Geometric Dimensioning & Tolerancing (GD&T)

A symbolic language for defining engineering tolerances on drawings. GD&T controls the form, orientation, location, and runout of features — not just their size. It communicates exactly how a part must be manufactured and inspected, eliminating ambiguity that leads to rejected parts.

Why GD&T Instead of ± Tolerances?

Plus-minus tolerancing controls size. GD&T controls geometry. For many parts, ± tolerances are sufficient. For others, they create ambiguity that increases cost and risk.

± Tolerancing Is Enough When	GD&T Is Necessary When
Simple rectangular or cylindrical parts with no critical mating surfaces	Bolt hole patterns where hole-to-hole position matters for assembly
Non-critical cosmetic or structural dimensions	Bearing bores, seal grooves, or press fits requiring form control (roundness, cylindricity)
Single-feature parts (one hole, one face)	Multiple datums required to define part orientation in the assembly
Prototypes where functional fit is still being refined	Rotating parts (shafts, spindles) where runout causes vibration
Parts assembled with adjustability (shims, set screws, slots)	Sealing surfaces where flatness directly determines leak-tightness

Cost Rule GD&T does not automatically increase cost. Specifying flatness 0.01mm on a surface that only needs 0.2mm is the real cost driver. GD&T lets you specify exactly what is needed — no more, no less. The problem is over-specifying, not GD&T itself. When used correctly, GD&T actually reduces disputes between design and manufacturing because the requirement is unambiguous.

Standards Reference ASME Y14.5-2018 (widely used in North America and global supply chains). ISO 1101:2017 (used in Europe and ISO-centric drawings). The symbols and concepts are nearly identical between the two standards. The differences are mainly in how certain modifiers and composite tolerances are applied.

The 14 Geometric Tolerance Symbols

GD&T defines 14 geometric characteristics organized into five categories. Form tolerances never require a datum. All others require at least one datum reference.

Symbol	Name	Category	Feature Type	Datum Required?	What It Controls	Practical Example
—	Straightness	Form	Line / Axis	No	How straight a line element or axis is	Guide rod must slide freely in a bushing
∩	Flatness	Form	Surface	No	All points on a surface lie between two parallel planes	Gasket mating surface, machine mounting face
ˆ	Circularity	Form	Surface	No	Cross-section lies between two concentric circles	Piston pin bore, bearing race
/	Cylindricity	Form	Surface	No	Entire cylindrical surface between two coaxial cylinders	Hydraulic cylinder bore, bearing seat
⊥	Perpendicularity	Orientation	Surface / Axis	Yes	Feature is 90° to a datum within tolerance zone	Hole perpendicular to mounting face for bolt assembly
∥	Parallelism	Orientation	Surface / Axis	Yes	Feature is parallel to a datum within tolerance zone	Two mating rails, opposite sides of a slot
∠	Angularity	Orientation	Surface / Axis	Yes	Feature is at a specified angle to a datum	Angled mounting surface, tapered bore
∅	Position	Location	Feature of Size	Yes	True position of a feature's center relative to datums	Bolt hole pattern, pin location
≅	Concentricity	Location	Feature of Size	Yes	Axis of a feature coincides with a datum axis	Bearing journal alignment (rarely used — runout preferred)
&sym;	Symmetry	Location	Feature of Size	Yes	Median plane of a feature coincides with datum median plane	Keyway slot centered on shaft axis (rarely used)
↗	Circular Runout	Runout	Surface	Yes	Total indicator reading at one cross-section during rotation	Shaft shoulder for bearing seating
↗	Total Runout	Runout	Surface	Yes	TIR across entire surface during rotation (controls cylindricity + circular runout)	Precision shaft, spindle journal
∩ with arc	Profile of a Line	Profile	Any	Optional	2D contour of a feature follows the true profile	CAM profile, complex 2D curve
∩ with line	Profile of a Surface	Profile	Any	Optional	3D surface follows the true profile within tolerance zone	Aero surface, mold cavity, complex 3D geometry

The Big Five for CNC Parts In practice, 80% of CNC parts use only five GD&T callouts: flatness, perpendicularity, position (with MMC), cylindricity, and runout. The remaining nine symbols are used for specialized requirements. Do not add GD&T callouts that the part does not functionally need.

