Counterbore vs countersink vs spotface: which hole feature should you call out, and how?

Counterbore vs countersink: when should you use each one?

Use a counterbore when the fastener has a cylindrical head that must sit flush or below the surface, use a countersink when the fastener has a conical head, and use a spotface when the head only needs a flat seat rather than a recess. The fastener you have already chosen decides the feature, not the other way around.

A counterbore suits socket head cap screws, shoulder screws and hex-head bolts with washers. The head bears on a flat annular face, so clamp load is carried squarely, and a cap screw keeps its full rated head strength, whereas metric hexagon socket countersunk screws to ISO 10642 are made with a reduced-loadability head. The cost is material: the part must be thick enough to bury the head and still leave a sound floor under it, and the recess needs room for a hex key or socket.

A countersink suits flat head (countersunk) screws, which give a smooth surface with nothing protruding. The cone also centers the screw in the hole, so a countersunk screw locates the part more than a cap screw in a clearance hole does. That self-centering is a drawback on a pattern of several screws: every cone tries to pull its own hole onto its screw, so small position errors turn into bending in the screws or a part that will not seat. Countersinks also take far less depth than a counterbore, which makes them the usual choice in thin plates and covers.

A spotface is not about hiding the head at all. It is the standard fix for a cast boss, a forged face or a curved surface where a bolt head would otherwise bear on one high point and either loosen or bend the bolt. It is typically cut only deep enough to clean up the surface, and it costs one short tool plunge.

• Flush or recessed cylindrical head: counterbore.
• Flush conical head, thin part, or smooth outer surface: countersink.
• Head or washer may stand proud, but the seat must be flat and square to the hole: spotface.
• Chamfer at a tapped or plain hole entry only: a countersink callout on that hole, not a separate feature.

How do you call out counterbore size and depth for a socket head cap screw?

Give the clearance hole diameter, then the counterbore diameter and depth, all taken from the screw’s head dimensions plus clearance. The counterbore diameter must clear the head and the wrench, and the depth must bury the head plus any washer and the flush tolerance you need.

A typical metric callout for an M6 socket head cap screw reads Ø6.6 THRU ⌴ Ø11 ↧ 6.4, and a typical inch callout for a 1/4-20 cap screw reads Ø.281 THRU ⌴ Ø.438 ↧ .265. The clearance hole comes from a clearance-hole table such as ISO 273 for metric or ASME B18.2.8 for inch fasteners. ISO 273 tabulates fine, medium and coarse series; B18.2.8 uses close, normal and loose fits. The head diameter and height come from ISO 4762 for metric cap screws and from ASME B18.3 for inch cap screws; the ASME scope notes that B18.3 itself includes an appendix of drill and counterbore sizes for socket head cap screws.

Three details decide whether the joint assembles. First, if a flat washer goes under the head, size the counterbore for the washer outside diameter, not the head. Second, if the screw is driven with a socket rather than a hex key, the counterbore must clear the socket wall, which is noticeably larger than the head. Third, a close-fit clearance hole needs a small edge break at its top, because the fillet under the screw head will otherwise bear on a sharp hole edge and the head will not seat on the counterbore floor.

Tolerance the counterbore loosely unless something else locates on it. A counterbore is a clearance feature: a plus tolerance on the diameter and a depth tolerance that keeps the head at or below the surface is enough. Tight counterbore tolerances add inspection time for no function.

How do you call out a spotface on a casting or a curved surface?

Give the spotface diameter and either its depth or the material thickness that must remain under it; if you give neither, ASME Y14.5 treats the spotface as the minimum depth needed to clean up to the full diameter. On castings, remaining thickness or a dimension from a datum is usually the safer choice because the as-cast surface moves from part to part.

A depth measured from a rough cast face is measured from a surface that varies, so two parts can pass the same depth callout with very different floor positions. Where the height of the seat matters for the assembly, dimension the spotface floor from a machined datum instead, and the depth becomes a result rather than a requirement. Our guide to setting datums on castings covers how to pick that datum.

Size the spotface diameter to the largest thing that bears on it, normally the washer or the flange of a flange nut, plus a little clearance. Then check that the cast boss is larger still. A spotface larger than its boss leaves a crescent of unmachined surface at one side, and the washer rocks on it. On the casting drawing, add machining stock on the boss face so the spotface always has metal to clean up.

A spotface on the far side of a part, where the tool cannot reach from the hole entry, is cut with a back-spotfacing tool that passes through the hole and cuts on the way out. Mark it “FAR SIDE” on the callout, and expect the shop to ask about the through hole diameter, because the tool body has to fit through it.

What should the drawing and RFQ say about counterbored and countersunk holes?

Name the fastener the hole serves, use one complete callout per hole feature, and say which seats are functional. With that information the machinist can pick standard tools and the inspector knows what to check.

• The fastener. “For M6 ISO 4762 SHCS with washer” or “for #10 82° flat head” next to the callout or in a note. It resolves most questions before they are asked.
• Standard tool sizes. Counterbore and countersink diameters that match standard counterbores and countersinks are cut in one plunge; odd sizes are interpolated with an end mill or need a special tool.
• Flush requirement. State flush, below flush within a stated amount, or “may protrude”. It is the real function of most recesses.
• Material and finish. Plating or anodizing builds on the countersink and the counterbore floor. If the head must be flush after finish, say whether the dimension applies before or after coating.
• Casting context. On a cast part, show the spotface on the machining drawing and the stock on the casting drawing.

The RFQ package guide lists everything else the drawing set should carry, and the thread callout guide covers the tapped holes that usually share the same part.