Orientation Tolerances

Orientation tolerances control how a feature is tilted relative to a datum: whether a face is square to the base, whether two surfaces are parallel, whether a face sits at the specified angle. They come after form tolerances in complexity because they always need at least one datum. This page covers perpendicularity, parallelism and angularity for surfaces and for axes, material condition and bonus tolerance on orientation, how orientation works together with position, and worked examples with the arithmetic. It is part of the GD&T guide and follows ASME Y14.5-2018.

What orientation tolerances do

Symbol	Characteristic	Zone	Orientation to the datum	Datum
	Perpendicularity	Two parallel planes t apart (or a cylinder ⌀t for an axis)	90° (square)	Required
	Parallelism	Two parallel planes t apart (or a cylinder ⌀t for an axis)	0° (parallel)	Required
	Angularity	Two parallel planes t apart at the basic angle	Any angle other than 0° or 90°, shown as a basic dimension	Required

• Orientation only. The zone is fixed in angle by the datum but free in position: it slides sideways to enclose the feature. Where the feature sits is limited by a size or location dimension, not by the orientation tolerance.
• It includes form. A face controlled for perpendicularity has to lie wholly within the two planes, so it also cannot be more wavy than t. A separate flatness tolerance can then only be smaller than the orientation tolerance, never larger.
• A datum is always required, and usually only the primary. The datum says what “square” or “parallel” is measured against. Adding a second datum to an orientation frame is rare.
• The angle is basic. For angularity the angle is drawn in a box (30°), so there is no ± on it. The tolerance comes from the frame alone. Any general angle tolerance in the title block does not apply to a basic angle.

Surfaces and axes

As with straightness, what the frame controls depends on where it is attached.

Frame attached to…	Feature controlled	Zone	Frame looks like
A surface (leader or extension line)	The whole surface	Two parallel planes t apart, oriented to the datum	| ⟂ | 0.05 | A |
The size dimension of a hole or pin	Its axis (derived median line)	A cylinder of diameter t, oriented to the datum	| ⟂ | ⌀0.1 | A | (the ⌀ gives the cylinder)
The size dimension of a slot or tab	Its center plane (derived median plane)	Two parallel planes t apart, centered on the feature	| ∥ | 0.05 | A |

One further option affects surfaces:

• Tangent plane Ⓣ. Written after the tolerance, it makes the control apply to the plane that touches the high points of the surface, instead of the whole surface. A bumpy surface can then pass an orientation control if its high points lie in a plane that is square or parallel, with the flatness of the surface limited separately. Use it for surfaces that mate along their high points (a flange face, a machined pad).

Perpendicularity

Perpendicularity is the control for “square”. The zone is two parallel planes t apart at 90° to the datum plane (for a surface), or a cylinder of diameter t at 90° to the datum (for an axis), or two planes for a center plane or an axis controlled in one direction only.

• A face square to a base (the vertical face of a bracket, the side of a block).
• A hole or boss square to a face: the axis lies in a cylinder of ⌀t whose own axis is perpendicular to the datum plane. With Ⓜ, the zone can grow as the feature leaves MMC (below).
• An axis square to an axis: a cross hole perpendicular to a bore, for example (datum is the bore’s axis).
• It is the tolerance form of an angle. A tolerance zone of t over a length L corresponds to a tilt of about t ÷ L. The table shows what a tolerance of 0.05 means as an angle:

Length of the feature	Tilt (t ÷ L)	In degrees	In arc-seconds
25 mm	2.00 mrad	0.1146°	413″
50 mm	1.00 mrad	0.0573°	206″
100 mm	0.50 mrad	0.0286°	103″
200 mm	0.25 mrad	0.0143°	52″

A longer face tolerates less tilt for the same zone: a 0.05 tolerance is about 0.11° over 25 mm but 0.014° over 200 mm. This is why a control that is easy on a small tab can be demanding on a long wall.

