⟂ Perpendicularity
Perpendicularity · Orientación · ISO 1101 + ASME Y14.5
Example in plan
How to interpret it
The indicated axis or feature must be perpendicular to datum A within a cylindrical tolerance zone 0.05 mm in diameter: the whole real feature must fit inside that ideal cylinder set at 90° to the datum.
What controls
Controls that a feature (face, axis or median plane) is at 90° to the referenced datum. It is an orientation tolerance: it says nothing about the form of the feature itself (a face can be perfectly perpendicular on average and still not be flat, which is why flatness should also be specified where it applies). With ⌀ in front of the value, the tolerance zone is a cylinder around the theoretically perpendicular axis; without it, it is two parallel planes oriented at 90° to the datum.
How to verify
Rest the part on the datum (a table or surface plate that simulates it) and use a certified precision square together with feeler gauges to measure the gap at the top of the face being checked. With a dial indicator, mount a calibrated perpendicular stand on the datum and sweep the face: the variation in the reading is the perpendicularity error. On a CMM, the datum (plane or axis) is constructed first and the feature is evaluated relative to that reference frame, not relative to the machine table.
tolerance zone
Cylindrical zone around the axis theoretically perpendicular to the datum (with ⌀); without ⌀, two parallel planes at 90°.
Datums and notes
Requires at least a primary datum (plane or axis).
Workshop guideline values
- General
- 0.05–0.15 mm on squared seating faces in general machining.
- Accuracy
- 0.01–0.03 mm on fitted guideways or columns.
- High precision
- 0.005–0.01 mm on heads, spindles or master squares.
Guidance only: the drawing's value always wins.
Common mistakes when interpreting it
- Applying perpendicularity without first verifying the flatness of the datum itself: if the reference face is not flat, any 90° measurement taken from it is unreliable.
- Mistaking the value for an angular tolerance in degrees: it is always a linear distance (mm) defining the width of the zone, not a tolerance in minutes of arc.
How to get it in the workshop / if it comes out of tolerance
Very common on seating faces against a datum A. With ⌀ in front of the value, the tolerance zone is a cylinder around the theoretical perpendicular axis.
Before blaming the machine, clean and deburr the datum face: a burr or chip under the seating surface is enough to throw the 90° off measurably. Check the actual squareness of the head/table against a known master, especially after a crash or a spindle change. On a lathe, if you face the reference surface with a worn insert, it can come out concave/convex: take a skim pass with a fresh insert before the critical pass.
Related symbols
Other symbols in Orientation
See the full symbol libraryRelated tools
ISO fits
Calculates indicative ISO 286 tolerances for shaft and hole, H7/g6, H7/h6, H7/k6 and H7/p6 fits with clearance, transition and interference graph.
Inspection Plans
Upload a plan, extract dimensions and GD&T with AI and export your inspection guideline in PDF or CSV.
Shop trigonometry
Workshop trigonometry: right triangle, C chamfer, Z countersink, sine bar, taper and polar→X/Y for CNC operators.