GD&T Symbols Explained: The Complete Reference Guide to Form, Orientation, Position & Runout Tolerances

Geometric Dimensioning and Tolerancing — GD&T — is the engineering language used to specify allowable variation in the size, form, orientation, location and runout of features on a part. It replaces traditional ±(plus-or-minus) coordinate dimensioning in any application where functional fit, assembly stack-up or measurement repeatability matters. Done right, GD&T tells the manufacturer exactly what's required, gives the inspector unambiguous criteria, and produces interchangeable parts that fit together every time.

Done wrong — or worse, ignored — and you get parts that measure within tolerance but won't assemble; designers blaming machinists; machinists blaming inspectors; and assembly lines stopped while engineers argue about what the drawing actually means. GD&T exists to remove that ambiguity. This guide is the complete Australian reference: every one of the 14 symbols decoded; ASME Y14.5, ISO 1101 and AS/NZS 1100 standards reconciled; datum reference frames explained; material condition modifiers (MMC, LMC, RFS) and bonus tolerance worked through; feature control frames parsed step by step; and the common mistakes that cause real-world drawing disputes.

This is a reference guide, not a quick read. Bookmark it. Use the table of contents in your browser, or jump to the symbol-by-symbol section that matches the drawing in front of you.

What is GD&T?

GD&T is a system of symbols, rules and conventions for specifying the geometry of manufactured parts. It complements (and in functional applications largely replaces) traditional plus-or-minus tolerance dimensioning. Where ±0.1 says "the dimension can vary by 0.1 millimetres in either direction", GD&T says specifically what the form, orientation, location or runout of a feature must be — and relative to what reference (the datum).

The case for GD&T over ±tolerancing is functional. A hole drilled at the correct centre coordinates but tilted out of perpendicular to the surface won't accept a press-fit pin. A flat machined to the right thickness but wavy across its length won't seat against a mating part. Coordinate tolerancing alone can't catch these defects; geometric tolerancing can, and tells the manufacturer in advance which deviations matter and which don't.

GD&T is also the language of inspection. A coordinate measuring machine (CMM) operator inspecting a part to a GD&T drawing has unambiguous criteria — measure feature X relative to datum reference frame ABC, compare to the tolerance zone defined in the feature control frame, pass or fail. Without GD&T, two inspectors can measure the same part to the same drawing and reach different conclusions.

GD&T applies wherever drawings drive manufacturing: aerospace, automotive, medical devices, defence, mining equipment, agricultural machinery, machine tools, instrumentation, and most precision manufacturing in Australia. It is the international engineering standard for dimensional control.

The standards: ASME Y14.5, ISO 1101 and AS/NZS 1100

Three standards cover GD&T globally, and Australian industry uses all three depending on sector and trading partner.

Standard	Origin	Latest revision	Used by AU industries
ASME Y14.5	USA (American Society of Mechanical Engineers)	2018 (replacing 2009 and 1994)	Aerospace, automotive (US-aligned), oil and gas, defence projects with US partners, machine tool industry
ISO 1101 (with related ISO GPS series)	International (ISO Geometrical Product Specifications)	2017 (with ISO 5459 datum, ISO 14405 size, ISO 8015 fundamental tolerances, others)	European-aligned manufacturing, medical device, automotive (EU/JP-aligned), pharmaceutical equipment
AS/NZS 1100 Part 201	Australia/New Zealand (Standards Australia)	1992 base, with subsequent amendments	The AU/NZ technical drawing standard. Mechanical engineering drawing — adopts ISO conventions for line types, projections, dimensioning, with provisions for both ISO 1101 and ASME-style geometric tolerancing

AS/NZS 1100 Part 201 is the Australian technical drawing standard. It governs how engineering drawings are presented in Australian and New Zealand industry — line types, projections, sectioning, dimensioning, tolerancing conventions, abbreviations and symbols. For geometric tolerancing specifically, AS/NZS 1100.201 is aligned with ISO 1101 conventions, but most AU drawings will reference either ASME Y14.5 or ISO 1101 directly in the drawing notes depending on the customer or industry sector.

The practical reality for an Australian engineer or machinist: you will see all three standards in use, often on different drawings on the same factory floor. A defence project might be ASME Y14.5; the medical device contract on the next bench might be ISO 1101; and the locally-designed mining equipment fab drawing might cite AS/NZS 1100.201. The drawing's title block or general notes will state which standard applies. Always check.

The good news: the 14 GD&T symbols are essentially identical across ASME Y14.5 and ISO 1101. The differences are in detail — terminology, default rules, modifier conventions — and we cover those throughout this guide.

The 14 GD&T symbols by category

GD&T uses 14 geometric characteristic symbols, grouped into five categories by what they control.

Category	Symbols	Datum required?	Controls
Form	Straightness, Flatness, Circularity (Roundness), Cylindricity	No	The shape of a feature taken in isolation. How straight, flat, round or cylindrical is it?
Orientation	Perpendicularity, Parallelism, Angularity	Yes	The angular relationship between a feature and a datum. How square, parallel or angled is it relative to the reference?
Location	Position, Concentricity (deprecated 2018), Symmetry (deprecated 2018)	Yes	Where the feature is located relative to a datum reference frame.
Profile	Profile of a Line, Profile of a Surface	Optional (with or without datum)	The form, orientation, location and size of an irregular feature in one combined control.
Runout	Circular Runout, Total Runout	Yes (datum axis)	How a rotational surface deviates as the part rotates about a datum axis. Composite — combines form, orientation, location.