Parallelism

Parallelism is the control for “the same direction as the datum”. The zone is two parallel planes t apart and parallel to the datum plane, or a cylinder ⌀t parallel to a datum axis.

• The top of a plate parallel to its base. This controls tilt and flatness of the top, and combined with the thickness limits it controls how much the top can wander in height.
• A bore parallel to a mounting face or to another bore (gearbox shafts, a pair of parallel holes).
• A slot center plane parallel to an edge.
• Parallelism and thickness. The two surfaces of a plate are controlled in size by the thickness tolerance and in orientation by the parallelism tolerance. The parallelism tolerance should be smaller than the thickness tolerance, or the thickness tolerance alone already limits it (Rule #1, for a feature of size).

Example. A plate is 20.00 ±0.10 thick (19.90 to 20.10), with a parallelism of 0.05 on its top face to the bottom face (datum A). Local thickness at any point must stay between 19.90 and 20.10, and the top face must stay in a 0.05 band parallel to A. So if one end is 20.08 thick, the other end can be no thinner than 20.03 and no thicker than 20.10; without the parallelism control it could be anywhere down to 19.90, a 0.18 wedge.

Angularity

Angularity is the control for a face or axis at an angle other than 0° or 90°. The angle is a basic dimension (drawn in a box), and the zone is two parallel planes t apart tilted at that angle to the datum.

• The datum is the plane the angle is measured from. A surface at 30° to the base uses the base as datum A.
• The angle can be put on an axis too (a drilled hole at 15° to a face): the zone is a cylinder of ⌀t at the basic angle.
• Why basic, not ±. A ± angular tolerance gives a wedge-shaped zone that is narrower near the vertex and wider far from it. A basic angle with a tolerance zone of fixed width t gives the same tolerance anywhere along the face.

Checking an angle with a sine bar

A sine bar tilts a part to a known angle using a stack of gauge blocks of height h = L × sin θ, where L is the distance between the bar’s two rollers (100 mm or 200 mm are common) and θ the angle.

Angle	Gauge-block stack, 100 mm sine bar	Gauge-block stack, 200 mm sine bar
15°	25.882 mm	51.764 mm
30°	50.000 mm	100.000 mm
45°	70.711 mm	141.421 mm
60°	86.603 mm	173.205 mm

To check a surface at 30° with an angularity of 0.1: set a 100 mm sine bar on the surface plate with a 50.000 mm stack under one roller, clamp the part on the bar with the datum face down, and traverse a dial indicator along the angled surface. The indicator spread over the length of the surface must be no more than 0.1.

Features of size: MMC and bonus

When the controlled feature is a feature of size (a hole, pin, slot or tab), the orientation tolerance on its axis or center plane can use a material condition modifier. Ⓜ after the tolerance lets the tolerance grow as the feature moves away from its worst-case (MMC) size, because a feature that is not at its largest (pin) or smallest (hole) leaves clearance, and tilt that would have fouled at MMC no longer does.

Bonus tolerance = (actual size − MMC size) for a hole; (MMC size − actual size) for a pin

Total tolerance = stated tolerance + bonus

Virtual condition = MMC − tolerance (hole); MMC + tolerance (pin)

The virtual condition is the worst-case boundary the feature produces combined with its orientation error. It is the size of the gage pin (for a hole) or gage hole (for a pin) that must fit: for the hole above it is 10.0 − 0.1 = 9.9. Any hole whose real size and tilt let a ⌀9.9 pin go in, square to A, is good.

Actual hole size	Bonus	Allowed zone ⌀
10.00	0.00	0.10
10.05	0.05	0.15
10.10	0.10	0.20
10.20	0.20	0.30

For an external feature, for example a pin ⌀9.8 to 10.0 with perpendicularity ⌀0.05 at MMC, the virtual condition is 10.0 + 0.05 = 10.05 and a gage hole of ⌀10.05 square to A should accept the pin. Ⓛ (least material condition) works the other way and is used to protect a minimum wall thickness; Ⓜ and Ⓛ are covered with the other modifiers on the Modifiers and Material Conditions page.

