GD&T Symbol Reference Chart
All 14 geometric tolerance symbols, modifiers, and datum frames — ASME Y14.5 shop reference
Geometric Dimensioning and Tolerancing (GD&T) replaces vague plus/minus callouts with a precise language for form, orientation, location, and runout. This chart lists every standard feature-control symbol, what each tolerance zone looks like, and how modifiers and datums change what the print actually requires.
Why GD&T Exists (vs Plus/Minus Tolerancing)
Plus/minus dimensioning controls size. It does not clearly say whether a hole can be off-center, whether a face must be flat, or whether a shaft must run true to a bearing journal. Shops historically “interpreted” those gaps with tribal knowledge — and then argued with QC when parts that measured inside every ± band still would not assemble.
GD&T (ASME Y14.5) fixes that by defining a tolerance zone: a geometric envelope the feature must stay inside. A position tolerance of 0.010 in at MMC on a hole pattern does not mean “±0.005 on X and Y.” It means the axis of each hole must lie inside a cylindrical zone of diameter 0.010 in (larger when the hole is made bigger than MMC). That single rule simultaneously controls location, allows bonus material when size helps, and ties the requirement to a datum reference frame so everyone measures from the same origin.
You need GD&T on a print when parts mate across multiple features, when orientation or form matters as much as size, when interchangeability must survive vendor-to-vendor variation, or when CMM inspection needs an unambiguous acceptance rule. Job-shop fab of simple brackets with generous clearances can often live on ±. Precision fixtures, bearing bores, seal faces, pin patterns, and anything that must assemble without selective fit usually cannot.
Common shop misreads: treating a position frame like independent ± on X and Y; ignoring the material condition modifier (MMC vs RFS changes bonus and inspection method); measuring from a convenient edge instead of the stated datums; confusing circularity with cylindricity; and reading circular runout as if it controlled the entire surface the way total runout does. When a feature control frame appears on a print, read it left to right — symbol, tolerance value, material condition, then primary/secondary/tertiary datums — before you set up the part.
All 14 GD&T Symbols
Feature control frames use these geometric characteristic symbols. Zone type describes the shape of the allowable variation; typical use is where you actually see the callout on fab and machining prints.
| Symbol | Name | Tolerance Zone Type | Typical Use Case |
|---|---|---|---|
| ⎯ | Straightness | 2D line / cylindrical zone for axis | Shaft axis bow, edge straightness, long bar stock |
| ▱ | Flatness | Two parallel planes | Gasket faces, mounting pads, ground plates |
| ○ | Circularity (Roundness) | Two concentric circles (cross-section) | O-ring grooves, bearing OD at a section |
| ⌭ | Cylindricity | Two coaxial cylinders | Pistons, hydraulic rods, precision shafts full length |
| ⌒ | Profile of a Line | 2D uniform boundary along a curve | Cam profiles, 2D contour checks on a plane |
| ⌓ | Profile of a Surface | 3D uniform boundary around a surface | Complex freeform surfaces, molded / machined contours |
| ∠ | Angularity | Two parallel planes at a basic angle | Chamfers, wedges, angled faces vs a datum |
| ⊥ | Perpendicularity | Two parallel planes / cylinder at 90° | Shoulders square to axes, flange faces to bores |
| ∥ | Parallelism | Two parallel planes / cylinder | Opposite faces, slot sides, parallel shafts |
| ⌖ | Position | Sphere / cylinder / boundary for location | Hole patterns, pin locations, fastener groups |
| ◎ | Concentricity | Cylindrical zone for median points | Legacy coaxial control (often replaced by position/runout) |
| ⌯ | Symmetry | Two parallel planes about a center plane | Legacy center-plane control (often replaced by position) |
| ⌰ | Circular Runout | Circular elements vs datum axis | Bearing journals, sealing diameters, single cross-sections |
| ⌱ | Total Runout | Entire surface vs datum axis | Full face and OD control on rotating parts |
Form controls (straightness, flatness, circularity, cylindricity) do not reference datums. Orientation (angularity, perpendicularity, parallelism), location (position, concentricity, symmetry), and runout always relate to one or more datums. Profile can be used with or without datums depending on whether the surface is located in space or only shaped.
Material Condition Modifiers — MMC, LMC, RFS / RFT
When a geometric tolerance applies to a feature of size (hole, pin, slot width), a material condition modifier tells you whether the stated tolerance is fixed or can grow as size departs from the worst-case material limit.
| Modifier | Symbol | What It Changes |
|---|---|---|
| MMC (Maximum Material Condition) | Ⓜ | Tolerance applies at the size with the most material (smallest hole / largest pin). As the feature departs from MMC toward LMC, bonus tolerance is added. Favors assembly of mating features and functional gauges. |
| LMC (Least Material Condition) | Ⓛ | Tolerance applies at the size with the least material (largest hole / smallest pin). Bonus accrues as the feature moves toward MMC. Used when wall thickness, minimum distance, or breakout risk matters more than easy assembly. |
| RFS (Regardless of Feature Size) | No symbol (default) | Geometric tolerance stays fixed no matter the actual size. No bonus. Common on position when location must be held at every size, and on most orientation/form callouts that are not tied to virtual condition gauges. |
| RFT (Regardless of Feature Size — projected / related) | Context / notes | Shop shorthand for “no size-dependent bonus” on related requirements. Modern ASME drawings leave RFS implied (no Ⓢ). If you still see a circled S on older prints, treat it as RFS — fixed geometric tolerance, no MMC/LMC bonus. |
Rule of thumb: MMC on a hole pattern usually means “will it assemble with a gauge pin at MMC?” RFS means “is the axis inside the zone at the size we actually made?” Do not apply MMC bonus in a linear ± stack calculator — compute size first, then add bonus per the print. Pair this chart with the Tolerance Stack-Up Calculator and Tolerance Stack-Up Guide for the linear envelope, then fold GD&T bonus by hand.
