GD&T

Why GD&T

Plus-and-minus tolerances say how big a feature can be, but not how flat, straight, square or well located it must be, or what it is measured from. Two inspectors can measure the same part differently and both be “right”. Geometric dimensioning and tolerancing (GD&T) is a symbolic language that fixes this: it states which surfaces are the references (datums), what shape each tolerance zone has, and how big it can be, based on how the part actually works.

Two standards are in common use. ASME Y14.5 (current edition 2018) is used mainly in North America. ISO GPS (geometrical product specifications, including ISO 1101 for the symbols) is used in Europe and much of the world. The symbols look almost identical, but some default rules differ, so always check which standard the drawing’s title block names. This page follows ASME Y14.5-2018 and notes where ISO differs.

Reading a feature control frame

Every geometric tolerance is written in a feature control frame: a row of boxes attached to the feature it controls. Read it left to right like a sentence.

• First box: the geometric characteristic (what is controlled).
• Second box: the tolerance. A ⌀ in front means the zone is a cylinder; without it, the zone is between two parallel lines or planes. A modifier such as Ⓜ (MMC) or Ⓛ (LMC) can follow.
• Remaining boxes: the datum references in order of priority: primary, secondary, tertiary. Form tolerances (flatness, straightness, circularity, cylindricity) never have datums.
• Basic dimensions are drawn in a rectangle (for example 25). They give the exact theoretical location or angle; the tolerance comes from the feature control frame, not from a ± on the dimension.

The geometric characteristics

There are 14 traditional symbols in five groups. ASME Y14.5-2018 removed concentricity and symmetry, leaving 12; ISO still uses them, and older ASME drawings may too.

Symbol	Characteristic	Group	Datum needed?	Controls
	Straightness	Form	No	A line on a surface, or an axis, is straight
	Flatness	Form	No	A surface lies between two parallel planes
	Circularity (roundness)	Form	No	Each cross-section of a round feature is round
	Cylindricity	Form	No	Roundness, straightness and taper of a whole cylinder together
	Profile of a line	Profile	Optional	Each cross-section of a surface follows its true profile
	Profile of a surface	Profile	Optional	A whole surface lies within a band around its true shape; very versatile
	Angularity	Orientation	Yes	A surface or axis is at the specified angle to a datum
	Perpendicularity	Orientation	Yes	A surface or axis is at 90° to a datum
	Parallelism	Orientation	Yes	A surface or axis is parallel to a datum
	Position	Location	Usually	A feature’s axis or center plane is at its true position; the most used control
	Concentricity	Location	Yes	Removed in ASME 2018 (use runout, position or profile). Still used in ISO
	Symmetry	Location	Yes	Removed in ASME 2018 (use position or profile). Still used in ISO
	Circular runout	Runout	Yes (axis)	Each circular element wobbles less than the tolerance as the part rotates
	Total runout	Runout	Yes (axis)	The whole surface wobbles less than the tolerance as the part rotates

Common modifiers

Symbol	Meaning
⌀	Diameter: the tolerance zone is a cylinder (S⌀ for a sphere)
Ⓜ	Maximum material condition: bonus tolerance as the feature departs from MMC
Ⓛ	Least material condition: bonus tolerance as the feature departs from LMC
Ⓟ	Projected tolerance zone: the zone extends above the part, used for tapped holes and pressed pins
Ⓕ	Free state: applies to a flexible part when not restrained
Ⓣ	Tangent plane: controls the plane touching the high points of a surface
Ⓤ	Unequally disposed profile: shifts a profile zone more to one side
Ⓔ	Envelope requirement (ISO): size limits also control form

Which control to use

Start from what the part has to do, then pick the weakest control that does it.