Note on deprecation (ASME Y14.5-2018): Concentricity and Symmetry were removed from the standard in the 2018 revision because both can be (and now should be) controlled with Position tolerance using appropriate datum references and material condition modifiers. They still appear on legacy drawings and you'll see them on older equipment, so we cover them below — but new designs should use Position instead.

Profile tolerances (Profile of a Line and Profile of a Surface) are the most versatile: a single profile callout with an appropriate datum reference can control form, orientation, location and even size simultaneously. Modern GD&T best practice favours profile tolerances over multiple stacked controls where appropriate.

Form tolerances — Straightness, Flatness, Circularity, Cylindricity

Form tolerances control how a feature deviates from its perfect geometric shape in isolation. No datum is required — these are characteristics of the feature itself, regardless of how it sits in space.

Straightness — symbol: a horizontal line ⏤

What it controls: how straight a line element on a surface, the axis of a cylinder, or a centre plane is.

Tolerance zone (line element on a surface): the tolerance value defines the width of a 2-dimensional zone — two parallel straight lines, separated by the tolerance value, in the plane of the toleranced line element. Every point on the surface line must lie between these two parallel reference lines. Imagine a perfectly straight reference line; the surface can wave above and below it, but no point can exceed half the tolerance value above or below.

Tolerance zone (axis of a cylinder, with the symbol applied to the diameter dimension): when straightness is applied to an axis (typically by placing the FCF below the diameter dimension or with a ⌀ symbol in the FCF), the tolerance zone becomes a cylindrical zone of the specified diameter, within which the axis of the feature must lie. The axis can curve or tilt within this cylinder, but cannot exit it.

Application: shafts, pins, edges of plates where a straight datum will mate against another part, machine tool ways, alignment fixtures.

ISO 1101 vs ASME Y14.5: identical in symbol and meaning. ISO uses the same horizontal-line symbol with the same interpretation.

Flatness — symbol: a parallelogram ⏥

What it controls: how flat a planar surface is.

Tolerance zone: two parallel planes separated by the tolerance value, between which all points of the surface must lie. The two planes are not located at any specified position in space — they are wherever they need to be to contain the entire surface within the specified gap. The actual surface can be high or low anywhere within that envelope.

Application: machined faces that mate to gaskets, bearing seats, mounting pads, surface plates, machine tool tables, optical mounts, sealing surfaces.

Practical note: flatness is one of the most-used GD&T controls because surface flatness is critical for almost any sealed or seated mating part. A flatness tolerance is independent of the size of the part — a 0.05 mm flatness on a 50 mm pad and on a 500 mm pad both mean the surface is contained within a 0.05 mm gap between two parallel planes.

Circularity (Roundness) — symbol: a circle ◯

What it controls: how round a circular cross-section is. Applied to a single cross-section perpendicular to the axis of a feature of revolution (cylinder, cone, sphere).

Tolerance zone: two concentric circles in the plane perpendicular to the axis of the feature, separated radially by the tolerance value. Every point on the circumference at that cross-section must lie between the two circles. The two circles are not located at any particular centre — they are wherever they need to be to contain the actual cross-section within the radial gap.

Application: bearing journals, cylindrical pins, pump shafts, rotating components where the cross-section roundness affects bearing or seal contact.

Note on terminology: "circularity" is the modern ASME and ISO term; "roundness" is the older term and still used colloquially. AS/NZS 1100 follows ISO and uses "circularity".

Cylindricity — symbol: a circle with two slanted parallel lines ⌭

What it controls: how cylindrical a feature is — combines circularity at every cross-section AND straightness of all line elements along the cylinder. A composite form control for cylinders.

Tolerance zone: two coaxial cylinders, separated radially by the tolerance value, between which the entire cylindrical surface must lie. Like circularity, the two cylinders are not located in space — they are wherever they need to be to contain the entire surface within the radial gap. Unlike circularity (a 2D control at one cross-section), cylindricity is a 3D control along the entire length.

Application: bearing journals where both roundness AND straight cylindrical form matter, hydraulic ram rods, precision shafts, gauge pins, master cylinders.

Cost implication: cylindricity is more demanding to inspect than circularity (requires multiple cross-sections measured, or a roundness machine with axial scanning) and more demanding to manufacture (requires consistent grinding or hard-turning along the full length). Apply only where the function requires it.

Orientation tolerances — Perpendicularity, Parallelism, Angularity

Orientation tolerances control the angular relationship between a feature and a datum. A datum is required — the reference frame the orientation is measured against.

Perpendicularity — symbol: an inverted T ⟂

What it controls: how square (90°) a feature is to a datum. Applied to a surface, an axis or a centre plane.

Tolerance zone (surface): two parallel planes separated by the tolerance value, oriented perpendicular to the datum, between which the toleranced surface must lie.

Tolerance zone (axis, with ⌀ symbol): a cylindrical zone of the specified diameter, oriented perpendicular to the datum plane, within which the axis of the feature must lie.

Application: drilled holes that must be square to a mating face (press-fit pins, dowel holes, locating bushes); machined faces that must be square to a base; vertical columns on machine bases.

