The 14 Geometric Characteristics
ISO 1101 defines 14 geometric characteristics in four groups: form, profile, orientation, and location/run-out. The datum requirement and tolerance zone shape depend on the characteristic — details for each are shown below.
The surface must lie between two parallel planes separated by the tolerance value. Applied to a single flat surface — no datum needed, as it controls shape only.
No datum requiredA line on a surface, or an axis, must lie within a tolerance zone. For an axis: add Ø prefix for a cylindrical zone. Controls bow and curvature on shafts and cylindrical features.
No datum requiredEach circular cross-section of a cylindrical or conical surface must lie between two concentric circles. Measured at individual cross-sections independently.
No datum requiredThe entire cylindrical surface must lie between two coaxial cylinders. Controls circularity, straightness, and taper simultaneously — the most stringent single form control for a cylinder.
No datum requiredA 2D cross-section must lie within a zone bounded by two offset curves from the true profile. Without datums it controls form only; with datums it also controls location.
Datum: optionalA 3D surface must lie within a zone offset from the true profile. The most versatile control in GD&T — without datums it controls form; with datums it controls form, orientation, and location together. Essential for freeform and complex surfaces.
Datum: optional / required for locationA surface or axis must lie within a tolerance zone at a specified angle to a datum. The angle is always a basic (theoretically exact) dimension — never a toleranced angle.
Datum requiredA surface or axis must be within a tolerance zone exactly 90° to a datum. A special case of angularity. Using Ø creates a cylindrical zone — preferred for axes and boss alignments.
Datum requiredA surface or axis must lie within a tolerance zone parallel to a datum. Controls orientation only — not location. The feature can be any distance from the datum.
Datum requiredThe axis or median plane must lie within a cylindrical (Ø) or bi-directional zone at the theoretically exact basic position. Datum references are typically required to locate the position, but for a self-referencing pattern (e.g. a bolt circle toleranced relative to itself), the pattern may be specified without external datums.
Datum typically required; optional for self-referencing patternsThe median points (concentricity) or axis (coaxiality) of a feature must lie within a cylindrical zone coaxial to a datum axis. Difficult to measure directly — circular run-out is commonly used as a practical substitute.
Datum requiredThe median plane of a feature must lie within two parallel planes symmetrically disposed about a datum median plane. Used to ensure slots, tabs, and symmetric features are centred on a reference.
Datum requiredAt each individual cross-section, the surface deviation during one full rotation about the datum axis must not exceed the tolerance. Combines circularity and coaxiality control at each section. Practical and measurable with a standard dial gauge.
Datum required (axis of rotation)Over the entire surface length during full rotation, the surface must lie within two coaxial cylinders or parallel planes separated by the tolerance. Controls cylindricity and coaxiality simultaneously — more stringent than circular run-out.
Datum required (axis of rotation)True position typically requires datums to locate the tolerance zone in space. However, when a pattern of features (e.g. a bolt circle) is toleranced relative to itself — controlling the spacing between features within the pattern rather than their location relative to external datums — position can be applied without datum references. This is pattern tolerancing per ISO 5458. The individual feature-to-feature relationship is controlled, but the pattern as a whole is not located relative to the part.
Datum Reference Principles
Datums are theoretically exact geometric references — planes, axes, or points — derived from physical datum features on the part. ISO 5459 governs datum definition, datum reference frames, and datum targets. The datum reference frame constrains the part's degrees of freedom for measurement and inspection.
The concept of constraining degrees of freedom with an ordered set of datums (primary, secondary, tertiary) is common to both ISO 5459 and ASME Y14.5. However, the explicit "3-2-1" rule — naming the number of contact points per datum — is a term more associated with ASME Y14.5 and fixture design practice. ISO 5459 uses the concept of datum reference frames and degrees of freedom without formalising the 3-2-1 label. The underlying geometry is identical: a primary plane constrains 3 DOF, a secondary constrains 2, a tertiary constrains 1.
| Datum | Typical Feature | DOF Constrained | What it locks |
|---|---|---|---|
| Primary | Flat surface (plane) | 3 | Translation in Z, Rotation about X, Rotation about Y |
| Secondary | Edge surface or cylindrical axis | 2 | Translation in X or Y, Rotation about Z |
| Tertiary | Point or short edge | 1 | Remaining translation (X or Y) |
| Datum Feature | Simulated Datum | DOF Constrained | Typical Application |
|---|---|---|---|
| Flat surface | Plane | 3 (as primary) | Primary datum for prismatic parts — most common |
| Cylindrical OD or ID | Axis | 4 (as primary) | Shafts and bores — constrains 2 translations + 2 rotations |
| Width / slot / tab | Median plane | 2 (as secondary) | Centring reference for symmetric features |
| Cone / taper | Apex point + axis | 5 | Tapered shafts; complex fixture setups |
| Hole pattern | Pattern axis group | Varies | Pattern used as datum for locating mating features |
Always specify datums in order of functional importance — primary first. The primary datum represents the most critical functional contact surface (typically the largest and most stable). Reversing the order changes the part's orientation in the datum reference frame, which changes which tolerance zones apply and what passes or fails inspection.
When a datum feature is too large, too rough, or too flexible for reliable full surface contact, datum targets define specific points, lines, or areas on the part surface to contact instead. Indicated on drawings with a split circle: the identifier above the dividing line, the target area size below. Standard practice for castings, forgings, sheet metal stampings, and flexible weldments.
Material Condition Modifiers
Modifiers change how a geometric tolerance applies relative to the actual produced size of a feature. They are only applicable to features of size — holes, shafts, slots, and tabs. ISO 2692 governs the MMC and LMC principles. The modifier symbol is placed after the tolerance value inside the feature control frame.