Datum Reference Frame — Primary, Secondary, Tertiary (3-2-1)
Datums are the mutually perpendicular planes, axes, or points that lock the part in space for measurement. The feature control frame lists them in order after the tolerance: primary, secondary, tertiary.
Primary datum
Contacts the fixture or CMM first and constrains the most degrees of freedom — typically three points on a plane (stops rock). All subsequent measurements relate back through this surface or axis.
Secondary datum
Usually two points against an edge or cylinder. Removes the next freedoms (slide / rotation) while remaining consistent with the primary contact.
Tertiary datum
Typically one point. Kills the last remaining translation so the part cannot slide along the secondary stop. That is the classic 3-2-1 fixture principle.
If the print says |⌖|0.2Ⓜ|A|B|C|, you must establish A, then B, then C before evaluating position. Measuring from a shop-convenient edge that is not on the datum list is a nonconformance waiting to happen — the part can “pass” on the bench and fail on a CMM that follows the frame. Datum targets (partial areas) appear when the full surface is not reliable; still respect the order in the frame.
How to Read a Feature Control Frame
- Left cell = geometric symbol (what kind of control)
- Next = tolerance value (and diameter symbol ⌀ if the zone is cylindrical)
- Optional = material condition modifier (Ⓜ / Ⓛ) or projected tolerance zone
- Then = datum references in order (A, then B, then C…)
- Basic dimensions (boxed) locate the tolerance zone — they are theoretically exact, not ±
Example: a hole with |⌖|⌀0.010Ⓜ|A|B|C| and basic 2.000 / 3.000 dimensions means the hole axis must lie in a ⌀0.010 cylinder at MMC relative to datums A-B-C. Open the hole larger than MMC and the allowable position zone grows by the amount of size departure (bonus). That is not the same as ±0.005 on each coordinate.
Recommended Metrology Tools for GD&T Checks
Calipers, radius gauges, and layout tools for verifying size before you interpret geometric frames
Starrett Electronic Slide Caliper 0–6 in
- Confirm feature-of-size before MMC bonus
- 0.0005 in resolution for setup checks
- Carbide-tipped jaws hold calibration
- Large LCD for shop floor use
- First step before CMM or indicator work
SS Radius Gauge Set
- Check fillet and edge profile quickly
- Catch form issues before full inspection
- Useful with profile callouts
- Compact set for the toolbox
- Pairs with caliper size checks
Neiko Transfer Punch Set
- Transfer hole patterns from mating parts
- Verify position intent before drilling
- Reduces walk on layout starts
- 28-piece shop coverage
- Handy when prints show basic hole grids
Tap Magic Cutting Fluid
- Cleaner finishing cuts on steel
- Helps hold size for tight MMC holes
- Less BUE on finishing passes
- Shop staple next to the mill
- Supports surface and form callouts
Permatex Anti-Seize Lubricant
- Protects precision mating surfaces
- Press fits separate cleanly
- Stainless and aluminum assemblies
- Useful after tight position patterns
- Prevents galling on inspected parts
As an Amazon Associate, TestTalkHQ earns from qualifying purchases.
GD&T and Surface Finish
Geometric tolerances control form and relationship; surface texture (Ra, Rz) controls how rough the surface is. A flatness callout of 0.002 in does not replace a 32 μin Ra requirement on a seal face — you can be flat and still too rough to seal. Read both. Use the Surface Finish Ra Calculator, Surface Finish Guide, and How to Read a Surface Finish Callout when the print stacks a finish symbol next to a feature control frame.
Common Print Misreads
Position ≠ ± on coordinates. Diameter symbol in the tolerance cell means a cylindrical (or circular) zone, not a square ± box unless the print explicitly uses a non-diameter boundary.
Circularity ≠ cylindricity. Circularity is checked one cross-section at a time. Cylindricity controls the entire cylindrical surface in one zone — stricter and more expensive to inspect.
Circular runout ≠ total runout. Circular runout lets you walk an indicator around one circle. Total runout requires the indicator to sweep the whole length or face — taper and camber count.
Concentricity / symmetry are rare on new drawings. Many modern prints use position or runout instead because they are easier to inspect and usually control the functional requirement better. If you still see concentricity, budget CMM median-point analysis — not a simple dial-indicator “runout” check.
Related Calculators & Guides
Use this chart as the symbol decoder, then run the numbers on the mating stack and finish requirements:
- Tolerance Stack-Up Calculator — worst-case and RSS linear stacks (apply MMC/LMC bonus from this chart separately)
- Tolerance Stack-Up Guide — when worst-case vs RSS fits the job
- Surface Finish Ra Calculator — theoretical Ra from nose radius and feed
- Surface Finish Guide — Ra, Rz, and how to hit the spec
- How to Read a Surface Finish Callout — decode the finish symbol on the print
- Machining & Fabrication Hub — speeds, bends, tolerances, and shop tools