Reference chart

GD&T cheat sheet

All eleven geometric characteristics, each with its symbol, drawing callout, tolerance zone and inspection setup, plus datums, feature control frames and the material condition modifiers. Written to ASME Y14.5-2018.

Free download

Get the GD&T cheat sheet as a PDF.

The whole cheat sheet on a single page, drawn at poster scale so the symbols stay readable pinned above a desk.

Eleven geometric characteristics, each with its symbol, drawing callout, tolerance zone and inspection setup
Datums, degrees of freedom, and feature control frame anatomy read left to right
Material condition modifiers, basic dimensions, and a drawing checklist to sign off against

Get the free PDF

Downloading takes a free Drafter account. One account gets you every chart in the toolbox, plus the monthly newsletter, which you can leave from any issue in one click.

Cover of Drafter's GD&T Cheat Sheet, a printed reference page of geometric characteristic symbols on an orange ground.

Foundations

The vocabulary the rest of the sheet assumes: what GD&T controls, what it measures from, and how a control gets written down.

What GD&T controls

GD&T is a symbolic language used in engineering drawings to define the allowable variations in the geometry of parts and assemblies. GD&T controls four characteristics of your given part: size, location, orientation and form (SLOF).

Every characteristic further down this page is one of those four, or a combination of them. The label on each card says which, in the same color as its tag in the figure here.

Datums

Datums are theoretical axes, planes, or points used as fixed references for manufacturing and inspection. They are derived from datum features, the actual physical surfaces or features on the part.

The datum feature symbol shown here is how one gets named on a drawing: a letter in a box on a leader, with the filled triangle touching the surface the letter refers to.

Basic dimensions

The theoretically exact dimension used to define the size, location, or orientation of a feature. Basic dimensions are used to indicate distance or angles that are controlled by the GD&T symbol in a feature control frame.

The datum reference frame

Effective datums create a datum reference frame that can constrain up to 6 degrees of freedom (DOF). These are chosen based on features most critical to the part’s function.

Six is three translations and three rotations, one of each about X, Y and Z, which is what the three axes and three curved arrows in the diagram are counting off.

The order the datums are called in matters as much as which ones they are: each one takes away what the one before it left free, which is why a feature control frame reads its datums left to right.

Datum	What it typically constrains
Primary	Typically a surface or feature of size that constrains three or four degrees of freedom.
Secondary	Typically a secondary surface or feature of size that controls two more degrees of freedom.
Tertiary	Typically the final surface or feature, fully constraining all six degrees of freedom.

Feature of size

A part feature with a measurable dimension, like a hole, slot, pin, or tab, which can often be measured directly using calipers. It defines size limits, and form (if not further refined) of the feature. A feature of size is required to use MMC or LMC.

Rule 1: the envelope principle

The surfaces of a feature of size shall not extend beyond a boundary (envelope) of perfect form at maximum material condition (MMC). For example, a part at its largest size limit must be perfectly shaped, like a cylinder being round and straight at MMC, to ensure proper fit and function.

Point at, tap or tab to a part to read it.

Geometric characteristic symbol
Diameter symbol
0.075Tolerance
Material condition symbol
APrimary datum feature reference
BSecondary datum feature reference
CTertiary datum feature reference

Geometric characteristic symbol ⌖

Position: the feature's axis or center plane must lie in a zone centered on its true position, which basic dimensions locate from the datums.

ASME Y14.5-2018, paras. 6.3.1, 3.48 · Figs. 6-1 and 6-24

Diameter symbol ⌀

The zone is a cylinder and the value is its diameter; without the symbol the value would be the width between two parallel planes.

ASME Y14.5-2018, paras. 6.6, 6.3.7 · Fig. 6-24

Tolerance 0.075

0.075 mm: the size of the zone, its diameter.

ASME Y14.5-2018, paras. 6.4.1, 6.6 · Fig. 6-24

Material condition symbol Ⓜ

At MMC: the 0.075 mm holds at the maximum material size (the smallest hole, the largest pin), and the zone grows by however far the unrelated actual mating envelope departs from it.

ASME Y14.5-2018, paras. 5.9.4, 6.3.5 · Fig. 6-24

Primary datum feature reference A

Datum A comes first: the part is set against it before any other datum, so it constrains every degree of freedom its feature can.

ASME Y14.5-2018, paras. 6.4.3, 7.10 · Fig. 6-26

Secondary datum feature reference B

Datum B comes next: the part is set against it while keeping contact with A.

ASME Y14.5-2018, paras. 6.4.3, 7.10 · Fig. 6-26

Tertiary datum feature reference C

Datum C comes last: the part is set against it while keeping contact with A and B, and it takes what freedom is left.