Real-world implication: a hole position can be perfectly correct in X-Y coordinates but still be a perpendicularity reject — if the hole is tilted, a press-fit pin won't enter or won't seat fully. Perpendicularity catches what pure coordinate dimensioning misses.

Parallelism — symbol: two parallel slanted lines ⫽

What it controls: how parallel a feature is to a datum.

Tolerance zone (surface): two parallel planes separated by the tolerance value, oriented parallel to the datum, between which the toleranced surface must lie.

Tolerance zone (axis, with ⌀ symbol): a cylindrical zone of the specified diameter, oriented parallel to the datum, within which the axis of the feature must lie.

Application: upper and lower surfaces of a machined block where the two faces must remain parallel (jig plates, slide blocks, parallels for machining setups); bearing housing bores in a gearbox where axes must remain parallel; rail tracks for linear motion guides.

Angularity — symbol: an angle ∠

What it controls: how close a feature is to a specified angle other than 90° or 0°, measured against a datum.

Tolerance zone: two parallel planes separated by the tolerance value, oriented at the specified angle to the datum, between which the toleranced surface must lie. (Or for an axis: a cylindrical zone at the specified angle.)

Application: chamfers with critical angles, dovetail slides, tapered surfaces, V-block mating faces, draft angles on castings where the angle matters.

Note: angularity is the angle-equivalent of perpendicularity (which is angularity at 90°) and parallelism (angularity at 0°). The symbol is reserved for non-90, non-0 angles. The angle itself is typically given as a basic dimension (boxed) in the drawing, with the tolerance value applied through the angularity FCF.

Location tolerances — Position, Concentricity, Symmetry

Location tolerances control where a feature is in space, relative to a datum reference frame. Position is the workhorse; concentricity and symmetry are largely deprecated in favour of position with appropriate datums.

Position — symbol: a circle with crosshairs ⌖

What it controls: the location of a feature's centre point, axis or centre plane relative to a datum reference frame.

Tolerance zone (axis, most common, with ⌀ symbol): a cylindrical zone of the specified diameter, located at the perfect (basic) position relative to the datums, within which the axis of the actual feature must lie. The basic position is given as boxed dimensions on the drawing — the basic dimension is theoretically perfect; the position FCF allows variation only within the cylindrical tolerance zone.

Tolerance zone (surface or centre plane, without ⌀): two parallel planes separated by the tolerance value, located at the basic position, between which the centre plane or surface must lie.

The single most-used GD&T control. Position with appropriate datum references and material condition modifiers can replace concentricity, symmetry and most other location controls. Position with MMC modifier is the standard for hole patterns (bolt circles, pin patterns, mounting hole arrays).

Terminology change (ASME Y14.5-2009 and later): the term "true position" was officially dropped in 2009; the modern term is just "position". You'll still hear "true position" used colloquially and on legacy drawings — they mean the same thing.

ISO 1101: the symbol and meaning are identical to ASME. ISO calls it "position" too.

Concentricity — symbol: two concentric circles ◎ (deprecated in ASME Y14.5-2018)

What it controlled: the median points of all diametrically-opposed elements of a feature of revolution must lie on a common axis with the datum axis. In effect, the feature's axis must coincide with the datum axis within the tolerance zone (a cylindrical zone of the specified diameter, coaxial with the datum).

Why deprecated: concentricity is extremely difficult to measure correctly. The "median points" definition requires identifying opposite-side surface points, calculating their midpoints, and checking whether all those midpoints fall within the tolerance zone. In practice, inspectors often (incorrectly) substituted runout or position checks. ASME Y14.5-2018 removed concentricity from the standard, recommending Position with appropriate datum modifiers instead.

What to do today: use Position tolerance applied to the feature's axis with the datum axis as primary datum, often with MMC modifier. The result is functionally similar without the measurement ambiguity.

ISO 1101: ISO retained concentricity in ISO 1101:2017 — but ISO terminology and tolerance zone definition differs from ASME. AS/NZS-aligned drawings tend to follow whichever standard the title block cites; in modern practice, position is preferred.

Symmetry — symbol: three horizontal lines stacked ⌯ (deprecated in ASME Y14.5-2018)

What it controlled: the median points of all opposed elements of a feature must lie within a tolerance zone defined by two parallel planes equidistant from the datum centre plane.

Why deprecated: same measurement issue as concentricity — median points are hard to inspect. Replaced in ASME Y14.5-2018 by Position tolerance applied to the feature's centre plane.

ISO 1101: retained, with the same symbol.

Profile tolerances — Profile of a Line, Profile of a Surface

Profile tolerances are the Swiss Army knives of GD&T. A single profile callout with appropriate datum references can simultaneously control form, orientation, location and size of an irregular feature. They are increasingly used in modern drawings, often replacing multiple stacked tolerances.

Profile of a Line — symbol: an open semicircle ⌒

What it controls: the form (and optionally orientation and location, depending on whether datums are referenced) of a 2-dimensional line element across a surface — for example, the cross-section of an extrusion, a turned surface profile, a sheet metal section.

Tolerance zone: two curves parallel to the basic (perfect) profile, offset by half the tolerance value above and half below the perfect profile. Every point on the actual line element must lie between these two curves.

