Guide
Perpendicularity in GD&T vs angularity: which orientation control does a bore or face need?
Perpendicularity is the GD&T orientation control that holds a surface, axis or center plane inside a tolerance zone set at exactly 90° to a datum, while angularity does the same job at any other basic angle. Both use a zone of constant width rather than a range of degrees, and neither one controls where the feature sits.
By Saola Manufacturing engineering team · Published · Updated
This guide is about choosing between the two symbols on a milled part, usually a machined casting or block, and about what each choice does to inspection. The symbol chart, the datum theory and the coaxial controls are covered in other guides; here the focus is the practical decision for bores, faces and angled holes, the arithmetic that separates a GD&T zone from a plus-or-minus angle, and the drawing notes that keep a supplier from guessing.
On this page
What does each orientation control hold, and what does it leave free?
Both controls fix the tilt of a feature relative to a datum and nothing else: the zone may slide to wherever the feature actually is. Perpendicularity is the special case at 90°, angularity covers every other basic angle, and parallelism covers 0°.
Per ASME Y14.5-2018 and ISO 1101:2017, the shape of the zone depends on what the frame points at. Applied to a flat face, either control creates two parallel planes, a set distance apart, held at the stated angle to the datum. The whole face must lie between them, which means the callout also limits the flatness of that face to the same value. Applied to the axis of a bore or pin with a diameter sign in front of the value, the zone becomes a cylinder at the stated angle, and the axis must stay inside it. Without the diameter sign, an axis zone is two parallel planes, which controls tilt in one direction only.
Three things are deliberately left free. Location is not controlled: a perfectly square bore can still be in the wrong place, which is why bores that assemble normally carry a position callout as well. Size is not controlled: the diameter comes from its own dimension. And on an axis, form of the hole wall is not controlled: a bore can be barrel-shaped and still have a perfectly square axis. The GD&T symbols chart places these two symbols among the other ten if you need the wider picture.
One more difference matters on the print. Perpendicularity carries its angle implicitly; no 90° is written. Angularity needs the angle drawn as a basic dimension, in a box, because the tolerance belongs to the zone and not to the angle. A plain, unboxed 30° next to an angularity frame is an error a supplier will have to query.
How is perpendicularity GD&T different from a plus-or-minus angle tolerance?
A plus-or-minus angle creates a wedge-shaped zone that grows wider the farther you get from the vertex, while a perpendicularity or angularity zone has the same width along the whole feature. On a long face the GD&T zone is much tighter; on a short one the two can be close.
This is the single most useful fact for choosing a callout, and it is pure geometry. A linear zone of fixed width permits less tilt as the feature gets longer, so the allowed angle shrinks with length. A plus-or-minus angle permits the same tilt at any length, so the allowed deviation at the far end grows with length. The table works one example of each: a zone 0.05 mm wide, and an angle tolerance of plus or minus half a degree, across feature lengths typical of milled housings. Both are read the same way, as how far the far end of a straight feature may sit off nominal, to one side, relative to the end at the datum. For the fixed zone that offset equals the zone width at every length; the second column turns it into degrees, and the third column gives the same offset for the angle tolerance.
Read the columns together. At the shortest length the two callouts allow deviation of the same order, so a plain angle tolerance may be all a chamfer or a lead-in needs. At the longer lengths the angle tolerance lets the far end wander many times further than the GD&T zone, which is exactly the situation where a bearing bore, a guide face or a mounting pad needs perpendicularity instead.
| Length of the controlled feature (mm) | Tilt allowed by a 0.05 mm zone, to one side (degrees) | Far-end offset allowed by a half-degree angle tolerance, to one side (mm) |
|---|---|---|
| 10 | 0.286 | 0.087 |
| 25 | 0.115 | 0.218 |
| 50 | 0.057 | 0.436 |
| 100 | 0.029 | 0.873 |
What perpendicularity applies when the drawing gives no callout?
On an ASME drawing, an implied right angle is held only by the general angle tolerance in the title block. On an ISO drawing with a note such as ISO 2768-mK, the K class sets a default perpendicularity that grows with the length of the shorter side.
Per ASME Y14.5, lines drawn at right angles with no angle shown are implied 90° angles, and the general angular tolerance from the title block applies to them. That default is a plus-or-minus angle, so it has the wedge behavior shown above: loose on long faces. If a datum face and a mounting face must be square over a long span, put a perpendicularity frame on the drawing rather than trusting the title block.