Feature Control Frames

The feature control frame (FCF) is the standard method for specifying a geometric tolerance on a drawing. It is a rectangular box divided into compartments, read left to right. Every GD&T callout on a drawing uses this format.

Block	Content	Example	Notes
1st	Geometric characteristic symbol	⊥	Identifies which tolerance applies (straightness, flatness, position, etc.)
2nd	Tolerance zone shape + value + modifier	∅0.05 M	Diameter symbol (∅) for cylindrical zones, modifier (M/L) if applicable
3rd	Primary datum reference	A	The main reference feature
4th	Secondary datum (optional)	B	Constrains remaining degrees of freedom
5th	Tertiary datum (optional)	C	Fully constrains the feature

Reading an FCF


          ⊥ | ∅0.05 | A | B | M

"The axis of this hole must be perpendicular to datum A within a 0.05mm cylindrical tolerance zone, with datum B as secondary reference, at maximum material condition."

Reading a Simpler FCF


          ∩ | 0.02

"This surface must be flat within 0.02mm. No datum required." — Form tolerances never reference datums because they control the shape of a single feature, not its relationship to other features.

Datum Selection

Datums are the reference features from which all geometric tolerances are measured. They are marked on the drawing with a letter inside a diamond-shaped box, attached to the feature. Datum selection determines how the part is fixtured for machining and inspection — choose them based on how the part functions in the assembly.

Datum Hierarchy

Datum	Degrees of Freedom Constrained	Typical Feature	Selection Rule
Primary (A)	3 (one rotational, two translational)	Large flat surface, flange face	The surface the part rests on in the assembly. Must be the largest, most stable contact surface.
Secondary (B)	2 (one rotational, one translational)	Side face, edge, cylindrical surface	The surface that aligns the part laterally in the assembly. Must be perpendicular to datum A.
Tertiary (C)	1 (one translational)	Edge, pin hole, stop face	The surface that stops the part from moving along the remaining axis. Must be perpendicular to both A and B.

Datum Selection Rules

Rule	Explanation	Violation Example
Match the assembly	Choose datums based on how the part sits in the real assembly, not what is convenient for machining.	Selecting a machined surface as datum A when the part actually mounts on a cast surface in the assembly.
Largest contact surface first	Primary datum should be the largest, most stable surface that contacts the mating part.	Using a narrow edge as datum A instead of the large flange face.
Functional mating features	Datums should be surfaces that interface with mating parts in the assembly.	Using a non-mating cosmetic surface as datum A for a bolt hole pattern.
Consider manufacturing sequence	Choose datums that can be machined and measured in a single setup if possible.	Datum B is a surface only accessible after flipping the part, requiring a second setup.
Use features of size as datums for holes/shafts	When the critical relationship is between holes or between a hole and a shaft, use the hole/shaft axis as a datum.	Using an edge surface as datum when the real requirement is hole-to-hole concentricity.

Common Datum Mistake: Datum B Not Perpendicular to A The secondary datum must be perpendicular to the primary datum. If datum A is the bottom face, datum B must be a side face — not another face that is at an angle. If your part requires an angled reference, use angularity or a compound datum.

Modifiers: MMC, LMC, RFS

Material condition modifiers define how the geometric tolerance interacts with the feature's size. They determine whether the tolerance gets tighter, looser, or stays the same as the feature size changes. This directly affects cost because it changes how many parts pass inspection.