The stated tolerance applies when the feature is at its maximum material size. As the feature departs from MMC toward LMC, a bonus tolerance equal to that departure is added to the stated tolerance. Used when assembly clearance is the design intent — most common modifier for hole patterns and fastener clearances.
The stated tolerance applies when the feature is at its minimum material size. Bonus tolerance available as the feature departs from LMC. Used to protect minimum wall thickness around holes, or to prevent breakout in thin-walled sections.
The tolerance applies at whatever size the feature is produced — no bonus tolerance is granted. This is the default condition in ISO 1101 when no modifier is shown in the feature control frame. Used for precision location controls and run-out where position error cannot be traded for size variation.
The tolerance zone is projected beyond the part surface into the space of the mating component. Used for threaded inserts and press-fit pins — the concern is how straight the fastener stands above the surface, not the angle of the hole itself. The projection height is specified alongside the modifier.
Adding the Ø prefix before the tolerance value changes the zone from two parallel planes to a cylinder. Applies to axes and positional controls. A cylindrical zone has 57% more area than a square zone of the same stated value and correctly reflects circular functional clearance — always use for hole and shaft position.
Multiple separate features share one common tolerance zone — all must collectively satisfy it. The CZ notation is specific to ISO 1101 and is used to indicate simultaneous requirements across a pattern. Conceptually equivalent to the simultaneous requirement rule or the lower segment of a composite position frame in ASME Y14.5.
Example: hole Ø10 H7 (limits: +0 / +0.021 mm), with a position tolerance of Ø0.1 at MMC referenced to datums A, B, C.
At MMC (smallest hole = Ø10.000 mm): position tolerance = Ø0.1 mm. At LMC (largest hole = Ø10.021 mm): position tolerance = Ø0.1 + 0.021 = Ø0.121 mm. The full size tolerance of the hole becomes available as bonus position tolerance. The functional mating condition — whether the pin clears the hole — is guaranteed at every combination of size and position within this envelope.
ISO 1101 vs ASME Y14.5
Both standards serve the same engineering purpose but differ on key defaults and fundamental principles. These differences can cause real inspection failures when drawings from one system are read using the rules of the other.
| Topic | ISO 1101 | ASME Y14.5 (2018) |
|---|---|---|
| Default material condition | RFS — implied when no modifier is shown | RFS — same (post-2009 revision) |
| Independency principle | Default: size and form are independent | Rule #1: Perfect form at MMC is required by default |
| Envelope requirement | Must be explicitly invoked by adding the envelope symbol to the size dimension | Applies automatically to all features of size — Rule #1 |
| Concentricity / Symmetry | Both defined and in active use in ISO 1101 | Both removed in the 2018 revision — replaced by Position or Run-Out |
| Unequal profile offset | UZ modifier specifies the unequal offset value | U modifier with the unequal value |
| Simultaneous requirements | CZ notation (Combined Zone) | Composite Feature Control Frame (two-tier FCF) |
| 3-2-1 datum terminology | Concept used but term not formalised — ISO 5459 uses "datum reference frame" and degrees of freedom | 3-2-1 rule explicitly described in ASME Y14.5 and widely used in US practice |
| Basic dimensions | Theoretically exact values in rectangular boxes | Theoretically exact values in rectangular boxes — same appearance |
| Drawing identification | "ISO 1101" noted in title block | "ASME Y14.5-2018" noted in title block |
ASME Rule #1 (Envelope Principle): A feature of size must not violate perfect form at MMC. A shaft dimensioned Ø20h6 must fit within a perfect cylinder of Ø20 mm — any form error is consumed within the size tolerance. No separate straightness or cylindricity callout is needed to enforce this boundary.
ISO Independency: By default, size and form are independent. The same shaft Ø20h6 can have straightness error exceeding its size tolerance unless a separate form control is added, or the envelope requirement symbol is explicitly shown next to the size dimension. This is the most common source of misinterpretation between the two systems, and a real-world inspection failure risk on drawings that do not clearly state which standard governs.
Tolerance Zone Shapes
The shape of the tolerance zone determines what passes and fails inspection. It is as important a design decision as the tolerance value itself.
| Zone Shape | How Specified | Applies to | Functional meaning |
|---|---|---|---|
| Two parallel planes | Tolerance value only — e.g. 0.1 | Surfaces, flatness, parallelism, orientation controls | Feature lies between two planes separated by the tolerance value. Default zone shape for surface controls. |
| Cylinder | Ø prefix before value — e.g. Ø 0.1 | Axes, position of holes and shafts, axis straightness | Axis must lie within a cylinder of the stated diameter. 57% more area than a square zone of the same value. |
| Two concentric circles | Value only, applied at each cross-section | Circularity, circular run-out | At each cross-section, the surface must lie within an annular zone of radial width equal to half the tolerance value. |
| Two coaxial cylinders | Value only, applied over the full surface length | Cylindricity, total run-out | The entire surface must lie between two coaxial cylinders with a radial separation of half the tolerance value. |
| 3D offset surface zone | Profile tolerance value only | Profile of a surface | The surface must lie within a 3D zone offset equally on both sides of the true profile by half the tolerance value. |
| Sphere | SØ prefix before value | Centre point of spherical features | The centre must lie within a sphere of the stated diameter. Rarely specified in practice. |
A square position tolerance zone of 0.2 × 0.2 mm accepts a diagonal axis error of up to Ø0.283 mm — but rejects a purely diagonal error of Ø0.210 mm, even though that error would functionally clear a mating pin. A cylindrical zone Ø0.2 mm is rotationally symmetric and directly corresponds to the pin-to-hole clearance. The cylindrical zone has 57% more usable area for the same stated tolerance value, eliminates the artificial corner-reject problem, and better represents functional assembly intent. Always specify Ø for hole and shaft position controls.