ASME Y14.5-2018, paras. 6.4.3, 7.10 · Fig. 6-26

Reading a feature control frame

One frame, read left to right, is the whole instruction: which characteristic is controlled, how much of it is allowed, and what it is measured from. Every card in the sections below shows the same frame drawn onto a real part.

Not every compartment appears every time. A form characteristic references no datum at all, so its frame stops after the tolerance, and a material modifier only appears where the control applies to a feature of size. The diameter symbol in front of a tolerance is worth reading carefully: it says the zone is a cylinder rather than two parallel planes.

Compartment	What it specifies
Geometric symbol	Which of the eleven characteristics is being controlled.
Tolerance	How big the tolerance zone is, with a diameter symbol in front of it where the zone is cylindrical.
Material modifier	MMC or LMC, where the tolerance is allowed to grow as the feature departs from that condition. Needs a feature of size.
Primary datum	The first reference the feature is measured from.
Secondary datum	The second, constraining what the primary left free.
Tertiary datum	The third, constraining what is still left.

Point at, tap or tab to a part to read it.

Geometric characteristic symbol
Diameter symbol
Tolerance
Material condition symbol
APrimary datum feature reference
BSecondary datum feature reference
CTertiary datum feature reference

Both segments · Geometric characteristic symbol ⌖

Position: the feature's axis or center plane must lie in a zone centered on its true position, which basic dimensions locate from the datums. Entered once and shared by every segment (6.4.4).

ASME Y14.5-2018, paras. 6.3.1, 3.48, 6.4.4 · Figs. 6-1 and 6-24

Upper segment · Diameter symbol ⌀

The zone is a cylinder and the value is its diameter; without the symbol the value would be the width between two parallel planes. The upper segment locates the pattern as a group from its datums (10.5.1(a)).

ASME Y14.5-2018, paras. 6.6, 6.3.7, 10.5.1 · Fig. 6-24

Upper segment · Tolerance 0.085

0.085 mm: the size of the zone, its diameter. The upper segment locates the pattern as a group from its datums (10.5.1(a)).

ASME Y14.5-2018, paras. 6.4.1, 6.6, 10.5.1 · Fig. 6-24

Upper segment · Material condition symbol Ⓜ

At MMC: the 0.085 mm holds at the maximum material size (the smallest hole, the largest pin), and the zone grows by however far the unrelated actual mating envelope departs from it. The upper segment locates the pattern as a group from its datums (10.5.1(a)).

ASME Y14.5-2018, paras. 5.9.4, 6.3.5, 10.5.1 · Fig. 6-24

Upper segment · Primary datum feature reference A

Datum A comes first: the part is set against it before any other datum, so it constrains every degree of freedom its feature can. The upper segment locates the pattern as a group from its datums (10.5.1(a)).

ASME Y14.5-2018, paras. 6.4.3, 7.10, 10.5.1 · Fig. 6-26

Upper segment · Secondary datum feature reference B

Datum B comes next: the part is set against it while keeping contact with A. The upper segment locates the pattern as a group from its datums (10.5.1(a)).

ASME Y14.5-2018, paras. 6.4.3, 7.10, 10.5.1 · Fig. 6-26

Upper segment · Tertiary datum feature reference C

Datum C comes last: the part is set against it while keeping contact with A and B, and it takes what freedom is left. The upper segment locates the pattern as a group from its datums (10.5.1(a)).

ASME Y14.5-2018, paras. 6.4.3, 7.10, 10.5.1 · Fig. 6-26

Lower segment · Diameter symbol ⌀

The zone is a cylinder and the value is its diameter; without the symbol the value would be the width between two parallel planes. This lower segment relates the features to one another, its datums holding its zone in orientation only (10.5.1(b)).

ASME Y14.5-2018, paras. 6.6, 6.3.7, 10.5.1 · Fig. 6-24

Lower segment · Tolerance 0.025

0.025 mm: the size of the zone, its diameter. This lower segment relates the features to one another, its datums holding its zone in orientation only (10.5.1(b)).

ASME Y14.5-2018, paras. 6.4.1, 6.6, 10.5.1 · Fig. 6-24

Lower segment · Material condition symbol Ⓜ

At MMC: the 0.025 mm holds at the maximum material size (the smallest hole, the largest pin), and the zone grows by however far the unrelated actual mating envelope departs from it. This lower segment relates the features to one another, its datums holding its zone in orientation only (10.5.1(b)).

ASME Y14.5-2018, paras. 5.9.4, 6.3.5, 10.5.1 · Fig. 6-24

Lower segment · Primary datum feature reference A

Datum A, primary in this segment: it holds this lower segment's zones in orientation only, constraining their rotation and not their location, which the upper segment sets (10.5.1(b)(2), 10.5.1.8).