Modifier	Symbol	Meaning	Bonus Tolerance	Cost Impact	When to Use
Maximum Material Condition	M (in circle)	Feature contains the most material. Hole at smallest diameter, shaft at largest diameter.	Yes — tolerance increases as feature moves away from MMC	Lowers cost significantly. More parts pass inspection.	Bolt holes, clearance fits, locating pins — any feature where assembly matters and some deviation is acceptable.
Least Material Condition	L (in circle)	Feature contains the least material. Hole at largest diameter, shaft at smallest diameter.	Yes — tolerance increases as feature moves away from LMC	Moderate cost benefit. Useful for thin walls.	Minimum wall thickness control, fluid flow in bores, ensuring material is not removed beyond a limit.
Regardless of Feature Size	None (or S in circle in older ASME)	Tolerance applies regardless of the feature's actual size.	No bonus. Tolerance is fixed.	Higher cost. Fewer parts pass inspection.	Functional requirements that do not vary with size: sealing surfaces, critical alignment features, balance requirements.

MMC Bonus Tolerance Example

Bolt Hole Position with MMC


          ∅6.5 ±0.2 | Position | ∅0.4 M | A | B | C

Hole MMC = 6.3mm (smallest hole, most material left).
At MMC: positional tolerance = 0.4mm.
At LMC (6.7mm): positional tolerance = 0.4 + (6.7 − 6.3) = 0.8mm.
The larger the hole gets, the more positional tolerance you have. This means the hole drill can wander more and the part still passes — reducing scrap rate and cost.

Default is RFS (ASME Y14.5-2009 and later) If no modifier is specified, the default is Regardless of Feature Size (RFS) under current ASME standard. This means no bonus tolerance. Always specify M or L if you want bonus tolerance. Under ISO 1101, the default behavior is the same — tolerance applies regardless of size unless a modifier is shown.

Form Tolerances

Form tolerances control the shape of individual features. They never require a datum because they describe the feature itself, not its relationship to other features. Form tolerances are additive to size tolerances — the actual form error must fit within whatever space remains after the size tolerance is consumed.

Flatness

Property	Detail
Symbol	∩
Controls	All points on a surface lie between two parallel planes separated by the tolerance value
Datum	None
Typical Values	0.005mm (sealing surface) – 0.1mm (general mounting)
Common Application	Gasket surfaces, O-ring mating faces, machine mounting bases, precision tooling plates
Inspection	Surface plate + dial indicator, CMM scan of surface points, optical flat (for very tight tolerances)
Cost Note	0.01mm flatness on a 100mm surface is standard CNC. 0.005mm requires a light finishing pass. 0.001mm requires grinding.

Straightness

Property	Detail
Symbol	—
Controls	Line elements on a surface (surface straightness) or the axis of a cylindrical feature (derived median line straightness)
Datum	None
Typical Values	0.01mm – 0.05mm over the feature length
Common Application	Guide rods, shafts that slide in bushings, edge quality on long flat parts
Inspection	Straightedge + feeler gauge, CMM line scan, V-blocks with dial indicator
Cost Note	Axis straightness is more expensive to control than surface straightness because it requires the entire cylinder to be measured.

Circularity (Roundness)

Property	Detail
Symbol	ˆ
Controls	Each cross-section of a cylindrical or conical surface lies between two concentric circles
Datum	None
Typical Values	0.005mm (bearing bore) – 0.05mm (general shaft)
Common Application	Bearing races, piston pins, high-speed rotating shafts
Inspection	Roundness tester (V-block method or spindle method), CMM polar scan
Cost Note	Tight circularity (≤0.005mm) typically requires grinding or honing. Standard CNC turning achieves 0.01–0.02mm.

Cylindricity

Property	Detail
Symbol	/
Controls	Entire cylindrical surface lies between two coaxial cylinders. Combines circularity, straightness, and taper into a single control.
Datum	None
Typical Values	0.005mm (hydraulic bore) – 0.02mm (bearing seat)
Common Application	Hydraulic cylinder bores, precision bearing seats, pump barrels
Inspection	CMM (scan full cylinder surface), roundness tester at multiple cross-sections
Cost Note	Cylindricity is one of the most expensive form tolerances. It controls multiple error types simultaneously. If only roundness or straightness matters, specify those individually instead.