Application: 2D profiles of moulded or cast features where only the cross-section matters; airfoil sections; cam profiles measured at one cross-section; sheet metal stamping profiles.

Profile of a Surface — symbol: a closed semicircle (with line) ⌓

What it controls: the form (and optionally orientation and location) of a 3-dimensional surface — for example, the entire profile of a moulded boss, a turbine blade, a complex machined feature.

Tolerance zone: two surfaces parallel to the basic perfect surface, offset above and below by half the tolerance value. The entire 3D surface must lie within this zone.

The power of profile: profile tolerance combines what would otherwise need separate form, orientation, location and size controls into one. Increasingly used in moulded plastic parts, complex machined surfaces, automotive sheet metal, aerospace control surfaces, and 3D-printed parts where conventional dimensioning is impractical.

Without a datum reference: profile becomes a pure form control — the actual surface must match the basic profile in shape, regardless of where it sits in space.

With one datum: orientation is added — the profile must match the basic shape AND be oriented correctly relative to the datum.

With multiple datums (full DRF): location is added — the profile must match shape, orientation AND location.

ISO 1101: identical symbols and meanings. ISO uses the same convention.

Runout tolerances — Circular Runout, Total Runout

Runout tolerances apply to features of revolution and control how the surface deviates as the part rotates about a datum axis. A datum axis is mandatory.

Circular Runout — symbol: an arrow at an angle ↗

What it controls: the maximum allowable variation in a 2D cross-section of a rotating surface, measured at any single position along the axis. Effectively combines circularity and concentricity at that one cross-section.

Tolerance zone: at any cross-section perpendicular to the datum axis, the maximum-to-minimum range of indicator readings as the part rotates 360° must not exceed the tolerance value. The zone is essentially the difference between two coaxial circles at that cross-section.

Application: shaft surfaces where a single cross-section runs against a seal lip; rotating parts where dynamic balance and concentric rotation matter at specific stations along the shaft.

Inspection method: rotate the part on the datum axis, place a dial indicator on the surface at one position, record full-revolution Total Indicator Reading (TIR). Repeat at multiple cross-sections — each one separately must be within the tolerance.

Total Runout — symbol: two arrows at an angle ↗↗

What it controls: the maximum allowable variation across the entire rotating surface, measured continuously as the part rotates about the datum axis with the indicator traversed along the axis. Combines circularity, cylindricity AND coaxiality with the datum across the full surface length.

Tolerance zone: two coaxial cylinders, separated radially by the tolerance value, with the datum axis. The entire rotating surface must lie within this annular zone.

Application: bearing journals where consistent runout along the full length matters; rotor surfaces for sealing; pulley or sheave grooves where eccentricity at any point causes belt vibration.

Total runout is more demanding than circular runout — circular runout might pass at every individual cross-section while total runout fails because the cylinder as a whole is not coaxial with the datum. Specify total runout when full-length runout matters; specify circular runout when only specific stations matter.

The feature control frame (FCF) decoded

The feature control frame is the rectangular notation that carries the GD&T information on a drawing. Reading an FCF correctly is the single biggest hurdle for newcomers to GD&T. Each compartment of the FCF has a specific job.

Standard FCF format (left to right):

1. Geometric characteristic symbol — the GD&T symbol (one of the 14 covered above)
2. Diameter symbol (⌀) if applicable — indicates a cylindrical tolerance zone (axis or centre point control)
3. Tolerance value — the size of the tolerance zone, in mm or inches per the drawing convention
4. Material condition modifier (optional) — Ⓜ (MMC), Ⓛ (LMC), or none (RFS, the default)
5. Primary datum reference (if datum required) — letter, e.g. A
6. Secondary datum reference (optional) — letter, e.g. B
7. Tertiary datum reference (optional) — letter, e.g. C
8. Datum modifier (optional) — Ⓜ or Ⓛ applied to a datum letter

Worked example — an FCF reading [⌀ 0.1 Ⓜ A B C]:

1. The geometric characteristic is Position (◌, the position symbol)
2. The ⌀ symbol means the tolerance zone is cylindrical
3. The tolerance value is 0.1 mm — diameter of the cylindrical zone
4. The Ⓜ modifier means the tolerance applies at MMC (Maximum Material Condition) — bonus tolerance is available as the feature departs from MMC
5. Datum A is primary (3 contact points, locks 3 degrees of freedom)
6. Datum B is secondary (2 contact points, locks 2 more degrees of freedom)
7. Datum C is tertiary (1 contact point, locks the final translational degree of freedom)
8. Together, A-B-C constitute the full datum reference frame

Reading order matters. The datum letters in an FCF are read primary-secondary-tertiary regardless of the alphabetic value of the letter. [A B C] and [B A C] are different — different feature contacts the part first, different degrees of freedom locked first. Engineers and machinists must respect the order specified.

Datums and the datum reference frame (DRF)

A datum is a theoretically perfect reference (point, axis, plane) from which other features are measured. The actual physical surface or feature on the part that simulates the datum is called a datum feature — distinct from the datum itself.

For example: the bottom of a part might be machined to be the primary datum feature. The datum itself is the theoretical perfect plane that contacts the high points of that surface when the part sits on a surface plate. The datum is the reference; the datum feature is the imperfect physical surface that simulates the reference.

