GD&T: Geometric Dimensioning & Tolerancing (2026)

What is GD&T?

GD&T (Geometric Dimensioning and Tolerancing) is a symbolic language defined by ASME Y14.5 that specifies form, orientation, location, and runout of features on a part. It uses datums as a repeatable measurement reference and tolerance zones (e.g., cylinders for position, pairs of parallel planes for flatness) instead of stacked ± dimensions. Use GD&T when parts must assemble with tight functional requirements—it often allows larger tolerance zones than ± callouts while maintaining fit, and reduces ambiguity for manufacturing and inspection.

The Fundamental Problem

Why GD&T Exists: The Problem with ± Tolerancing

Before you learn any GD&T symbols, you need to understand the problem GD&T was invented to solve. ± tolerancing has three fundamental limitations that cause rejected parts, assembly failures, and ambiguous drawings.

Square zone vs. cylindrical zone

When you locate a hole with ±0.005 in. in X and ±0.005 in. in Y, you create a square tolerance zone (0.010 × 0.010 in.). But holes are round — what matters functionally is the radial distance from true position. A cylindrical zone of ⌀0.014 in. (the inscribed circle of that square) gives you 57% more usable area than the ± square zone. GD&T position uses a cylindrical zone by default, so you get more tolerance — and cheaper parts — for the same functional requirement.

Tolerance stacking ambiguity

With ± dimensions, a 4-hole bolt pattern might be dimensioned from edge-to-first-hole, then hole-to-hole, then hole-to-hole, then hole-to-last-hole. Each ± tolerance stacks, and the total variation on the last hole relative to the first can be 4× the individual tolerance. GD&T position references all holes to the same datum reference frame, eliminating stack-up and making the drawing unambiguous.

No way to control form or orientation

± dimensions control size and location — they say nothing about whether a surface is flat, whether a bore is perpendicular to its mounting face, or whether a shaft is straight. A surface can be within ± tolerance on every individual dimension and still be warped, tapered, or out-of-round. GD&T adds form and orientation controls that ± cannot express.

No connection between size and location

Consider a hole that must accept an M6 bolt. If the hole is at maximum size (largest), it has more room for position error and will still assemble. ± dimensions cannot capture this relationship. GD&T's material condition modifiers (MMC, LMC) tie size to location tolerance — as the hole gets larger, the position tolerance grows (bonus tolerance), which reflects physical reality and enables functional gaging.

The bottom line

GD&T is not an academic exercise — it is the solution to real manufacturing problems. Every time a part fails assembly despite being “in tolerance” on every individual dimension, that failure was preventable with proper GD&T. The rest of this guide teaches you how.

Introduction

What is GD&T?

GD&T replaces or supplements linear ± dimensions with geometric tolerances that control form (flatness, roundness), orientation (parallelism, perpendicularity), location (position, concentricity), and runout. Each control uses a symbol, a tolerance value, and optionally datums. The result is a drawing that communicates design intent clearly and gives the shop a defined tolerance zone—often larger than the equivalent stacked ± box—which can lower cost and ease inspection.

Core Skill

How to Read a Feature Control Frame

The feature control frame (FCF) is the rectangle on a drawing that contains a GD&T callout. Every FCF reads left to right and has 2–5 compartments. Once you can read one, you can read any GD&T callout on any drawing.

Feature Control Frame Anatomy (read left → right)

Compartment	Contains	Example	Meaning
1st	Geometric characteristic symbol	⌖	Position (true position)
2nd	Tolerance value (may have ⌀ prefix for cylindrical zone)	⌀ 0.010	Cylindrical tolerance zone of 0.010 in. (0.25 mm) diameter
2nd (cont.)	Material condition modifier (optional)	Ⓜ	At MMC — bonus tolerance applies as feature departs from MMC
3rd	Primary datum reference	A	Measured relative to datum A (primary constraint — 3 DOF)
4th	Secondary datum reference	B	Secondary constraint — adds 2 more DOF
5th	Tertiary datum reference (optional)	C	Fully constrains the part — 6 DOF locked

Reading example: position callout

⌖ | ⌀ 0.010 Ⓜ | A | B | C

“The true position of this feature shall be within a cylindrical zone of 0.010 in. (0.25 mm) diameter at MMC, referenced to datums A (primary), B (secondary), C (tertiary).” If the hole is larger than MMC, bonus tolerance applies — the zone grows by the amount the hole departs from MMC.