Do Not Specify Cylindricity When Position + Roundness Will Do Cylindricity is a composite control. For many bearing applications, specifying circularity (roundness) for the cross-section and position for the axis location achieves the same functional result at lower inspection cost.

Orientation Tolerances

Orientation tolerances control the angular relationship between a feature and one or more datums. They always require at least one datum reference. The tolerance zone is defined relative to the datum — not to an arbitrary angle on the part.

Perpendicularity

Property	Detail
Symbol	⊥
Controls	Feature is at 90° to the referenced datum within a tolerance zone (two parallel planes for surfaces, cylindrical zone for axes)
Datum	Required (at least one)
Typical Values	0.01mm (precision) – 0.05mm (general) per 25mm of height
Common Application	Holes drilled into a face, shoulder faces perpendicular to shaft axis, mounting faces
Inspection	Square / angle plate + dial indicator, CMM measured to datum plane, granite surface plate with height gauge
Cost Note	Perpendicularity of a hole to a face is controlled by machine accuracy. Standard 3-axis CNC achieves 0.02mm/25mm without special measures. Tighter values require boring or reaming.

Parallelism

Property	Detail
Symbol	∥
Controls	Feature is parallel to the referenced datum within a tolerance zone
Datum	Required (at least one)
Typical Values	0.01mm (sealing) – 0.05mm (general)
Common Application	Opposite faces of a slot, mating guide rails, bearing housing bores
Inspection	Surface plate + dial indicator, CMM comparison to datum
Cost Note	Parallelism is often controlled implicitly by flatness + thickness tolerance. Specify it explicitly when two features must be parallel to each other, not just individually flat.

Angularity

Property	Detail
Symbol	∠
Controls	Feature is at a specified angle (other than 90°) to the referenced datum
Datum	Required (at least one)
Typical Values	0.02mm – 0.1mm within the tolerance zone
Common Application	Angled mounting surfaces, tapered bores, chamfer angles on critical features
Inspection	Sine bar + dial indicator, CMM angular measurement, precision protractor with surface plate
Cost Note	Requires 4th or 5th axis machining for most angles. Cost increases with tighter angular tolerances because the rotary axis accuracy becomes the limiting factor.

Location Tolerances

Location tolerances control where a feature is relative to the datum reference frame. Position is by far the most commonly used location tolerance in CNC machining. Concentricity and symmetry exist in the standard but are rarely specified on modern drawings because runout and position can achieve the same functional result with simpler inspection.

Position Tolerance

Property	Detail
Symbol	∅
Controls	Location of a feature's true position (center point, axis, or center plane) relative to datums
Datum	Required
Typical Values	∅0.1mm (general) – ∅0.5mm (bolt holes) at MMC
Common Application	Bolt hole patterns, dowel pin locations, mating features between two parts
Inspection	Functional gage (go/no-go for MMC), CMM coordinate measurement
Cost Note	Position with MMC is the most cost-effective way to tolerance hole patterns. The bonus tolerance means more good parts pass. Always use MMC for clearance holes unless there is a specific reason not to.

Position Tolerance with MMC — The Standard for Bolt Holes


          4x ∅8.4 ±0.2 | Position | ∅0.4 M | A | B | C

Four M8 clearance holes, position tolerance 0.4mm at MMC. At MMC (8.2mm hole), positional tolerance is 0.4mm diameter. At LMC (8.6mm), bonus tolerance adds 0.4mm, giving 0.8mm total positional tolerance. A functional gage with 8.2mm pins at true position checks all four holes simultaneously — fast and cheap inspection for volume production.

Concentricity

Property	Detail
Symbol	≅
Controls	Median points of a feature's surface are aligned with the datum axis
Datum	Required
Common Application	Bearing journals where dynamic balance is critical
Inspection	Requires measuring median points — complex and expensive
Cost Note	Very expensive to inspect. Use runout instead in almost all cases. Runout controls the same functional requirement (surface coaxiality) but is much simpler to measure.