Primary, secondary, tertiary datums

A complete datum reference frame typically uses three orthogonal datums to fully constrain the part in space. Each lock progressively more degrees of freedom:

• Primary datum (3 contact points) — the first contact, locks 3 degrees of freedom: 1 translational + 2 rotational. Typically the largest, flattest, most functional surface — the surface the part sits on or seats against in assembly.
• Secondary datum (2 contact points) — locks 2 more degrees of freedom: 1 translational + 1 rotational. Typically a perpendicular face or a hole used to locate a corner or edge.
• Tertiary datum (1 contact point) — locks the final translational degree of freedom. Typically an edge or hole that finalises the corner location.

Practical interpretation: when an inspector clamps a part for measurement, they should be clamping it down on the primary datum first (3-point seat), then registering it against the secondary (2-point seat), then locating the tertiary (1-point seat). The part is now in the same orientation it would be in for assembly, and measurements are repeatable.

Datum feature simulation in practice

On a CMM (coordinate measuring machine), datums are simulated by mathematical "best-fit" planes, axes and points calculated from probed points on the datum features. On a manual measurement bench, datums are simulated by precision surface plates (primary), angle plates (secondary) and pin gauges (tertiary). The exact simulation method matters for measurement accuracy — a part can pass on one fixture and fail on another if the datum simulation differs.

Material condition modifiers — MMC, LMC, RFS

Material condition modifiers describe the size of the feature when its tolerance applies. They appear inside the FCF after the tolerance value.

Maximum Material Condition (MMC) — symbol: Ⓜ

The condition where the feature contains the maximum amount of material within its size tolerance. For an external feature (like a shaft), MMC is the maximum diameter. For an internal feature (like a hole), MMC is the minimum diameter. MMC is the worst-case for fit — the situation where assembly is hardest.

When MMC is specified, the feature gains "bonus tolerance" as it departs from MMC. Example: a hole specified ⌀ 10.0 +0.2/-0.0 with position tolerance ⌀ 0.1 Ⓜ at MMC. At MMC (10.0 mm minimum hole), the position tolerance is exactly 0.1 mm. As the hole grows toward LMC (10.2 mm), the bonus tolerance grows by the difference — the position tolerance becomes 0.1 + (10.2 - 10.0) = 0.3 mm at LMC. The hole has more positional freedom when it's larger, because the larger hole accepts the mating part with more clearance.

Use MMC for assembly-critical features — bolt holes, pin holes, dowel hole patterns. The bonus tolerance is functionally equivalent to the available clearance, so it costs nothing in fit while making manufacture easier.

Least Material Condition (LMC) — symbol: Ⓛ

The condition where the feature contains the least amount of material within its size tolerance. For external features (shaft), LMC is the minimum diameter; for internal features (hole), LMC is the maximum diameter.

LMC is the inverse of MMC — bonus tolerance increases as the feature moves toward MMC. Used for wall-thickness-critical applications: where a bonus from a larger hole or smaller boss would compromise the wall thickness or strength of the part. Less commonly applied than MMC.

Regardless of Feature Size (RFS) — no symbol (default)

The tolerance applies regardless of the feature's actual size — no bonus tolerance is available, no matter how the feature size varies within its size tolerance.

RFS is the default in ASME Y14.5-1994 and later. If no modifier symbol appears in the FCF, RFS applies. (Older drawings to ASME Y14.5-1982 used the Ⓢ symbol explicitly; this is now obsolete and should not appear on modern drawings, though you'll see it on legacy work.)

RFS is used where tolerance must be held strictly regardless of fit — precision shafts, sealing surfaces, kinematic alignments where the function depends on the absolute geometric relationship.

Bonus tolerance and virtual condition

Bonus tolerance is the extra geometric tolerance that becomes available when an MMC or LMC modifier is in effect and the feature size is not at the worst-case condition.

Bonus tolerance formula (MMC modifier):

• Bonus = Actual feature size — MMC size (for internal features like holes — bonus exists when hole is larger than minimum)
• Bonus = MMC size — Actual feature size (for external features like shafts — bonus exists when shaft is smaller than maximum)
• Total geometric tolerance available = Stated tolerance + Bonus tolerance

Worked example — hole with position-MMC:

• Hole size: ⌀ 10.0 +0.2/-0.0 (MMC = 10.0 mm, LMC = 10.2 mm)
• Position tolerance: ⌀ 0.1 Ⓜ A B C
• If hole is measured at 10.0 mm: position tolerance = 0.1 mm (no bonus — hole is at MMC)
• If hole is measured at 10.1 mm: position tolerance = 0.1 + 0.1 = 0.2 mm (10.1 - 10.0 = 0.1 bonus)
• If hole is measured at 10.2 mm: position tolerance = 0.1 + 0.2 = 0.3 mm (full bonus available)

Virtual condition is the worst-case mating size of a feature, accounting for its size tolerance and its geometric tolerance applied at MMC. It defines the size of the gauge that would just accept (or just clear) the feature in its worst combined state.

• Virtual condition (external feature, MMC) = MMC size + geometric tolerance
• Virtual condition (internal feature, MMC) = MMC size − geometric tolerance

Virtual condition is the basis for functional gauging — a Go gauge designed to the virtual condition will accept any acceptable part regardless of where in its tolerance range each individual measurement falls. This is the operational power of MMC tolerancing: it guarantees assembly fit while allowing maximum manufacturing freedom.

