Countersink vs Counterbore vs Spotface: Getting the Hole Callout Right

Three features sit on the same drawing and look almost identical in section: a cone, a flat-bottomed cylinder, and a shallow circular face. They are quoted differently, machined with different tools and inspected against different criteria. Getting the callout wrong on a print usually shows up later as a screw head standing proud of a surface, a fastener pulling a part out of flat, or a burr ring that fails incoming inspection.

This guide covers the three features, the screw standards that dictate their geometry, the tolerances that are worth putting a number on, and the ones that quietly add cost.

The three features, defined by what they hold

A countersink is a conical seat. It exists to accept a flat head screw so the head finishes flush with, or slightly below, the surrounding surface. The angle is fixed by the screw standard, not by preference.

A counterbore is a cylindrical recess with a flat bottom. It accepts a socket head cap screw, a button head, or a dowel so the fastener sits below the surface, and it leaves a flat annular face for the washer face of the head to clamp against.

A spotface is a very shallow counterbore, often only 0.5 to 1.5 mm deep. Its purpose is not to hide a fastener. It is to create a flat, perpendicular seating face on a rough surface — a casting skin, a forged boss, a laser-cut edge — so that a washer or a nut seats without rocking.

The distinction matters because the same word is used loosely in shops. "C'bore the M6" sometimes means a spotface for a washer. If the drawing does not show the depth and the intent, the shop will guess, and guesses go in the direction that is cheapest to machine rather than the direction the assembly needs.

The angle is not a design choice

Metric flat head screws to ISO 10642 are 90°. The older DIN 7991 flat head is also 90°. Inch-series flat head screws to ANSI B18.6.2 are 82°, with 100° appearing in some aerospace and flush-rivet standards.

A countersink cut at 82° for a 90° screw creates line contact instead of surface contact. The head seats on a narrow ring, the joint loosens under vibration, and the screw sits low or high by an amount that depends on how tight it was driven. On a painted or anodized part the contact ring also wears through the coating in service.

So the callout should name the standard, not just the angle: "90° csk to suit ISO 10642 M5" removes the ambiguity. A machinist reading "csk M5" will use whatever tool is in the holder, which is usually the metric 90° one, but not always.

Diameter matters too. A countersink whose major diameter is exactly the screw head diameter leaves a knife edge at the rim. The usual rule is to hold the major diameter to the head diameter plus 0.1 to 0.2 mm, which gives a small margin without widening the seat so much that the head sinks.

See also: Sheet Metal Fabrication Design Guide: 9 Rules That Cut Cost and Deburring Methods Compared: From Edge Break Callout to Media Choice.

Why countersinks chatter and counterbores do not

A countersink is a form tool cutting on its full cone at once. On stainless, titanium and any work-hardening alloy, a single-flute or zero-rake countersink will chatter, and chatter shows up as a faceted seat that leaks light when you check the head with marking compound. Multi-flute countersinks and slow spindle speeds with a firm feed are the usual fix, and rigid setup matters more than the tool.

A counterbore is cut with an end mill or a piloted tool, so it is an interrupted, controlled cut. It is slower to program but far more predictable in depth. That is why the counterbore is the feature to specify when the depth tolerance is tight.

Depth control is where most problems come from. A countersink's depth is a function of the cone angle and diameter, so depth and diameter cannot both be free. Tolerance only the diameter and let the depth follow; or tolerance the depth and accept the diameter that results.

Counterbore depth: nominal plus what?

A counterbore for a socket head cap screw needs enough depth for the head plus a small margin so the head never bottoms out. If the screw head is 5 mm tall, a 5.5 mm counterbore is adequate; a 6 mm counterbore wastes material and weakens the wall but is safe.

Hold depth to +0.1/−0 mm rather than a symmetric tolerance. Deeper is not dangerous for clearance, but it removes material that may be structurally useful and it moves the clamping face away from where the design assumed it was.

Two details that get left off prints and then argued about at inspection:

• Corner radius at the bottom. An end mill leaves its corner radius, typically 0.4 to 1.0 mm depending on tool. If the screw head has a sharp corner, it will not seat. Either specify a small undercut or accept the radius and check clearance.
• Concentricity to the through hole. A counterbore that is 0.2 mm off-centre on an M4 screw leaves a visible crescent gap and reduces the bearing area. Position tolerance on the counterbore should be tighter than the hole it surrounds, and it should be called out relative to the same datum.