Reading example: flatness callout

⏤ | 0.002

“This surface must lie between two parallel planes 0.002 in. (0.05 mm) apart.” No datum is referenced because flatness is a form control — it describes the shape of the surface independent of any other feature. The surface can be tilted or displaced; flatness only controls waviness.

Pro Tip

When you encounter an unfamiliar FCF on a drawing, read it aloud using this template: “The [symbol name] of this feature shall be within [tolerance value] [zone shape] [at material condition], referenced to datum [A], [B], [C].” This mechanical reading works for every GD&T callout and removes the guesswork.

Standards

GD&T Standards

In the US, ASME Y14.5-2018 is the authoritative standard for dimensioning and tolerancing. It defines symbols, datum reference frames, material condition modifiers (MMC, LMC, RFS), and rules for interpretation. Internationally, ISO 1101 (with ISO 5459 for datums) is used; symbolism and defaults differ slightly. Specify the standard in your title block (e.g., “ASME Y14.5-2018”) so suppliers and inspectors apply the same rules. All numeric values in this guide use dual units (inch and mm) where applicable.

Datums

Datums and Datum Reference Frames

A datum is a theoretically exact point, axis, or plane derived from a datum feature (a physical surface or feature of size). A datum reference frame (DRF) is built from primary (A), secondary (B), and tertiary (C) datums in order. Choose datum features that match assembly and function: typically a large mounting face as A, a locating hole or edge as B, and a third feature as C. The order defines how the part is constrained for measurement and manufacturing; changing the order can change the tolerance zone and cost.

Datum A: the mounting face

Choose the largest, most stable surface that contacts the mating part as datum A. For a bracket that bolts to a wall, datum A is the wall-contact face. For a bearing housing, datum A is the flange face that seats against the structure. Datum A removes 3 degrees of freedom (translation in one axis + rotation about two axes).

Datum B: the locating feature

Choose a feature that constrains the part in the remaining directions — typically a locating hole or an edge. For a bolt-pattern bracket, datum B is often the primary locating hole (the one with the tightest position tolerance). Datum B removes 2 more degrees of freedom.

Datum C: the anti-rotation feature

The tertiary datum prevents the part from rotating about the axis established by B. A second locating hole, a slot, or an edge serves this purpose. Not every part needs datum C — if the part is axially symmetric or orientation does not matter, two datums may suffice.

Common mistake: choosing small or flexible datums

New engineers often pick a small hole or a thin edge as a primary datum because it seems precise. But small features are unstable — measurement variability is high, and the part rocks on the inspection fixture. Choose the largest, stiffest surface. If the functional mounting surface is a large face, that is your primary datum — even if it has a wider flatness tolerance than a small bore.

Form Controls

Form tolerances control the shape of a single feature and do not require a datum. Flatness constrains a surface between two parallel planes. Straightness applies to a line or axis. Circularity (roundness) constrains a cross-section between two concentric circles. Cylindricity combines roundness, straightness, and taper for a cylinder. Typical values for machined parts: 0.001″–0.005″ (0.025–0.13 mm) for flatness and parallelism; 0.001″–0.003″ (0.025–0.08 mm) for circularity and cylindricity, depending on feature size and process.

Orientation and Location

Orientation and Location Controls

Orientation controls (parallelism, perpendicularity, angularity) relate a feature to a datum; they do not locate the feature. Location controls (position, concentricity, symmetry) define where a feature is relative to datums. Position (true position) is the most common location control: it defines a cylindrical or spherical zone (or rectangular in some cases) for the center of a hole, pin, or boss. Position at MMC allows bonus tolerance as the feature departs from MMC, which can reduce cost and enable functional gaging. Concentricity and symmetry are used less in modern practice; position or runout are often preferred per ASME Y14.5-2018.

Control	Requires Datum	Typical Use
Parallelism	Yes	Faces parallel to mounting surface
Perpendicularity	Yes	Bores or faces square to datum
Position	Yes (typically)	Hole patterns, pins, bosses
Runout	Yes (axis)	Rotating parts, bearings

Symbol Reference

GD&T Symbol Reference Table

Common GD&T symbols per ASME Y14.5-2018. Typical tolerance ranges are achievable under standard CNC machining conditions; tighter values may require secondary operations or specialized inspection.