Common GD&T mistakes and how to avoid them

Mistake 1 — incomplete datum reference frame. Specifying only one or two datums when three are needed for full constraint. Result: ambiguous measurement, parts that pass inspection but don't assemble. Fix: specify primary, secondary and tertiary datums whenever the geometric tolerance requires full constraint (which is most position, profile and orientation tolerances).

Mistake 2 — wrong datum order. Listing datums in the wrong primary-secondary-tertiary order (e.g. [B A C] when the function requires [A B C]). The order determines which surface is contacted first during inspection, which locks degrees of freedom in which sequence. Fix: think about the assembly — what surface seats the part first in actual use? That's the primary.

Mistake 3 — applying MMC where it doesn't apply functionally. Modifier choice matters. MMC for assembly-critical features (bolt holes); LMC for wall-thickness-critical features; RFS for kinematic precision. Don't blanket-apply MMC because it gives the most bonus.

Mistake 4 — concentricity or symmetry on new drawings. Both deprecated in ASME Y14.5-2018. New designs should use Position with appropriate datum references and modifiers. Existing drawings to older standards remain valid.

Mistake 5 — coordinate ± tolerances mixed with GD&T without clarity. If a drawing has both ±tolerances and GD&T tolerances on the same feature, which controls? Best practice: GD&T tolerances control geometric characteristics; ± tolerances control feature size only. The drawing's general notes should make this clear.

Mistake 6 — over-specifying tolerance with multiple controls. Profile tolerance with appropriate datums often replaces stacked controls (form + orientation + location + size). Reducing to one well-chosen control simplifies inspection and reduces inspection cost.

Mistake 7 — under-specifying for the function. Putting only ±tolerances on a part where assembly fit, sealing, or rotation balance matters. The cheaper-looking drawing produces parts that look right but don't work.

Mistake 8 — ignoring the standard cited. ASME Y14.5-2018 differs from ISO 1101:2017 in subtle but significant ways: default rules for size, datum simulation conventions, modifier conventions. Always know which standard the drawing references and apply its rules.

Reading a real engineering drawing

Putting it together — here's how to parse a feature control frame and supporting dimensions on a real engineering drawing.

Worked example:

You have a steel mounting plate with three holes. The drawing shows:

• Hole pattern dimensioned with basic dimensions (boxed): 50 mm x-spacing, 25 mm y-spacing, 10 mm from datum B edge, 10 mm from datum C edge.
• Hole size: ⌀ 8.0 +0.3/-0.0
• Feature control frame: [◌ ⌀ 0.2 Ⓜ A B C]
• Datum A is the bottom face, identified by an [A] label with leader to that surface.
• Datum B is one edge, identified [B].
• Datum C is the perpendicular edge, identified [C].
• Title block: "ASME Y14.5-2018".

Reading this drawing:

1. The standard is ASME Y14.5-2018. RFS is the default unless otherwise noted; modifier conventions per 2018.
2. The hole size is 8.0 mm minimum (MMC), 8.3 mm maximum (LMC).
3. The geometric characteristic is Position (◌). The tolerance zone is cylindrical (⌀). The diameter of the zone at MMC is 0.2 mm.
4. The position tolerance applies at MMC — bonus tolerance is available as the hole grows from 8.0 toward 8.3 mm.
5. Datums A-B-C in that order: A primary (3 contact points on the bottom face — locks Z, rotation about X, rotation about Y); B secondary (2 contact points — locks X translation, rotation about Z); C tertiary (1 contact point — locks Y translation).
6. For each hole: locate the basic position from the boxed dimensions (10 mm + n × spacing, etc.); the actual hole axis must lie within a cylindrical zone of diameter [0.2 mm + bonus tolerance from hole size measurement] centred on the basic position, with the cylinder oriented perpendicular to datum A and located by datums B and C.

This is what a feature control frame says, in plain English. Once you've parsed two or three FCFs, the pattern becomes second nature — and the drawing shifts from a confusing technical document to an unambiguous specification you can manufacture and inspect to.

Quick reference: the GD&T symbol cheat sheet

Symbol name	Symbol	Category	Datum required?	Modifier compatible (MMC/LMC)?	Tolerance zone
Straightness	⏤ (horizontal line)	Form	No	Only when applied to axis or centre plane (not surface elements)	Two parallel straight lines (line element) OR cylindrical zone (axis)
Flatness	⏥ (parallelogram)	Form	No	No	Two parallel planes
Circularity / Roundness	◯ (circle)	Form	No	No	Two concentric circles in a cross-section perpendicular to axis
Cylindricity	⌭ (circle with slanted lines)	Form	No	No	Two coaxial cylinders
Perpendicularity	⟂ (inverted T)	Orientation	Yes	Yes (axis or centre plane)	Two parallel planes (surface) OR cylindrical zone (axis), oriented 90° to datum
Parallelism	⫽ (two parallel slanted lines)	Orientation	Yes	Yes (axis or centre plane)	Two parallel planes (surface) OR cylindrical zone (axis), parallel to datum
Angularity	∠ (angle)	Orientation	Yes	Yes (axis or centre plane)	Two parallel planes at the basic angle to datum
Position	◌ (circle with crosshairs)	Location	Yes	Yes	Cylindrical zone (axis) or two parallel planes (centre plane), located at basic position
Concentricity (deprecated 2018)	◎ (concentric circles)	Location	Yes (axis)	No (per ASME 1994 onwards)	Cylindrical zone, coaxial with datum axis
Symmetry (deprecated 2018)	⌯ (three stacked lines)	Location	Yes (centre plane)	No	Two parallel planes, equidistant from datum centre plane
Profile of a Line	⌒ (open semicircle)	Profile	Optional	No	Two parallel curves offset from basic profile (2D)
Profile of a Surface	⌓ (closed semicircle)	Profile	Optional	No	Two parallel surfaces offset from basic profile (3D)
Circular Runout	↗ (single arrow)	Runout	Yes (axis)	No	Two coaxial circles at any single cross-section
Total Runout	↗↗ (double arrow)	Runout	Yes (axis)	No	Two coaxial cylinders for the full feature length