I need to control…	Use	Datum?	More
How flat a face is, for sealing or seating	Flatness	No	Form Tolerances
How straight a rod, rail or axis is	Straightness	No	Form Tolerances
How round a cross-section is, or a whole cylinder	Circularity or cylindricity	No	Form Tolerances
A face or axis square to a datum	Perpendicularity	Yes	Orientation Tolerances
A face or axis parallel to a datum	Parallelism	Yes	Orientation Tolerances
A face or axis at a set angle	Angularity	Yes	Orientation Tolerances
Where a hole, pin, slot or tab is	Position	Yes	Position and Location
A curved or free-form surface, or a surface’s location and shape together	Profile of a surface	Optional	Profile and Runout
A cross-section of a surface (a wing section, a cam)	Profile of a line	Optional	Profile and Runout
Wobble of a rotating part about its axis	Circular or total runout	Yes (axis)	Profile and Runout
Two diameters sharing an axis	Position, runout or profile (not concentricity in ASME 2018)	Yes	Position and Location

Datums

A datum is a theoretically perfect plane, axis or point that measurements start from. It is established by a real datum feature on the part, marked with a datum feature symbol: a capital letter in a box, attached to the surface with a filled triangle. Together, the primary, secondary and tertiary datums form a datum reference frame that locks the part in place in all six degrees of freedom. The full treatment, with datum targets and datum shift, is on the Datums and Datum Reference Frames page.

• Order matters. |A|B|C| and |B|A|C| describe different set-ups and can measure the same part differently. The primary datum should be the surface that seats the part in its assembly.
• Pick functional, accessible features: large, stable mating faces and locating bores, not small cosmetic edges.
• Datum features can be axes. A shaft or bore used as a datum gives an axis, which is how runout and coaxial position are defined.

Position and tolerance zones

With ± coordinates, a hole’s allowed area is a square. But a hole that is off by the same amount in any direction works equally well, so the natural zone is round. A position tolerance gives a cylindrical zone that just contains the old square: the same worst-case corner, with 57% more area. More good parts pass inspection, with no loss of function.

The actual position of a feature, measured as a diameter, comes from its x and y offsets from true position:

Actual position (⌀) = 2 × √( Δx² + Δy² )

MMC, LMC and bonus tolerance

Maximum material condition (MMC) is the size at which a feature contains the most material: the smallest hole or the largest pin. Least material condition (LMC) is the opposite: the largest hole or the smallest pin. With no modifier, a tolerance applies at any size (regardless of feature size, RFS), which has been the default in ASME since 1994.

Feature	MMC	LMC
Hole ⌀10.0–10.2	10.0 (smallest)	10.2 (largest)
Pin ⌀9.8–10.0	10.0 (largest)	9.8 (smallest)

When a position tolerance carries the Ⓜ modifier, every bit the feature departs from MMC is added to the tolerance as bonus tolerance. That is fair, because a bigger hole gives a mating pin more room to fit even if the hole is slightly out of place.

Use Ⓜ for clearance fits such as bolt patterns, where it makes parts cheaper without affecting assembly. Do not use it where the location matters at every size, such as press fits, bearings or features that align motion. Ⓛ is used to protect minimum wall thickness or edge distance.

Fastener formulas

These two formulas, from the ASME standard’s appendix, size position tolerances for bolted joints so that parts always assemble. H is the clearance hole size at MMC, F the fastener size at MMC, and T the position tolerance (diameter, at MMC).

Case	What it means	Formula
Floating fastener	Bolts pass through clearance holes in both parts and are held by nuts	T = H − F (for each part)
Fixed fastener	One part has tapped holes or press-fit studs; the other has clearance holes	T1 + T2 = H − F (shared between the parts)

