datum and inspection datum so results match the drawing.
- For two-hole location use round pin + diamond pin and MMC to maximize tolerance.
Quick Check
- Does the fixture datum reproduce the drawing datum precedence?
- Is locator contact on the exact datum feature?
- Are position tolerances evaluated with the correct material condition?