ASME Y14.5-2018, paras. 6.4.3, 10.5.1 · Fig. 6-26

Lower segment · Secondary datum feature reference B

Datum B, secondary in this segment: it holds this lower segment's zones in orientation only, constraining their rotation and not their location, which the upper segment sets (10.5.1(b)(2), 10.5.1.8).

ASME Y14.5-2018, paras. 6.4.3, 10.5.1 · Fig. 6-26

Composite control frames

One geometric symbol against two stacked segments. The upper segment locates the pattern; the lower one tightens how the features sit relative to each other without relocating them.

Segment	What it controls
Upper segment	Controls location and orientation between features. Constrains translation and rotational DOF around the datum reference frame.
Lower segment	Refines orientation between features. Constrains only rotation to the datum reference frame.

GD&T drawing checklist

Check items off as you go. Nothing here is saved: it resets the next time you open the page.

	Step	What to do
	Title block	Add and fill all relevant specifications and company information.
	Views	Place as few views as are required to show all critical features.
	Datum features	Identify all pertinent datums that orient and constrain the part in up to 6 DOF.
	Critical features	Add GD&T symbols and tolerances to all datums and features that require precise control.
	Basic dimensions	Apply dimensions to all critical features and datums.
	Defining critical information	Add any surface finishes, threaded holes, and so on.
	General notes	Add any critical information not represented in the drawings.

The characteristics

Eleven symbols, grouped by what they control. Each card opens to the drawing callout, the tolerance zone it creates, and how an inspector measures it.

Form

Shape on its own terms. None of these four reference a datum: they ask whether the feature is the shape it claims to be, wherever it happens to sit.

Flatness

⏥

FormMaterial modifier on a feature of size

Flatness in GD&T is a form tolerance that ensures a surface is flat without reference to a datum feature. The views below show surface control. Flatness can also apply to a feature of size, where the derived median plane is controlled.

Read the guide to flatness

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 para. 8.4.2). Drawn far wider than scale; drag to turn it.

How it is measured

Straightness

⏤

FormMaterial modifier on a feature of size

Straightness in GD&T is a form tolerance that can be applied to ensure either a surface remains uniformly linear or the axis of a feature remains straight. It can be called out on a surface feature or the axis of a cylindrical feature, depending on the specific application. The views below show surface control. Straightness can also apply to a feature of size, where the derived median line is controlled.

Read the guide to straightness

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 paras. 8.4.1, 8.4.1.1). Drawn far wider than scale; drag to turn it.

How it is measured

Circularity

○

FormNo material modifier

Circularity in GD&T is a form tolerance used to control how close a feature’s cross section is to a perfect circle. It applies to individual circular elements of a surface and is evaluated independently at each cross section, without reference to any datum.

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 para. 8.4.3). Drawn far wider than scale; drag to turn it.

How it is measured

Cylindricity

⌭

FormNo material modifier

Cylindricity in GD&T is a form tolerance used to control the overall shape of a cylindrical feature. It ensures the surface lies within two coaxial cylinders over the full length of the feature and is evaluated without reference to any datum. Cylindricity combines the requirements of circularity and straightness to control the overall form of a cylindrical feature.

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 para. 8.4.4). Drawn far wider than scale; drag to turn it.

How it is measured

Orientation

How a feature sits relative to a datum. All three take a datum reference, and all three control the form of a surface as a side effect of controlling its attitude.

Parallelism

∥

OrientationFormsurfaces onlyMaterial modifier on a feature of size

Parallelism in GD&T ensures that a referenced feature maintains a parallel orientation to a specified datum within a 3D tolerance zone. The views below show surface control. Parallelism can also apply to a feature of size, where the derived median plane or line is controlled.

Read the guide to parallelism

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 paras. 9.3.1, 9.3.2(a)). Drawn far wider than scale; drag to turn it.

How it is measured

Perpendicularity

⊥

OrientationFormsurfaces onlyMaterial modifier on a feature of size

Perpendicularity in GD&T is an orientation tolerance that ensures a surface or axis is at a 90 degree angle to a specified datum. It can be applied to control the perpendicularity of a surface feature or the axis of a cylindrical feature relative to a datum. The views below show surface control. Perpendicularity can also apply to a feature of size, where the derived median plane or line is controlled.

Read the guide to perpendicularity

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 paras. 9.3.1, 9.3.2(a)). Drawn far wider than scale; drag to turn it.

How it is measured

Angularity

∠

OrientationFormsurfaces onlyMaterial modifier on a feature of size

Angularity in GD&T is a symbol that defines the orientation of one feature relative to another at a specified angle within a 3D tolerance zone. The views below show surface control. Angularity can also apply to a feature of size, where the derived median plane or line is controlled.

Read the guide to angularity

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 paras. 9.3.1, 9.3.2(a)). Drawn far wider than scale; drag to turn it.

How it is measured

Profile

The one characteristic that can control size, form, orientation and location at once, which is why it stands in for several of the others on a curved surface.