ISO 2768-2:1989 gives general perpendicularity tolerances in three classes. The longer of the two sides forming the right angle is taken as the datum, and the length of the shorter side selects the row. The part has been withdrawn and replaced by ISO 22081:2021, but drawings in circulation still cite it, and the ISO 2768 and NADCA tolerance guide explains what that means for a new drawing.
| Shorter side length (mm) | Class H (mm) | Class K (mm) | Class L (mm) |
|---|---|---|---|
| up to 100 | 0.2 | 0.4 | 0.6 |
| over 100 up to 300 | 0.3 | 0.6 | 1 |
| over 300 up to 1000 | 0.4 | 0.8 | 1.5 |
| over 1000 up to 3000 | 0.5 | 1 | 2 |
Those defaults are generous for anything that carries a bearing or a seal. Treat them as the floor for non-functional corners, and call out every functional right angle explicitly.
When should a bore or face get perpendicularity, and when angularity?
Use perpendicularity whenever the design angle is 90°, which covers most bores, bosses and mounting faces on a milled part. Use angularity only for features that are genuinely inclined, such as an angled port, a tilted mounting pad or a drilled cross hole that is not square to its datum.
Within those two cases, the useful decisions are about the datum, the zone shape and the modifiers:
- Datum. Reference the face the part actually sits on or bolts down on in the assembly. A bearing bore made square to a cosmetic top face, rather than to the mounting flange, can pass inspection and still run tilted in the machine. On a casting, choose a datum face that gets machined; the guide to datums on cast parts covers that choice.
- Zone shape on an axis. Put the diameter sign in front of the value for a bore or pin that must be square in every direction. Leave it off only when tilt matters in one plane, such as a slot or a hole whose tilt along a rail is harmless.
- Material condition. A bore or pin that assembles with a mating pin or shaft can take the maximum material condition modifier, which adds bonus tolerance as the feature departs from its maximum material size (a hole grows, a pin shrinks) and allows a simple functional gauge. A bearing seat or a press fit should stay regardless of feature size. The MMC bonus tolerance guide works the arithmetic.
- Secondary datum on an angled hole. Angularity to a single datum plane only fixes the hole’s angle to that plane; the hole can still swing around the plane’s normal. If the direction of the incline matters, add a secondary datum that clocks it.
- Projected zone on a threaded hole. When a stud or a bolt shank sticks out of a tapped hole, its tilt matters above the part, not inside the thread. A projected tolerance zone handles that, and the threaded-hole position guide shows the callout.
A practical note: per ASME Y14.5, a position callout to a datum reference frame already controls the orientation of a hole to its primary datum within the position zone. A separate perpendicularity frame is only worth adding when it is tighter than the position value, as a refinement. A perpendicularity value equal to or larger than the position value adds nothing and invites a question.
How are perpendicularity and angularity measured?
Perpendicularity of a face is usually checked on a surface plate, with the datum face clamped to an angle plate or against a precision square and an indicator swept over the controlled face. Angularity uses the same idea with a sine bar or sine plate set to the basic angle, or a coordinate measuring machine.
The surface-plate methods turn an orientation check into a parallelism check. For perpendicularity, the datum face is held against a vertical reference and the total indicator movement across the controlled face is the error. For angularity, a sine bar is lifted on gauge blocks so that the controlled face, at its basic angle, comes out horizontal; the stack height is the sine of the angle times the length of the bar, so a typical 5 in sine bar set to 30° sits on a stack of 2.5000 in. The indicator reading across the face is then the angularity error. Gauge blocks, sine bars and indicators are only as good as their calibration chain; NIST’s page on metrological traceability explains what a traceable calibration means.
A bore axis cannot be touched directly, so it is simulated. On a bench, a gauge pin or an expanding mandrel that fills the bore is indicated at two heights. Remember to scale the reading: a reading taken over a pin that sticks far out of a short bore magnifies the deviation by the ratio of the reading span to the bore depth, while the tolerance applies over the length of the bore itself, so scale the reading back to bore depth. On a coordinate measuring machine, the axis is fitted from circles probed at two or more depths, and a short bore makes that fit sensitive, because a small error in each circle center becomes a large error in angle. For short bores, say on the drawing or the inspection plan how the axis is to be established.