Symbol	Name	Category	Description	Typical Tolerance
⏤	Flatness	Form	Surface must lie between two parallel planes. No datum required.	0.001″–0.005″ (0.025–0.13 mm)
—	Straightness	Form	Line or axis must lie within a tolerance zone (line or cylinder).	0.001″–0.005″ (0.025–0.13 mm)
○	Circularity (Roundness)	Form	Cross-section must lie between two concentric circles. No datum.	0.001″–0.003″ (0.025–0.08 mm)
⌭	Cylindricity	Form	Combined control of roundness, straightness, and taper of a cylinder.	0.001″–0.003″ (0.025–0.08 mm)
∥	Parallelism	Orientation	Surface or axis parallel to a datum plane or axis.	0.001″–0.005″ (0.025–0.13 mm)
⊥	Perpendicularity	Orientation	Surface or axis perpendicular to a datum.	0.001″–0.005″ (0.025–0.13 mm)
∠	Angularity	Orientation	Surface or axis at a specified angle to a datum.	0.001″–0.005″ (0.025–0.13 mm)
⌖	Position	Location	True position of a feature (hole, pin) relative to datums. Most common location control.	0.005″–0.010″ (0.13–0.25 mm) or ±0.002″ (±0.05 mm) RFS
◎	Concentricity	Location	Median points of a feature coincide with datum axis. (Note: ASME Y14.5-2018 recommends position or runout for new designs.)	0.002″–0.005″ (0.05–0.13 mm)
⊕	Symmetry	Location	Median points of a feature are symmetric about a datum plane. (Often replaced by position in modern practice.)	0.002″–0.005″ (0.05–0.13 mm)
↗	Circular Runout	Runout	Composite control of circularity and coaxiality at each cross-section.	0.001″–0.005″ (0.025–0.13 mm)
↗↗	Total Runout	Runout	Composite control over entire surface: circularity, straightness, coaxiality, taper.	0.002″–0.008″ (0.05–0.20 mm)

When to Use GD&T

When to Use GD&T vs ± Dimensions

Use GD&T when: (1) parts mate with other parts and fit depends on form or orientation—e.g., bearing bores, mounting faces, pin locations; (2) you want a larger tolerance zone than stacked ± (position gives a cylindrical zone); (3) you need to control form or orientation independently of size; (4) you want to enable functional gaging (e.g., position at MMC). Use ± dimensions for non-critical features, overall envelope dimensions, or when no datum relationship is needed. Avoid over-tolerancing: specify only the controls that affect function.

Inspection and Cost Impact

GD&T can reduce cost when it replaces overly tight ± tolerances with a single position or profile that allows a larger zone. It can increase cost when it requires CMM inspection, multiple datums, or very tight form/orientation. Position at MMC often allows fixed-size functional gages (fast); flatness and perpendicularity on large surfaces typically need CMM or surface plate. Call out inspection method in drawing notes when it matters for first-article or lot release.

Design tip

Only specify GD&T on features that affect fit, function, or assembly. Unnecessary form/orientation callouts add inspection time and cost. For a deeper dive on tolerance levels and cost, see our CNC Tolerances Guide.

Learn from Others

Common GD&T Mistakes New Engineers Make

These are the errors that show up most often in drawing reviews. Catching them before release saves weeks of back-and-forth with your supplier.

Over-tolerancing every feature

What goes wrong: Adding flatness, perpendicularity, and position to every surface and hole turns a simple bracket into an expensive precision part. Each GD&T callout adds inspection time (1–5 min per feature on a CMM). A 20-hole pattern with position, perpendicularity, and true position at RFS can add 60–100 min of CMM time per part.

Fix: Apply GD&T only to features that affect fit, function, or safety. Non-critical holes and surfaces should use standard ± block tolerances from your title block.

Wrong datum order (A, B, C)

What goes wrong: Swapping datum A and B changes how the part is constrained on the inspection fixture and can shift every measured position by the flatness error of the wrong primary datum. The shop builds fixtures based on datum order — changing it after first article is a costly revision.

Fix: Always match datum order to assembly sequence: primary datum = the surface that contacts the mating part first. Verify by asking: "If I set this part on a surface plate, which face touches first?"

Forgetting to specify the standard

What goes wrong: ASME Y14.5 and ISO 1101 differ in default material condition (ASME defaults to RFS; ISO interpretation varies), datum simulation, and composite position interpretation. If the drawing does not specify which standard applies, the shop guesses — and may guess wrong.

Fix: Add "DIMENSIONING AND TOLERANCING PER ASME Y14.5-2018" (or ISO 1101:2017) in the title block or general notes of every drawing.

Using concentricity when position or runout would work

What goes wrong: Concentricity per ASME Y14.5 requires measuring the median points of a feature — which is expensive (CMM with multiple cross-sections). ASME Y14.5-2018 specifically recommends position or runout for most applications because they are easier to inspect and functionally equivalent in most cases.