Profile

⌓

SizeFormOrientationLocationNo material modifier

Profile in GD&T defines a 3D tolerance zone around a surface, ensuring that every point along the surface conforms to the specified profile tolerance within a given tolerance. Profile can be used with or without a datum reference frame present.

The views below show both profiles: profile of a surface, one zone around the whole surface, then profile of a line, the same offset curves judged one cross section at a time.

Read the guide to profile

How it is called out, what the zone is, how it is measured4 views

How it is called out

Profile of a surface: the tolerance zone, in 3D (ASME Y14.5-2018 paras. 11.2.1.1, 11.3, 11.3.1). Drawn far wider than scale; drag to turn it.

Profile of a line: the tolerance zone, in 3D (ASME Y14.5-2018 paras. 11.2.1.2, 11.3.1, 11.9). Drawn far wider than scale; drag to turn it.

How it is measured

Location

Where the feature actually is, against where the basic dimensions said it would be. This is the one you reach for on a hole pattern.

Position

⌖

OrientationFOS onlyLocationFOS onlyMaterial modifier on surfaces or a feature of size

Position in GD&T is a tolerance that defines the allowable deviation of a feature’s location from its nominal, exact position. While it is commonly applied to control the location of a feature of size, it can also be used to control the position of two surfaces relative to one another, depending on the application.

Read the guide to position

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 para. 10.3.3.1(b)). Drawn far wider than scale; drag to turn it.

How it is measured

Runout

What an indicator reads while the part turns on its datum axis. Circular runout judges one cross section at a time, total runout the whole surface at once.

Circular runout

↗

LocationFormNo material modifier

Circular runout is a GD&T tolerance that controls the cumulative variation of form and coaxiality as the part is rotated around a datum axis, ensuring a 2D cross section is within a specified tolerance zone.

Read the guide to circular runout

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 paras. 12.4.1, 12.4.1.1). Drawn far wider than scale; drag to turn it.

How it is measured

Total runout

⌰

LocationOrientationFormNo material modifier

Total runout is a GD&T tolerance that controls the cumulative variations of a surface’s shape, orientation, and position as the part is rotated 360 degrees around a datum axis, ensuring the entire surface remains within a specified tolerance zone.

Read the guide to total runout

How it is called out, what the zone is, how it is measured3 views

How it is called out

The tolerance zone, in 3D (ASME Y14.5-2018 paras. 12.4.2, 12.4.2.1). Drawn far wider than scale; drag to turn it.

How it is measured

Other common symbols

The modifiers and annotations that ride along with a characteristic rather than being one. Every symbol here is real text or a drawing, so you can copy it.

Symbol	Name	What it means
Ⓜ	Maximum material condition (MMC)	MMC is the condition in which a feature of size contains the maximum amount of material, such as the smallest hole size or largest shaft size within the specified tolerance. MMC ensures that parts will fit together even at their worst case tolerances, allowing for additional tolerance in other controlled features.
Ⓛ	Least material condition (LMC)	LMC is the condition in which a feature of size contains the least amount of material, such as the largest hole size or smallest shaft size within the specified tolerance. LMC ensures that parts maintain functionality, even when they contain the least material, providing additional tolerance for certain features.
	All around	All around indicates that a tolerance applies to surfaces all around the perimeter of the view shown.
	All over	All over indicates that a given callout applies all over the three dimensional profile of a part. It ensures uniform control across the entire part.
	Surface finish	Surface finish indicates the required texture or smoothness of a surface, specifying how rough or smooth a surface must be after manufacturing. It ensures the surface meets functional or aesthetic requirements.
CF	Continuous feature	Continuous feature is used to identify a group of two or more features of size or surfaces where there is a requirement that they will be treated geometrically as a single feature of size or surface.
↔	Between	Specifies the exact limits of the surface or line that the profile tolerance controls. It indicates that a tolerance or specification applies to a limited segment, or across multiple features. This will be used in conjunction with letter identifiers that indicate placement on the specified part.

A shop reference, not a standard. This page covers the basic definitions of essential GD&T terminology; for detailed explanations of more advanced concepts, or of geometric symbols used elsewhere such as concentricity and symmetry, refer to ASME Y14.5-2018 or the 2009 standard.

Free download

Print the GD&T sheet for the wall.

The whole cheat sheet on a single page, drawn at poster scale so the symbols stay readable pinned above a desk.

Eleven geometric characteristics, each with its symbol, drawing callout, tolerance zone and inspection setup
Datums, degrees of freedom, and feature control frame anatomy read left to right
Material condition modifiers, basic dimensions, and a drawing checklist to sign off against

Get the free PDF

Downloading takes a free Drafter account. One account gets you every chart in the toolbox, plus the monthly newsletter, which you can leave from any issue in one click.