Key terms

Term	Meaning
Feature	A physical part of the object: a surface, hole, pin, slot, edge or thread.
Feature of size	A feature with a size that can vary and two opposing parts: a hole, a pin, a slot or tab, a sphere. Size modifiers (MMC, LMC) only apply to these.
Datum, datum feature	The perfect reference, and the real feature that establishes it.
Basic dimension	An exact theoretical value in a box: it has no tolerance of its own.
Tolerance zone	The space (planes, cylinder, band) the feature must stay inside.
MMC / LMC / RFS	Most material, least material, and “regardless of feature size”. See the modifiers table above.
Bonus tolerance	Extra tolerance gained when a feature of size departs from MMC (or LMC), if the modifier is shown.
Virtual condition	The worst-case boundary created by a feature’s size and its geometric tolerance together; the size of the functional gage.
Rule #1 (envelope)	In ASME, a feature of size must have perfect form at MMC.
Feature control frame	The boxed tolerance statement: symbol, tolerance, modifiers and datum references.
Simulator	The gage, plate, pin or chuck that stands in for a datum during inspection.

ASME vs ISO

Topic	ASME Y14.5-2018	ISO GPS
Size and form	Rule #1 (envelope principle): a feature at MMC must have perfect form, so size limits also control form unless stated otherwise	Independency principle (ISO 8015): size and form are separate unless the envelope symbol Ⓔ is used
Concentricity and symmetry	Removed in 2018	Still available
Default material condition	RFS (no modifier needed)	Independent of size unless Ⓜ or Ⓛ is shown
Projection of drawings	Usually third-angle	Usually first-angle
Which applies?	Named in the title block or notes, e.g. “Interpret per ASME Y14.5-2018”	Named in the title block, e.g. “ISO 8015” or “Tolerancing ISO 8015”

The Rule #1 difference matters most in practice: an ISO drawing with only a ± size on a shaft does not limit how bent the shaft is, while the same drawing read under ASME does.

Tips for applying GD&T

• Start from function. Ask how the part locates in its assembly; those surfaces become the datums.
• Use position for holes and pins instead of ± coordinates, and add Ⓜ for clearance fits.
• Use profile of a surface for complex or cast shapes: one callout can control size, form, orientation and location.
• Use runout for rotating parts (shafts, pulleys, gears) where wobble matters.
• Flatness on mating faces stops rocking and leaks; perpendicularity on locating faces keeps assemblies square.
• Don’t over-tolerance. Tighter tolerances cost money in machining and inspection. Match tolerances to function and to what your process can hold; see Speeds and Feeds and CNC Machining for process notes.

Related

• Tap Drill Size and Thread Pitch Lookup
• Bolt Torque and Thread Engagement Tool (coming soon)
• Speeds and Feeds

FAQ

Do I need GD&T for hobby or 3D-printed parts?

Often not: simple parts made and fitted by the same person rarely need it. It becomes valuable when someone else makes or inspects the part, when parts must interchange, or when a few features (a bolt pattern, a bearing bore) really matter. Even then, a few position and flatness callouts usually do most of the work.

What is a basic dimension?

A dimension in a rectangle that states the exact theoretical size, location or angle. It has no tolerance of its own; the allowed variation comes from the feature control frame that refers to it.

Why does a position tolerance usually have a ⌀ symbol?

Because the tolerance zone for a hole or pin axis is a cylinder. Without ⌀, the zone would be two parallel planes, which only controls location in one direction.

What replaced concentricity in ASME 2018?

Use runout when you want to control the wobble of a rotating surface (it is also easy to measure), position for the location of a coaxial axis, or profile of a surface when form and location are controlled together.

Is MMC always a good idea?

Only for features where more clearance means easier assembly, such as clearance holes and loosely fitting pins. For press fits, precision bores or features that guide motion, leave the modifier off so the tolerance applies at every size.

References

• ASME Y14.5-2018, Dimensioning and Tolerancing (including the fixed and floating fastener appendix).
• ISO 1101:2017, Geometrical product specifications (GPS): Geometrical tolerancing; ISO 8015:2011, Fundamentals: concepts, principles and rules; ISO 2692, maximum and least material requirements.
• Mitutoyo, ASME Y14.5-2018 overview (changes from the 2009 edition).

Last reviewed: October 2026. This is an introduction, not a substitute for the standard; for production drawings, follow the edition named on the drawing.