Symmetry

Property	Detail
Symbol	&sym;
Controls	Median plane of a feature is aligned with the datum median plane
Datum	Required
Common Application	Keyway slots, symmetric features
Inspection	Like concentricity — requires median point measurement, expensive
Cost Note	Rarely used in modern practice. Position tolerance applied to the slot width can achieve the same result with simpler inspection.

Avoid Concentricity and Symmetry Both require measurement of median points, which is complex and time-consuming. ASME Y14.5-2018 even de-emphasizes concentricity. Use runout for rotating parts and position for locating features. Reserve concentricity only for applications where dynamic balance demands control of the actual median axis, not just the surface.

Runout Tolerances

Runout tolerances control composite surface errors during rotation. They are measured by rotating the part around the datum axis and reading the total indicator reading (TIR). Runout is the go-to control for any part that rotates in service — shafts, spindles, pulleys, bearing journals.

Circular Runout

Property	Detail
Symbol	↗
Controls	TIR at a single cross-section. Detects circularity + coaxiality errors at that section only.
Datum	Required (datum axis)
Typical Values	0.005mm (precision bearing) – 0.02mm (general shaft)
Common Application	Shaft shoulders for bearing seating, O-ring grooves, flange faces
Inspection	V-blocks or centers + dial indicator. Rotate part, read TIR at one location.
Cost Note	Simple and inexpensive to measure. Standard equipment. No CMM required.

Total Runout

Property	Detail
Symbol	↗
Controls	TIR across the entire surface while the indicator moves axially. Controls circularity + cylindricity + coaxiality + taper simultaneously.
Datum	Required (datum axis)
Typical Values	0.005mm (precision spindle) – 0.03mm (general shaft)
Common Application	Precision shafts, spindle journals, long bearing seats, pump rotors
Inspection	V-blocks or centers + dial indicator. Rotate part while indicator sweeps along the full length of the feature.
Cost Note	More restrictive than circular runout. Harder to achieve and harder to inspect. Use only when the entire surface must be controlled, not just individual cross-sections.

Circular Runout vs Total Runout Decision Use circular runout when the surface only contacts the mating part at a narrow band (a bearing that sits against a shoulder). Use total runout when the entire cylindrical surface contacts the mating part (a bearing journal where the bearing slides along the full length).

GD&T Cost Impact

Geometric tolerances directly affect inspection cost and, for tight values, machining cost. The table below shows relative inspection complexity. Machining cost impact is included only for tolerances that require special processes (grinding, honing, boring).

Tolerance Type	Typical Value	Inspection Method	Relative Inspection Cost	Machining Cost Impact
Flatness (general)	0.02–0.05mm	Surface plate + dial indicator	Low	None (standard CNC)
Flatness (tight)	0.005–0.01mm	Optical flat / CMM	Medium	+10–20% (finishing pass or grinding)
Straightness (surface)	0.01–0.05mm	Straightedge + feeler gauge	Low	None (standard CNC)
Circularity	0.005–0.02mm	Roundness tester / CMM	Medium–High	+15–30% (grinding or honing for ≤0.005mm)
Cylindricity	0.005–0.02mm	CMM full surface scan	High	+20–40% (honing or grinding)
Perpendicularity	0.01–0.05mm	Angle plate + dial indicator / CMM	Low–Medium	None (standard CNC). Tighter: boring head required.
Parallelism	0.01–0.05mm	Surface plate + dial indicator	Low	None (standard CNC)
Angularity	0.02–0.1mm	Sine bar / CMM	Medium	+10–25% (4th/5th axis setup)
Position (MMC)	∅0.1–0.5mm M	Functional gage (go/no-go)	Low (gage) / Medium (CMM)	None (bonus tolerance helps)
Position (RFS)	∅0.05–0.2mm	CMM only	Medium–High	+5–15% (no bonus, tighter control)
Circular Runout	0.005–0.02mm	V-blocks + dial indicator	Low	+5–10% (between-centers turning preferred)
Total Runout	0.005–0.03mm	V-blocks + dial indicator (sweep)	Low–Medium	+10–25% (grinding for tight values)
Concentricity	0.005–0.02mm	CMM median point analysis	High	+15–30% (grinding, complex setup)
Profile of a Surface	0.02–0.1mm	CMM surface scan	High	+20–50% (5-axis or specialized tooling)

