How to Read a Hole Callout: Diameter, Depth, THRU and Patterns

The parts of a hole callout

Drawings describe most holes with a note on a leader rather than with separate dimensions, because one note can carry the count, the size, the depth and the treatment of the mouth. ASME Y14.5 sets out the symbols, and ISO 129-1 and ISO 15786 cover the ISO practice. Both build the note from the same pieces, read left to right:

Diameter and its tolerance

The diameter comes first after the count. Its tolerance follows in one of three forms. A fit class such as H7 points to ISO 286-2 for the deviations. Explicit deviations such as +0.015/0 give the limits directly. A ± value gives a symmetric band. A hole with no tolerance of its own takes the general tolerance from the title block. The limit dimensions calculator turns any of these into upper and lower limits.

A drawing may also state a drilling size, such as a tap drill note, which is a process instruction rather than a requirement on the finished part. When a note mixes the two, the finished-part value governs, and the process note is the shop's to follow or replace.

THRU and depth

THRU means the hole passes completely through the material. A blind hole carries a depth instead, with the depth symbol ↧ in ASME practice, or, in ISO practice, the depth after a × sign or with the same symbol. By ASME convention, the depth of a blind hole is the depth of its full diameter, measured from the surface where the hole starts. The cone left by a drill point is not part of that depth. When the drill point matters, the drawing shows its angle or dimensions it separately.

A callout with neither THRU nor a depth leaves the depth to the views. If a section or a hidden line shows the hole running through, the depth is defined. If no view shows it, the depth is missing and has to be asked for, never guessed from the scale of the drawing. The guide to missing dimensions covers how to ask.

Counterbores, countersinks and spotfaces

Counterbore (⌴)

A flat-bottomed enlargement at the mouth of a hole, sized by its diameter and depth, so a socket head sits at or below the surface. ⌴ Ø11 ↧6.8 on a Ø6.6 hole is one example.

Countersink (⌵)

A conical enlargement at the mouth, sized by its diameter at the surface and its included angle, for a countersunk head. ⌵ Ø12.4 × 90° is one example; the angle follows the screw head. The countersink calculator gives the depth that a diameter and an angle imply.

Spotface

A shallow counterbore that only cleans up a rough or curved surface so a washer or head sits flat. ASME marks it with SF inside the counterbore symbol. Its depth may be given, or the drawing may give the remaining thickness instead.

When a note stacks several of these, read it in order. The first diameter is the hole itself, and the treatments that follow apply at the surface the leader points to. A counterbore on the far side needs a view or a note that says so.

Counts and patterns

4X Ø6.6 THRU states four identical holes. The count does not locate them. Their positions come from dimensions or basic dimensions to each hole center, or from a pattern description such as equally spaced on a pitch circle diameter. On a bolt circle, check where the first hole is and which way the spacing runs. The bolt circle and hole pattern calculator turns a pitch circle and an angle into X and Y for every hole.

A position tolerance in a feature control frame under the callout applies to each hole of the pattern, relative to the datums it names. A count of holes that disagrees with what the views show is a conflict, not a typo to correct quietly.

A checklist for every hole callout