Clearance Hole Chart: Metric and Inch Drill Sizes (ISO 273 & ASME B18.2.8)

A clearance hole answers one question: should the bolt’s threads touch this part, or just pass through it? When the answer is ‘pass through,’ you drill the hole oversize so the fastener slides in without any thread engagement. The bolt then carries the joint as a clamp: head on one side, nut (or a threaded hole in the mating part) on the other, and the parts squeezed between them. Load travels through the clamped stack as friction and bearing, not through threads cut into the holed piece. This is the default arrangement for covers bolted to housings, plates bolted to frames, and any multi-part stack you expect to take apart again.

The opposite choice is the tapped hole, where the fastener’s threads cut into (or form in) the material itself and the hole size is a tap drill, not a clearance drill — for M6×1.0 that is 5.0 mm, not 6.6 mm. Confusing the two on a drawing is one of the classic shop-floor errors, because the difference between a tap drill and a clearance drill for the same fastener is more than a millimeter. Our thread sizes chart covers tap drills and thread dimensions; this page covers the clearance side. And if the bolt head must sit flush, the clearance hole gets a countersink or counterbore on top — see our guide to countersink holes for angles and diameters.

One practical note on how the hole is made: a standard twist drill produces a hole slightly over its nominal size, and the standardized clearance values in ISO 273 assume ordinary drilling accuracy. That is why the chart values are not round numbers — they are nominal bolt diameter plus a deliberate allowance, paired with a hole tolerance class that a drilled hole meets without reaming.

This is the complete metric clearance hole chart for the standard ISO 273 range used in machined parts. Read it by thread size, then pick the column for your fit class — medium (H13) unless you have a reason otherwise. The values are nominal hole diameters in millimeters; the tolerance class in parentheses is what the hole must hold, and ordinary drilling meets it. The M6 row deserves a highlight because it is the most queried: 6.4 mm fine, 6.6 mm medium, 7.0 mm coarse.

Note the pattern in the numbers: the medium series runs roughly 0.4 mm over nominal for small fasteners, 0.5 mm around M10–M12, and 1.0 mm or more past M18. That growing allowance is deliberate — larger bolts are used in larger fabrications where hole position tolerance is looser in absolute terms. If your hole size lands between chart values, always round up to the next standard drill rather than down; a hole that is slightly too big is a fit-class change, but a hole that is too small is a bolt that does not go in.

Reach for the loose/coarse class when the assembly environment is out of your control. The classic triggers: hot-dip galvanized or thickly coated fasteners (coating eats clearance), weldments and structural fabrications (hole positions move with heat), sheet-metal stacks (pierced holes vary), and field or maintenance assembly where technicians work with hand tools and no fixture. Loose fits also pair naturally with slotted holes when a part needs positional adjustment — oversized in one direction, and a slot in the other gives you controlled travel.

The costs are real, though. A loose hole gives up bolt-guided alignment, so if the bolt pattern positions the parts, you need dowel pins or a rabbet to do that job instead. Bearing stress under the bolt head and nut is unchanged, but the larger hole reduces the material ring carrying it — check washer coverage, especially in thin sheet, and specify washers when the hole is more than about one fit class oversize. In thin or soft materials, an oversized hole combined with high clamp load can pull the head through; a flanged fastener or a hardened washer fixes it. None of this is exotic — it is ordinary joint design — but it is the difference between a loose fit that saves assembly time and one that creates warranty calls.

On the drawing, put the fit class in the callout (‘Ø7.0 THRU, ISO 273 coarse’) rather than relying on the machinist to guess. Hole position tolerance matters as much as diameter here: a coarse hole with a sloppy position tolerance is just a bigger problem. Our CNC machining tolerances guide covers what position tolerances are realistic for drilled and bored holes.