Fix: Use circular runout or total runout for rotating parts (shafts, bearings). Use position (with datum axis) for static coaxiality. Reserve concentricity for the rare case where median-point control is genuinely required.

Calling out form controls tighter than the location control

What goes wrong: Per ASME Y14.5 Rule #1, the form of a feature must be within its size tolerance. If you specify a hole with ±0.005 in. on diameter but call out cylindricity of 0.001 in., the cylindricity callout may be unnecessarily tight relative to the size tolerance — adding cost without functional benefit.

Fix: Form controls should be equal to or larger than what the size tolerance already controls, unless there is a specific functional need (e.g., a bearing bore where roundness matters independently of diameter).

No datum on orientation or location controls

What goes wrong: Perpendicularity, parallelism, angularity, position, and runout all require datum references. A feature control frame with a perpendicularity symbol and a tolerance but no datum is incomplete and will generate an RFI from the shop — or worse, the inspector invents a datum and the measurement is meaningless.

Fix: Form controls (flatness, straightness, circularity, cylindricity) do not need datums. Everything else does. If you wrote a datum letter in the FCF, check that the datum feature is labeled on the drawing with a datum feature symbol.

Common Questions

Frequently Asked Questions

What is GD&T and why use it instead of ± dimensions?

GD&T (Geometric Dimensioning and Tolerancing) is a symbolic language defined by ASME Y14.5 that controls form, orientation, location, and runout of features. Unlike ± linear dimensions, GD&T defines tolerance zones (e.g., a cylinder for position, two parallel planes for flatness) and uses datums to establish a repeatable measurement reference. Use GD&T when parts must assemble with functional requirements—bearing bores, mounting holes, sealing faces—because it communicates design intent clearly and often allows larger tolerance zones than stacked ± dimensions, reducing cost while maintaining fit.

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

ASME Y14.5 (US) and ISO 1101 (international) both define GD&T symbols and rules, but differ in default interpretations and modifiers. ASME Y14.5-2018 uses inches as the default unit and has specific rules for datum precedence, material condition (MMC/LMC/RFS), and composite position. ISO 1101 defaults to metric and uses slightly different symbolism in places (e.g., envelope requirement). For US-based manufacturing and supply chains, specify ASME Y14.5 on the drawing; for global programs, note the standard in the title block to avoid ambiguity.

When should I use position tolerance instead of ± dimensions?

Use position (true position) when you need to control the location of a feature (hole, pin, boss) relative to datums in a way that allows maximum tolerance zone. Position uses a cylindrical or spherical zone; ± X and ± Y on a hole effectively create a square tolerance zone, which is smaller than the inscribed circle. Position also clarifies that the tolerance applies at MMC or LMC when material condition is specified, enabling functional gaging and often reducing inspection cost. Reserve ± dimensions for non-critical features or when no datum relationship is needed.

How does GD&T affect manufacturing and inspection cost?

GD&T can reduce cost when it replaces over-tight ± tolerances with a single position or profile callout that gives the shop a larger usable zone. It can increase cost when it requires CMM or functional gage inspection, multiple datums, or very tight form/orientation controls. Typical impact: position callouts with MMC can allow functional pin gaging (fast); flatness and perpendicularity on large surfaces may require CMM or surface plate inspection. Specify only the controls that affect fit and function, and call out inspection method in the drawing notes when it matters.

What are datums and how do I choose them?

Datums are theoretically exact points, axes, or planes derived from datum features (physical part surfaces) that establish the reference frame for measurement. Choose datums that match how the part mounts or functions: a mounting face as primary datum A, a locating hole or edge as B, and a secondary locating feature as C. The order matters—A establishes the first plane, B the second, C the third. Use features that are stable, accessible for inspection, and representative of the part's function. Avoid datums on small or flexible features when a larger, stiffer surface can serve.

What is MMC, LMC, and RFS in GD&T?

MMC (Maximum Material Condition) means the feature is at its maximum material limit—largest pin, smallest hole. LMC (Least Material Condition) is the opposite—smallest pin, largest hole. RFS (Regardless of Feature Size) means the tolerance applies at any size. When you specify position at MMC, the position tolerance can increase (bonus tolerance) as the feature departs from MMC, which often allows easier assembly and enables fixed-size functional gages. RFS is the default in ASME Y14.5-2018 when no modifier is shown. Specify MMC or LMC when functional gaging or bonus tolerance is desired.