Orientation and position together

A position tolerance controls where a feature’s axis is, and because its zone is fixed in angle by the datums, it also controls tilt: the axis cannot leave the zone, so it can be tilted only as far as the zone allows over the feature’s length. An orientation tolerance is the way to say “the position may be loose, but the squareness must be tight”.

• Position alone is enough when location and tilt are both about as critical as each other.
• Position plus orientation when a hole must be located within, say, ⌀0.5, but its axis must be square to the face within ⌀0.1 (a bearing bore, a hole that guides a pin, a thread for a screw that clamps). The orientation tolerance must be smaller than the position tolerance, or it adds nothing.
• Orientation alone when the location is toleranced in the normal way (± or loose position) and only the squareness matters.
• Position with a composite frame does the same job for a pattern: the lower segment of a composite frame is an orientation control for the pattern, with a tighter zone. It is covered with Position and Location.

Worked examples

Example 1: is the vertical face square enough?

A block sits on its base (datum A). A vertical face 80 mm high has a perpendicularity of 0.05 to A. An indicator on a height gauge is dragged up the face with the block standing against an angle plate. The face reads 0.000 at the bottom and +0.040 at the top, with no reading outside those two.

• The total spread of the indicator readings along the face is 0.040. Since the face never moves more than 0.040 across its height, it lies inside a band 0.040 wide that is square to A.
• 0.040 is less than 0.05: the face passes.
• Expressed as a tilt, 0.040 ÷ 80 = 0.50 mrad, or 0.0286°, about 103 arc-seconds.
• If the top had read +0.07, the spread of 0.070 would be greater than 0.05 and the face would fail, even though the part is only 0.05° out of square.

Example 2: a hole at MMC, with and without bonus

The hole of the figure above is ⌀10.0 to ⌀10.2, with perpendicularity ⌀0.1 at MMC to A, and is 30 mm deep. The part is measured: the hole’s actual size is ⌀10.07 and its axis is out of square by 0.14 (a ⌀0.14 zone) over the 30 mm depth.

• Bonus = 10.07 − 10.0 = 0.07.
• Total tolerance = 0.1 + 0.07 = ⌀0.17.
• Measured ⌀0.14 is less than ⌀0.17: the hole passes.
• Without the Ⓜ, the tolerance would be a fixed ⌀0.1 and the same hole would fail (0.14 > 0.1). The modifier turns a rejection into a pass when the extra clearance really is available.
• As an angle, the 0.14 zone over 30 mm is a tilt of 0.14 ÷ 30 = 4.67 mrad (0.267°).

Example 3: a 30° face

A wedge-shaped block rests on its base (datum A). Its sloping face is drawn at 30° (basic) to A with an angularity of 0.1. Using a 100 mm sine bar:

• Stack height = 100 × sin 30° = 100 × 0.5 = 50.000 mm.
• The block is clamped on the sine bar so that the sloping face is nominally level. A dial indicator is run along the face and the readings range from −0.03 to +0.04.
• Spread = 0.04 − (−0.03) = 0.07, less than 0.1: the face passes.
• If the drawing had said 30° ±0.5° instead, the face could be as far out as 100 × tan 0.5° = 0.87 mm over a 100 mm length. A basic 30° with a 0.1 zone is a far tighter and more clearly defined requirement.

Example 4: parallelism of two bores

A gearbox housing has two bores 150 mm apart. Bore B is the datum (axis). Bore C has a parallelism of ⌀0.05 to B over a 60 mm length. The tilt this allows is 0.05 ÷ 60 = 0.83 mrad (0.048°): at the other end of a 60 mm bearing the axes can be 0.05 apart in any direction. For a pair of meshing gears this is the misalignment that decides contact pattern and noise, which is why gearbox bores are one of the main places that orientation controls are used.