Spotfaces: less material, more thought

On a casting, the as-cast surface is neither flat nor perpendicular to the hole. A nut or washer torqued against it bends, and the joint relaxes. A spotface restores a machined seat.

Two rules keep spotfaces cheap. First, keep the depth to the minimum that cleans up: 0.5 to 1.0 mm is often enough, and every extra millimetre is another roughing pass. Second, size the diameter to the washer or nut face plus 1 mm, not to the boss. A spotface that runs off the edge of a boss creates an interrupted cut and a burr exactly where the washer will sit.

On thin sheet metal there is no material to spotface. The alternative is a stamped or coined emboss, or a weld nut, and that decision belongs in the design rather than in the shop.

Cost and strength: choosing between them

A countersink removes material in a cone that is widest at the surface, which is the worst place to lose section on a part loaded in bending. A counterbore removes a cylinder, so the material loss is more localised and further from the neutral axis of a plate. When a print shows a countersink at the root of a bend or at the edge of a narrow flange, that is usually a sign the feature should be a counterbore, or moved.

Tolerances worth paying for, and ones that are not

Position tolerance on the hole: yes, this drives assembly. Diameter of the through hole: yes, this drives clearance and thread engagement. Counterbore depth: yes, in one direction only.

Countersink angle: no, it is set by the tool. Countersink depth as a separate dimension: no, it follows from the diameter. Surface finish inside the seat: rarely, unless the joint is sealed, in which case the seat and the screw both need a finish callout and a torque value.

One more: deburr. A countersunk hole breaks through into a through hole and leaves a fine burr at the intersection, invisible from outside and perfectly placed to damage an O-ring or a cable. Call the edge break, and see the note on deburring methods for how that callout should read.

A callout that survives the shop floor

The version that creates the fewest questions looks like this:

• "⌵ 90° × Ø10.4 to suit ISO 10642 M5, head flush ±0.1"
• "⌴ Ø11.0 × 6.0 +0.1/0, concentric to Ø5.5 within Ø0.1 A"
• "Spotface Ø16 × 1.0 min, perpendicular to A within 0.05"

Every one of those lines tells the machinist what tool to reach for, what to hold, and what the assembly actually needs. That is the whole job of a hole callout. Everything else — the number of flutes, the feed, the order of operations — belongs to the shop, and a print that leaves it there gets quoted lower.

Frequently asked questions

Can I use a countersink for a socket head cap screw? No. A socket head has a cylindrical side and a flat underside, so a conical seat gives it line contact on the corner and no clamping face. Use a counterbore. The only exception is a purpose-made screw with a matching conical underside, which is a different fastener.

How deep should a counterbore be for an M6 socket head screw? The head height for ISO 4762 M6 is 6 mm, so a 6.5 mm counterbore leaves 0.5 mm of clearance. Going to 7 mm is harmless for the fastener but removes material you may need; going to 6.0 mm exactly means any burr or paint film in the bottom will hold the head off its seat.

Does a countersink need a separate depth dimension? Not usually. If the angle is fixed at 90° and the major diameter is toleranced, the depth is determined. Adding a depth tolerance as well creates a conflict: the shop can satisfy one or the other, not both. Dimension the diameter and the flushness requirement.

What is the difference between a spotface and a counterbore? Depth and intent. A spotface is shallow, typically under 1.5 mm, and exists to create a flat seat on a rough surface. A counterbore is deep enough to swallow a fastener head and is dimensioned for that fastener. Mechanically they are the same cut with different tooling and different acceptance criteria.

Next step

If a hole callout has been causing assembly problems or a supplier keeps quoting the same feature two different ways, send the drawing. We will mark up the features that are ambiguous, say which ones are driving the price, and return a quote that separates the machining from the deburring so both are visible.

Written by the JSHS engineering team. The machining capabilities page covers the shop-side detail; if you would rather test a part against it, send the drawing and the reply comes from the engineer who would machine it.