Ask any supplier, in any country, how each frame will be verified and what the reading is scaled to. The answer tells you more than the name of the instrument does. The ballooned drawing and inspection report guide shows how each frame gets a line in the report.
Which callout mistakes cause rejected parts or arguments at inspection?
Most problems come from a missing or unusable datum, an unboxed angle on an angularity frame, a missing diameter sign on a bore, and a perpendicularity value that duplicates or contradicts a position callout. Each one either inflates the quote or leaves the result open to two readings.
- No datum, or the wrong one. An orientation frame without a datum letter is invalid under both ASME and ISO rules. A datum on a narrow chamfer, a drafted cast wall or a small boss gives an unstable setup, and two inspectors will get two answers.
- Angle not basic. A toleranced angle next to an angularity frame creates two competing controls. Box the angle and let the frame carry the tolerance.
- Missing diameter sign. Without it, the axis of a bore is only controlled in one direction, which is rarely what the designer meant.
- Angularity used for 90°. The symbol is not invalid at 90° under every standard and edition, but most readers expect the perpendicularity symbol there and will query the frame. Use perpendicularity for right angles.
- No edition named. “Per ASME Y14.5-2018” or “per ISO 1101:2017” in the title block settles which rules apply. The ASME versus ISO GPS guide covers where the two systems read the same frame differently.
- Orientation expected to fix location. A square bore in the wrong place is still in the wrong place. If the bore must also be located, add position.
What should the drawing and the RFQ say about orientation controls?
Name the standard and its edition, attach every orientation frame to a clearly identified feature and datum, and say which features actually locate, seal or carry load. With that, a supplier can plan the setups and the inspection before quoting.
A typical bore callout on a milled housing reads: perpendicularity symbol, diameter sign, value, datum A, with A the machined mounting face. A typical inclined port reads: angularity symbol, value, datums A and B, with the port angle shown as a boxed basic dimension. In the RFQ, add three things the drawing rarely shows: which features are functional, whether the values apply before or after any coating, and which frames you want reported with measured values rather than pass or fail.
At Saola, milled work is secondary machining on castings: datum faces machined, bores bored and reamed, and tapped holes cut, as described on the CNC milling page. That page also states what the plant does not do: we do not offer simultaneous five-axis machining, so a feature at a compound angle is something to flag in the RFQ. The CNC turning page says the same in its own terms: a lathe is the wrong tool for off-axis holes at odd compound angles, and parts that need heavy off-axis milling are routed to milling. On the inspection side, the quality page lists what you receive: a first-article report that measures every toleranced dimension on the drawing, and a dimensional record with each lot. If you mark an orientation callout as a process-capability control dimension, it is watched through the run rather than only at first article. Keep one datum scheme across the casting and machining drawings, as the milling page recommends, and send the package through the quote form. The RFQ preparation guide covers the rest of the drawing set.
Frequently asked
Does perpendicularity control flatness?
On a face, yes: the whole surface must lie between the two planes of the zone, so its flatness error cannot exceed the perpendicularity value. A separate flatness callout on the same face is only useful if it is tighter. On an axis, perpendicularity says nothing about the form of the hole wall.
Can angularity be used instead of a plus-or-minus angle on a chamfer?
It can, but it rarely earns its inspection cost. A chamfer or lead-in seldom does a job that depends on its exact tilt, and a general angle tolerance is easier to check. Reserve angularity for inclined faces and holes that locate or seal.
Is perpendicularity the same as squareness?
In shop language, yes, and older drawings use the word squareness. The GD&T term is perpendicularity, and it needs a datum and a zone value to mean anything measurable.
Can perpendicularity take the MMC modifier?
Only when it is applied to a feature of size, such as a bore, pin, slot or tab. On a plain face there is no size to depart from, so no material condition modifier applies.
Why does the same bore pass on one machine and fail on another?
Usually because the axis was established differently: a different datum setup, a pin of a different fit, or a coordinate fit from circles at different depths on a short bore. Agree the method on the inspection plan before first article.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018
- ISO 1101:2017, Geometrical product specifications (GPS) — Geometrical tolerancing, ISO, 2017
- ISO 2768-2:1989, General tolerances — Part 2: Geometrical tolerances, ISO, 1989 (withdrawn)
- Metrological traceability, NIST, accessed October 2026