The Cumulative Cost Effect Each additional GD&T callout on a drawing adds inspection time. A part with flatness + perpendicularity + position + cylindricity + runout takes significantly longer to inspect than one with just position + flatness. Every callout should answer the question: "What happens if this feature is not controlled?" If the answer is "nothing significant," remove the callout.

Common Mistakes

#	Mistake	Why It Matters	Correct Approach
1	Applying GD&T to every feature	Each callout adds inspection time and cost. Over-controlled drawings are expensive to inspect and slow down production.	Apply GD&T only to features that need geometric control. Use ± tolerancing and ISO 2768 for everything else.
2	Forgetting the diameter symbol in position tolerances	Without the ∅ symbol, the tolerance zone is a square or rectangular area, not a circular one. A square zone rejects good parts that a circular zone would accept.	Always use ∅ before the tolerance value for position: ∅0.4, not 0.4.
3	Not specifying MMC when bonus tolerance is acceptable	RFS is the default under current ASME/ISO. Without the M modifier, there is no bonus tolerance — the positional tolerance is fixed regardless of feature size. This increases scrap rate.	Use MMC (M modifier) for clearance holes and locating features. Only use RFS for critical alignment that must not vary with size.
4	Datums that do not match the assembly	If the part is inspected against datums A-B-C but mounts in the assembly against different surfaces, a part that passes inspection may not fit in the assembly.	Choose datums based on how the part functions in the real assembly. The inspection fixture should replicate the assembly condition.
5	Specifying both flatness and parallelism on the same surface	Parallelism already controls flatness relative to a datum. Adding a separate flatness callout that is tighter than the parallelism value is redundant if it is looser.	Use flatness for a surface that must be flat regardless of other features. Use parallelism when the surface must be parallel to another surface. If you need both, specify the tighter value as flatness.
6	Using concentricity instead of runout	Concentricity requires measuring median points, which is complex and expensive. Runout measures the actual surface, which is what matters for rotating parts.	Use circular or total runout for rotating parts. Reserve concentricity for specialized dynamic balance applications.
7	Specifying form tolerances tighter than the size tolerance allows	A hole of 10.0 ±0.1mm cannot have circularity of 0.001mm. The form tolerance must fit within the size tolerance zone. Specifying an impossible form tolerance creates a conflict.	Form tolerance must always be less than the size tolerance. Rule of thumb: form tolerance ≤ 20–30% of the size tolerance for critical features.
8	Datum features that are too small or unstable	A narrow edge or small surface used as datum A will not provide stable fixturing. Inspection results will vary depending on how the part is set up.	Primary datum should be the largest, most stable surface available. If the functional surface is small, consider adding tooling holes for inspection fixturing.
9	Not accounting for datum shift with MMC modifiers on datums	When a datum feature is referenced at MMC, the datum reference frame can shift. This can result in parts passing inspection that would otherwise fail. If not intended, it leads to assembly problems.	Understand that datum M allows datum shift. Use datum M intentionally when the assembly allows it. Use datum RFS when the datum must be fixed.
10	Specifying GD&T without defining datums on the drawing	Tolerances that reference datums A, B, C are meaningless if those datums are not defined elsewhere on the drawing. The inspector has no reference to measure against.	Every datum letter used in an FCF must correspond to a datum feature symbol on the drawing. Ensure all datums are clearly identified.

← ISO 2768 & IT Grades

Fit Types →