Geometrical tolerances: the 14 ISO 1101 symbols and how to read them
Published October 2, 2026 — each symbol with its tolerance zone and whether it needs a datum, how to read the frame, the Ⓜ, Ⓔ, Ⓟ modifiers, and a converter between ± tolerances and position tolerance.
In short: ISO 1101 defines 14 geometrical characteristics in four families. Form tolerances (straightness, flatness, roundness, cylindricity) need no datum. Orientation (parallelism, perpendicularity, angularity), location (position, coaxiality, symmetry) and run-out tolerances are always measured from a datum (A, B, C). The two profiles (line and surface) can play either role.
1. The 14 ISO 1101 symbols and their tolerance zone
The tolerance zone is the space in which the actual feature must lie; t is the value written in the frame, in millimetres. When the value is preceded by Ø, the zone is cylindrical (or circular).
These tolerances are independent of size tolerances (ISO 8015 independency principle): a Ø 20 ± 0.1 dimension limits neither roundness nor axis straightness, unless the envelope requirement Ⓔ applies. Unstated form and orientation tolerances fall under the title-block general tolerance: see classes H, K, L in ISO 2768 general tolerances.
2. Reading a feature control frame
The frame reads left to right: the symbol, the tolerance value (with Ø if the zone is cylindrical and any modifiers), then the datums in order of precedence.
- ⌖ Ø 0.1: the hole axis must lie within a 0.1 mm diameter cylinder centred on its theoretically exact position.
- Ⓜ: the value applies at maximum material; it grows as the hole gets larger (see below).
- A, B, C: primary datum (the part rests on three points), secondary (two points), tertiary (one point). The order changes the result: it is not a list, it is a fixturing sequence.
- The theoretical position is given by boxed dimensions (theoretically exact), without tolerance: the frame carries the whole tolerance.
3. Modifiers
Ⓜ bonus example: a Ø 10 +0.2/0 hole carries a Ø 0.1 Ⓜ position. At maximum material (hole at Ø 10.0), the position tolerance is Ø 0.1. If the hole measures Ø 10.2, it becomes Ø 0.1 + 0.2 = Ø 0.3: the bolt still fits, and the shop scraps fewer good parts.
The envelope requirement Ⓔ is the natural companion of fits: Ø 20 H7 Ⓔ guarantees the mating shaft will enter, even if the bore is slightly oval. Choosing the fit itself is covered in the ISO 286 fit calculator.
4. Converter: ± tolerance and position tolerance
Enter the deviation in X and Y (a ± tolerance or a measured deviation from the theoretical position): the calculation gives the matching position diameter, 2·√(X² + Y²). Add the drawing's position tolerance to check conformity.
The second line gives the reverse: the square zone ± t / (2√2) that fits within Ø t. That is the classic trap when replacing ± dimensions with a position tolerance: for the same value, the cylindrical zone is 57 % larger in area than the square it contains, but it does not cover the corners of the ± t/2 square.
5. FAQ
What is the difference between flatness and parallelism?
Flatness is a form tolerance: it refers to nothing but the surface itself. Parallelism is an orientation tolerance relative to a datum; it also limits, as a side effect, the flatness of the toleranced surface.
What is the difference between coaxiality and concentricity?
They share the ◎ symbol in ISO 1101. Concentricity applies to a point (the centre of a circle in one section), coaxiality to an axis. The zone is a circle or a cylinder of diameter t centred on the datum.
How do you convert a ± tolerance into a position tolerance?
A square zone of ± x in X and Y has a half-diagonal of x√2: the equivalent position tolerance containing it is Ø 2√2·x, i.e. Ø 0.28 for ± 0.1. Conversely, a Ø t tolerance contains a square zone of ± t / (2√2), i.e. ± 0.035 for Ø 0.1.
What does Ⓜ mean in a feature control frame?
The maximum material requirement (ISO 2692): the stated tolerance applies at maximum material condition and grows by the departure from it. A Ø 10 +0.2/0 hole with a Ø 0.1 Ⓜ position accepts Ø 0.3 if it measures Ø 10.2.
Are ISO and ASME symbols the same?
Mostly, yes. But ASME Y14.5-2018 removed concentricity and symmetry, which ISO 1101 keeps, and the reading rules differ: ISO applies the independency principle by default (ISO 8015), ASME the envelope rule (Rule #1). A drawing must state which standard applies.