What clearance hole size should an M3 to M24 or #2 to 1-inch bolt get: close, normal or loose fit?

What clearance hole size does each metric bolt get under ISO 273?

Per ISO 273, the normal (medium) clearance hole is 3.4 mm for M3, 4.5 mm for M4, 5.5 mm for M5, 6.6 mm for M6, 9 mm for M8 and 11 mm for M10. At every size the fine series is the smaller hole and the coarse series the larger one.

ISO 273 calls the three fits fine, medium and coarse; ASME B18.2.8, which also covers metric sizes from M1.6 to M100, calls the same three classes close, normal and loose. ISO 273 covers threads from 1 mm to 150 mm and ties its hole sizes to the bearing faces of ISO bolts and nuts, so the numbers were set with the head and nut in mind, not only the shank (ISO 273:1979). ISO lists the 1979 edition as reviewed and confirmed in 2024, so it is still the current edition. The standard also suggests a small chamfer on the hole edge where the underhead fillet of the bolt could otherwise bear on it. Each diameter in the table is a size found in ordinary metric drill ranges.

When should you use a close, normal or loose fit clearance hole?

Use normal fit by default, close fit only when the screw itself has to locate the parts or the head bearing area is marginal, and loose fit when parts are assembled with poor alignment or the hole pattern cannot be held tightly. The fit is a trade between how far the parts can shift and how much position tolerance the holes can be given.

Normal fit suits most bolted joints in machined housings, brackets and covers. It drills with a standard bit, leaves room for a plated or coated screw, and gives the hole pattern a workable position tolerance without reaming.

Close fit is chosen when a small shift between the mating parts matters and dowel pins are not practical, or when a socket head sits in a counterbore and the bearing face is already narrow. It costs position tolerance: in metric sizes up to M6 a close hole leaves only a few tenths of a millimeter between hole and screw, per ISO 273. Close fit is not a substitute for a dowel. A screw shank is not a precision locating feature, and the joint can still slip by the full clearance if it is overloaded in shear.

Loose fit is for parts that are assembled blind, for weldments and castings whose hole positions cannot be held well, and for patterns with many holes where the stack-up would otherwise force tight positions. The bigger hole shrinks the ring of metal under the head, so with a loose fit check the head or flange diameter against the hole and add a washer if the part is soft aluminum or a thin section.

When should a clearance hole become a slot?

Use a slot when the parts need adjustment during assembly, or when the hole spacing between two parts cannot be held because of thermal growth, welding distortion or a long pattern. A slot keeps the close or normal width across the slot and gives freedom only along it.

Make the slot width equal to the clearance hole you would otherwise have used, and dimension its length from the adjustment you actually need plus that width. Orient the slot along the direction of the error, typically radially from a datum hole or along the long axis of a pattern, so that one round hole locates the part and the slot only stops rotation. Tolerance a slot with position on its center plane in the narrow direction, and leave the long direction to a size tolerance. A slot in every hole of a pattern removes location altogether, so pair slots with at least one round hole or a dowel. Under the head, a slot carries the same bearing-area concern as a loose hole, and a washer is the usual answer.

Does a clearance hole need to be drilled, reamed or milled?

A clearance hole is normally drilled, because its size tolerance is wide: ISO 273 gives the tolerance classes H12, H13 and H14 for the fine, medium and coarse series (for information, where a tolerance is wanted), all of which a drilled hole typically holds without reaming. Reaming or boring only becomes worth paying for when the position tolerance, not the size, is tight.

The limits follow the ISO system of fits in ISO 286-1:2010: for example, an H13 hole of the M6 normal size has a tolerance of 0.22 mm, plus only. Large clearance holes beyond the drills on hand, or holes in thin walls where a drill would wander or burr badly, are often helically interpolated with an end mill instead. What a drilled hole holds and when a reamer is needed is covered in the drilled vs reamed hole tolerance guide.