Reference
GD&T symbols: the 14 geometric tolerances of ISO 1101, explained
Geometric tolerances limit how far the shape, orientation and location of a feature may depart from perfect geometry – independently of its size. ISO 1101 defines fourteen symbols in four groups: form, orientation, location and run-out. Here are all fourteen with what each controls, whether a datum is needed and how it is usually checked, followed by the feature control frame and its modifiers.
GD&T symbols chart
| Symbol | Characteristic | Group | Datum | Controls | Checked with |
|---|---|---|---|---|---|
| ⏤ | Straightness | Form | no | how far a line or an axis departs from a perfect straight line | straight edge and light gap, dial indicator on a surface plate, CMM |
| ⏥ | Flatness | Form | no | how far a surface departs from a perfect plane | surface plate with dial indicator in several directions, CMM |
| ○ | Circularity (roundness) | Form | no | how far a cross-section departs from a perfect circle | roundness tester; a dial indicator between centres shows run-out, not roundness |
| ⌭ | Cylindricity | Form | no | roundness, straightness and taper of a cylinder together, in one zone | roundness tester or CMM – a caliper cannot see it |
| ⌒ | Profile of a line | Form | optional | how far a line departs from its theoretically exact profile | CMM with nominal–actual comparison, optical comparator, form gauge |
| ⌓ | Profile of a surface | Form | optional | how far a surface – a free-form surface, say – departs from its theoretically exact profile | CMM or 3D scan compared with the CAD model |
| ⟂ | Perpendicularity | Orientation | required | how far a surface or axis departs from 90° to the datum | square with light gap, dial indicator on a square, CMM |
| ∠ | Angularity | Orientation | required | how far a surface or axis departs from a specified angle other than 90° to the datum | sine bar with dial indicator, CMM |
| ∥ | Parallelism | Orientation | required | how far a surface or axis departs from being parallel to the datum | dial indicator over the full length on a surface plate, CMM |
| ⌖ | Position (true position) | Location | optional | how far a feature's location – hole centre, axis, median plane – departs from its theoretically exact location, usually as a cylindrical zone Ø | CMM; with Ⓜ also a functional gauge; a caliper only approximates it |
| ◎ | Concentricity / coaxiality | Location | required | how far an axis departs from the datum axis | run-out tester between centres, CMM |
| ⌯ | Symmetry | Location | required | how far the median plane of a feature departs from the median plane of the datum | CMM; dial indicator on both sides on a surface plate |
| ↗ | Circular run-out | Run-out | required | the wobble when the part turns about the datum axis – in one cross-section (radial) or on a face (axial) | dial indicator on a run-out tester between centres or in a V-block |
| ⌰ | Total run-out | Run-out | required | run-out over the whole length or face – the indicator travels while the part turns | run-out tester with a guided indicator, CMM |
Two mix-ups turn up in inspection reports again and again: circularity (form, no datum) versus circular run-out (with a datum axis), and concentricity versus run-out. Run-out contains both roundness and coaxiality, which is why it is what a dial indicator between centres really shows. Whoever checks »circularity 0.02« with an indicator between centres is checking something other than the drawing asks for.
Form, orientation, location, run-out
A form tolerance looks at one feature on its own: how straight is the edge, how flat the face, how round the section? It needs no datum. The other three groups relate a feature to another one – parallel, square, in the right place, without wobble when turning – and therefore name a datum with a letter in the frame. Profile of a line or surface, and position, exist both with and without a datum.
The feature control frame, box by box
On the drawing each geometric tolerance sits in a rectangular frame with two to five compartments, attached by a leader to the toleranced feature:
- The symbol – which characteristic is meant (chart above).
- The tolerance value in millimetres, preceded by the shape of the zone: nothing for two parallel lines or planes, Ø for a cylindrical zone (usual for position and coaxiality), SØ for a sphere. An addition like 0.05/100 means per 100 mm of length. Modifiers may follow the value (below).
- The datums – one, two or three letters in the order in which they locate the part: primary, secondary, tertiary. A-B is a common datum made of two features.
| Symbol | Meaning |
|---|---|
| Ⓜ | Maximum material condition (MMC, maximum material requirement) |
| Ⓛ | Least material condition (LMC, least material requirement) |
| Ⓟ | Projected tolerance zone |
| Ⓕ | Free state |
| Ⓤ | Unequally disposed (offset) tolerance zone (UZ) |
| Ⓔ | Envelope requirement |
| Ⓢ | Regardless of feature size (RFS, ASME) |
| Ⓣ | Tangent plane |
| Ⓡ | Reciprocity requirement |
| Ⓐ | Derived feature |
| Ⓒ | Minimax (Chebyshev) associated feature |
| Ⓖ | Least squares (Gaussian) associated feature |
| Ⓝ | Minimum circumscribed associated feature |
| Ⓧ | Maximum inscribed associated feature |
| Ⓘ | Independency principle |
The two you meet most: Ⓜ, maximum material condition – the tolerance applies at the maximum material size and grows as the feature departs from it, which makes checking with a functional gauge possible (the true position calculator adds that bonus for you). And Ⓔ, the envelope requirement on a size – the feature may nowhere break through the envelope of its maximum material size, so the size also limits the form.
Datums and datum systems
The rules for datums are in ISO 5459. A datum is not the surface itself but the ideal feature fitted to it – the plane laid on the resting face, the axis fitted into the bore. Three datums in the right order form a datum system that removes every degree of freedom: the primary datum seats the part, the secondary aligns it, the tertiary stops it. The same order is the set-up for measuring – clamp the part differently from the frame and you measure a different tolerance.
Independency: size and form are two things
Under ISO 8015 size tolerances and geometric tolerances apply independently: a Ø20 h7 shaft may be bent as long as every local diameter is within size – unless the drawing couples the two, for example with the envelope requirement Ⓔ. Which standard applies is named in the title block; check it before you measure. The size limits of classes such as h7 are in the ISO 286 tolerance charts.
How a geometric tolerance goes into the inspection report
- One line per frame, with the balloon number, the frame as drawn (↗ 0.05 A), the tolerance as the upper limit and no lower limit – the deviation cannot be negative.
- The measured value is the deviation, not a size: 0.02 means »0.02 mm run-out measured«. The datum belongs in the line or the inspection plan.
- The gauge must be able to see the characteristic. A caliper sees no cylindricity and no position at MMC; run-out needs the datum axis between centres or in a V-block.
- Missing datum? An orientation, location or run-out frame without a datum is a drawing error – ask the customer before measuring, don't guess.
Frequently asked questions
What is the difference between form and location tolerances?
A form tolerance limits how far a single feature departs from its ideal shape – straightness, flatness, circularity, cylindricity, profile – and needs no datum. Orientation, location and run-out tolerances relate a feature to another one, so they need a datum.
How many GD&T symbols are there?
ISO 1101 has fourteen: six for form (straightness, flatness, circularity, cylindricity, profile of a line, profile of a surface), three for orientation (parallelism, perpendicularity, angularity), three for location (position, concentricity/coaxiality, symmetry) and two for run-out (circular and total run-out).
What does Ⓜ mean in a feature control frame?
Maximum material condition: the tolerance applies at the maximum material size and grows as the feature departs from it – a hole larger than its smallest limit, a pin smaller than its largest. That extra is the bonus tolerance, and it allows checking with a functional gauge.
What is the difference between circularity and circular run-out?
Circularity is a form tolerance without datum: how round is the cross-section? Circular run-out has a datum axis: how far does the surface wobble when the part turns about it? Run-out contains roundness and coaxiality together – it is what a dial indicator between centres actually shows.