Troubleshooting

Symptom	Likely cause	Try
A part fails perpendicularity but the surface is flat	It is square only after a different datum is chosen: the datum surface is not truly flat or is rocking	Check the datum feature’s flatness and how the part sits; use a larger or better datum
A cross hole is not square to its bore	Drill wander, an angled start, or a long drill that deflects	Pilot drill, use a drill bushing or a jig, ream or bore to correct
Good parts fail in a fixed gage	The drawing says Ⓜ but the gage was made for RFS, or the reverse	Make the gage to the virtual condition and check which modifier the drawing calls
Inspector measures with the wrong datum	The datum letter is missing or the datum feature is hard to see	Mark datum features clearly and put the datum in every orientation frame
Orientation tolerance is larger than the position tolerance	The position zone already limits tilt, so the orientation control does nothing	Make the orientation tolerance smaller, or drop it
A long tab will not hold perpendicularity	The same angular error gives a larger error over a longer length	Tighten the control on the feature, shorten it, or locate it with a second datum or a better set-up

Related

• GD&T: the overview, symbols and a quick reference to the 14 characteristics.
• Datums and Datum Reference Frames: the references that orientation is measured from.
• Form Tolerances: the controls that need no datum and are contained in orientation.
• Position and Location: where a feature is, and how composite frames refine its orientation.
• Modifiers and Material Conditions: MMC, LMC, virtual condition and the tangent plane in detail.
• Bolt Torque & Thread Engagement Tool: threaded holes and the perpendicularity they need.

FAQ

Is perpendicularity the same as squareness?

Yes, in everyday language. In GD&T it means the surface or axis lies within a zone that is exactly 90° to the datum, with a width you choose. It is a tolerance, not a ± angle.

Do I always need a datum for orientation?

Yes. The datum is what “square”, “parallel” or “at 30°” is measured against. A tolerance with no datum would be a form tolerance.

Does a perpendicularity tolerance control flatness?

Yes, indirectly. The whole surface must lie within the two planes of the zone, so it cannot be more uneven than t. A flatness control, if you add one, must be smaller than the orientation tolerance.

What is the difference between perpendicularity and position of a hole?

Position locates the axis in space (and so limits tilt over the length); perpendicularity only controls the angle of the axis to a datum and not where it is. Use position for “where” and perpendicularity for “how square”, and combine them when both matter.

Why is the angle in a box?

A boxed angle is basic: it is theoretically exact. The permitted variation comes from the angularity frame, not from a ± on the angle, which gives a zone of constant width.

What does the tangent plane symbol do?

It applies the orientation control to the plane that touches the high points of the surface, not to the whole bumpy surface. It is useful for surfaces that mate on their high points.

Can orientation use MMC on a surface?

No. Material condition modifiers apply only to features of size (holes, pins, slots, tabs), because they depend on the size of the feature. A plain surface has no size, so there is nothing to give bonus tolerance.

How do I convert an orientation tolerance to an angle?

Divide the tolerance by the length: angle ≈ t ÷ L in radians (multiply by 57.3 for degrees). A tolerance of 0.05 over 50 mm is 0.001 rad, or 0.057°.

References

• ASME Y14.5-2018, Dimensioning and Tolerancing (orientation tolerances, tangent plane and material condition modifiers).
• ASME Y14.5.1M, Mathematical Definition of Dimensioning and Tolerancing Principles.
• ISO 1101, Geometrical product specifications (GPS): Geometrical tolerancing: Tolerances of form, orientation, location and run-out.
• ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures (gages at virtual condition).
• Oberg et al., Machinery’s Handbook, Industrial Press (sine bars and angle measurement).
• Krulikowski, A., Fundamentals of Geometric Dimensioning and Tolerancing, Cengage.

Last reviewed: October 2026. Worked values are examples; check the standard your drawing names for rules and symbols.