Where to learn more — and a portable reference

For a portable, machinist-pocket-sized reference covering GD&T plus the broader engineering toolbox (thread tables, drill sizes, material data, formulas, conversions), the Engineer's Black Book (Metric, 3rd Edition) is a long-running Australian industry standard. Its GD&T section condenses the symbols, modifier rules and FCF reading conventions covered in this guide into a quick-reference format that fits in a workshop apron pocket. For the full contents listing across the Engineer's, Fastener and Electrical Black Book series, see our Black Books contents reference.

For depth, the authoritative sources are the standards themselves — ASME Y14.5-2018 (purchased through ASME), ISO 1101:2017 (purchased through Standards Australia or ISO directly), and AS/NZS 1100 Part 201 (Standards Australia). For training, ASME, Tec-Ease, and KEYENCE all publish accessible GD&T introductions. For Australian university-level coverage, AS/NZS 1100 is the curriculum-standard reference in mechanical engineering programs.

Frequently Asked Questions

What are the 14 GD&T symbols?

The 14 GD&T symbols, grouped by category: Form — Straightness, Flatness, Circularity (Roundness), Cylindricity (4 symbols, no datum required). Orientation — Perpendicularity, Parallelism, Angularity (3 symbols, datum required). Location — Position, Concentricity (deprecated 2018), Symmetry (deprecated 2018). Profile — Profile of a Line, Profile of a Surface (datum optional). Runout — Circular Runout, Total Runout (datum axis required). All 14 are covered in detail in the cheat sheet table in this guide.

What is the difference between ASME Y14.5 and ISO 1101?

Both define GD&T conventions but with subtle differences. ASME Y14.5 is the American standard, predominantly used in US-aligned aerospace, automotive, defence and oil/gas industries. ISO 1101 (with the broader ISO Geometrical Product Specifications series) is the international standard, used in European-aligned manufacturing, medical devices and most non-US automotive. Differences include: default rules for the relationship between size and form (ASME has Rule #1, ISO uses the independence principle); concentricity and symmetry retained in ISO but deprecated in ASME 2018; datum simulation methods and modifier conventions vary. AS/NZS 1100 Part 201 — the Australian technical drawing standard — is broadly aligned with ISO conventions. Always check the drawing title block for the specific standard cited.

What is the 3-2-1 rule in GD&T?

The 3-2-1 rule defines how three orthogonal datums fully constrain a part in space for measurement and inspection. The primary datum contacts the part at 3 points (defining a plane and locking 3 degrees of freedom). The secondary datum adds 2 contact points (defining a line perpendicular to primary, locking 2 more degrees of freedom). The tertiary datum adds 1 contact point (locking the final translational degree of freedom). 3 + 2 + 1 = 6 contact points = 6 degrees of freedom locked = part fully constrained. The rule defines the contact-point hierarchy when establishing a complete datum reference frame.

What is a feature control frame?

The feature control frame (FCF) is the rectangular notation on a drawing that contains the GD&T information for a feature. Reading left to right, the FCF contains: the geometric characteristic symbol (which of the 14 GD&T tolerances applies); the diameter symbol (⌀) if the tolerance zone is cylindrical; the tolerance value; an optional material condition modifier (Ⓜ for MMC, Ⓛ for LMC, none for RFS); and the datum reference letters in primary-secondary-tertiary order. Together, the FCF gives the complete specification: what to control, how much variation is allowed, under what material conditions, and relative to what reference.

What does MMC mean in GD&T?

MMC stands for Maximum Material Condition — the condition where a feature contains the maximum amount of material within its size tolerance. For an external feature like a shaft, MMC is the maximum diameter; for an internal feature like a hole, MMC is the minimum diameter. When a tolerance is specified at MMC (with the Ⓜ modifier), bonus tolerance becomes available as the feature departs from MMC — the hole gets more positional freedom as it gets larger, the shaft gets more positional freedom as it gets smaller. MMC is used for assembly-critical features like bolt holes and pin patterns, where the bonus tolerance corresponds to actual mating clearance.

What is the difference between MMC and LMC?

MMC (Maximum Material Condition) is the condition where the feature contains the most material — maximum shaft diameter, minimum hole diameter. LMC (Least Material Condition) is the inverse — minimum shaft diameter, maximum hole diameter. Use MMC for assembly-critical features (most common use), where bonus tolerance corresponds to mating clearance. Use LMC for wall-thickness-critical features — boss locations, hole positions where the wall around the hole must remain thick enough for strength. LMC is less common but functionally important when wall thickness is the design driver.

What is bonus tolerance?

Bonus tolerance is extra geometric tolerance that becomes available when an MMC or LMC modifier is in effect and the feature size is not at the worst-case condition. For a hole with position tolerance ⌀ 0.1 Ⓜ at MMC: at the MMC size (smallest hole), the position tolerance is exactly 0.1 mm. As the hole grows toward LMC, bonus equal to the size deviation is added — at maximum hole size, total position tolerance = 0.1 + (size deviation) mm. The bonus tolerance corresponds to the actual mating clearance available, so it costs nothing in fit while making manufacture easier. Total available tolerance = stated tolerance + bonus.

What does RFS mean and is it still used?

RFS stands for Regardless of Feature Size — the tolerance applies regardless of how the feature size varies within its size tolerance. No bonus tolerance is available. RFS is the default condition in ASME Y14.5-1994 and later — if no modifier symbol appears in the feature control frame, RFS is implied. The Ⓢ symbol (older convention) is now obsolete; legacy drawings to ASME Y14.5-1982 or earlier may still show it. RFS is used for precision applications where geometric tolerance must be held strictly regardless of fit — sealing surfaces, kinematic alignments, optical mounts.

What is the difference between position and true position?

They are the same thing. "True position" was the official term in ASME Y14.5-1982 and earlier; "position" is the term in ASME Y14.5-2009 and later. The change reflected that the term "true" was redundant — there is no "false" position to distinguish it from. You will still hear "true position" used colloquially and on legacy drawings; both refer to the same geometric characteristic and use the same symbol (⌖, a circle with crosshairs). ISO 1101 has always used "position" without the "true" prefix.

What is a datum reference frame?

A datum reference frame (DRF) is the complete set of orthogonal datums that fully constrains a part in space for measurement and inspection. It typically consists of three mutually-perpendicular datums — primary, secondary, tertiary — applied in that order to lock the six degrees of freedom (three translational, three rotational) of a rigid body. The DRF establishes the coordinate system in which all geometric tolerances are interpreted. Different parts may use different DRF combinations depending on functional priorities — what surface seats the part first in actual assembly is typically the primary datum.

What is the difference between concentricity and runout?

Both apply to features of revolution and require a datum axis. Concentricity controls the location of the median points of opposed elements relative to the datum axis — the actual feature axis must coincide with the datum axis within a cylindrical zone. Runout (circular or total) controls the surface deviation as the part rotates — the maximum-to-minimum indicator reading across rotation. Concentricity is hard to measure directly (median points are mathematically derived); runout is easy (just rotate the part and observe). For this reason, concentricity was deprecated in ASME Y14.5-2018; runout, or position tolerance with appropriate datums, is now preferred. ISO 1101 retains concentricity.

When should I use a profile tolerance instead of explicit form/orientation/position?

Profile tolerance (of a line or of a surface) is increasingly preferred in modern GD&T because a single profile callout with appropriate datum references can simultaneously control form, orientation, location and size of an irregular feature. Use profile when the feature is non-cylindrical and non-planar (curved surfaces, complex shapes, moulded parts, sheet metal stampings); when multiple stacked controls would otherwise be needed; or when the feature is essentially "this shape, here, at this orientation" and a unified specification is clearer. Use explicit form/orientation/position controls when the feature is regular (planar, cylindrical) and individual characteristic constraints suit better.

What is virtual condition?

Virtual condition is the worst-case mating size of a feature, accounting for both its size tolerance and its geometric tolerance applied at MMC. For an external feature (shaft) with position-MMC: virtual condition = MMC size + geometric tolerance value. For an internal feature (hole): virtual condition = MMC size − geometric tolerance value. Virtual condition is the basis for functional gauging — a Go gauge designed to virtual condition will accept any acceptable part regardless of where in its tolerance range each individual measurement falls. Virtual condition is the key concept linking MMC tolerancing to assembly fit guarantee.

Is GD&T mandatory on engineering drawings?

It depends on the customer, industry and standards cited. Aerospace, defence, medical device and automotive industries typically mandate GD&T for functional features. Less critical fabrication may use only ±tolerances. AS/NZS 1100 Part 201 — the Australian technical drawing standard — accommodates both, but for any feature where assembly fit, sealing, rotation balance or interchangeability matters, GD&T is the appropriate tool. The drawing's title block notes typically state which standard applies and whether GD&T is required.

How do I learn GD&T as a beginner?

Start by understanding why GD&T exists — the failure modes of pure ±coordinate tolerancing in functional applications. Then learn the 14 symbols and their tolerance zones one category at a time (form first, then orientation, location, profile, runout). Practice reading feature control frames on real drawings. Understand the 3-2-1 datum rule and material condition modifiers. Work through bonus tolerance calculations until they're second nature. The standards (ASME Y14.5, ISO 1101) are the authoritative reference but heavy reading; introductory training materials from ASME, Tec-Ease, KEYENCE or the Engineer's Black Book are more accessible starting points. Most engineers and inspectors take six months to a year of regular drawing exposure to become fluent in GD&T.