Countersink Depth Calculator
How deep to cut a countersink so a flat head screw lands flush: enter your screw size or raw diameters and get the exact depth from the shop formula D = (OD − ID) / (2 × tan(θ/2)), with metric and imperial screw tables, six standard angles, a truncated-tool mode, and a depth-stop setup guide. 100% client-side.
For countersinks or spot drills whose tip is truncated (flat) instead of a sharp point: tool travel from the surface is Z = (D − T) / (2 × tan(α/2)) + a, where T is the flat tip diameter and a is the truncation allowance.
The countersink depth formula
D is the depth of the conical cut measured from the workpiece surface. OD is the head diameter — the diameter of the cone's mouth at the surface. ID is the pilot-hole diameter the cone grows out of (normally the screw's clearance hole). θ is the included angle of the countersink tool.
Why subtract the hole first? The cone only spans the ring between the hole edge and the head edge, so only that radial difference gets converted into depth by the cone's slope. And why does a sharper cone cut shallower? Because depth = radial difference × 1 / (2 × tan(θ/2)): a larger θ gives a larger tangent and a smaller depth. For a 90° tool the factor is exactly 0.5, so the depth is half the diameter difference.
Worked example 1: M6 flat head screw, 90°
- Look up the screw: an ISO 7046 flat head M6 has a head diameter of 11.3 mm; the normal-fit clearance hole is 6.6 mm.
- Pick the angle: metric flat heads seat in a 90° countersink.
- Apply the formula: D = (11.3 − 6.6) / (2 × tan(90°/2)) = 4.7 / (2 × tan 45°) = 4.7 / 2 = 2.35 mm.
- Target flush, not proud: add 0.15 mm so the head lands just below the surface → set the depth stop to 2.50 mm, then verify on a scrap offcut.
Worked example 2: #10 flat head screw, 82°
- Look up the screw: an ASME B18.6.3 #10 flat head has a head diameter of 0.385 in; the normal clearance hole is 0.201 in.
- Pick the angle: imperial flat heads seat in an 82° countersink.
- Apply the formula: D = (0.385 − 0.201) / (2 × tan(82°/2)) = 0.184 / (2 × tan 41°) = 0.184 / 1.73857 = 0.1058 in.
- In millimetres: 0.1058 × 25.4 = 2.69 mm — switch the unit toggle to mm and the calculator shows both.
Metric flat head screw table (ISO 7046, 90°)
| Thread | Head Ø (mm) | Clearance hole (mm) | Depth @ 82° | Depth @ 90° | Depth @ 100° |
|---|---|---|---|---|---|
| M3 | 5.5 | 3.4 | 1.21 | 1.05 | 0.88 |
| M4 | 8.4 | 4.5 | 2.24 | 1.95 | 1.64 |
| M5 | 9.3 | 5.5 | 2.19 | 1.90 | 1.59 |
| M6 | 11.3 | 6.6 | 2.70 | 2.35 | 1.97 |
| M8 | 15.8 | 9.0 | 3.91 | 3.40 | 2.85 |
| M10 | 18.3 | 11.0 | 4.20 | 3.65 | 3.06 |
Head diameters are the ISO 7046-1 maximum head diameter; clearance holes are the ISO 273 normal (medium) series. Depths are computed with D = (head − hole) / (2 × tan(θ/2)).
Imperial flat head screw table (ASME B18.6.3, 82°)
| Screw | Head Ø (in / mm) | Clearance hole (in) | Depth @ 82° (in / mm) | Depth @ 90° (in / mm) |
|---|---|---|---|---|
| #4 | 0.225 / 5.71 | 0.1285 | 0.0555 / 1.41 | 0.0483 / 1.23 |
| #6 | 0.279 / 7.09 | 0.1495 | 0.0745 / 1.89 | 0.0648 / 1.64 |
| #8 | 0.332 / 8.43 | 0.1770 | 0.0892 / 2.26 | 0.0775 / 1.97 |
| #10 | 0.385 / 9.78 | 0.2010 | 0.1058 / 2.69 | 0.0920 / 2.34 |
| 1/4 | 0.507 / 12.88 | 0.2660 | 0.1386 / 3.52 | 0.1205 / 3.06 |
| 5/16 | 0.635 / 16.13 | 0.3320 | 0.1743 / 4.43 | 0.1515 / 3.85 |
| 3/8 | 0.762 / 19.35 | 0.3970 | 0.2099 / 5.33 | 0.1825 / 4.64 |
| 1/2 | 0.875 / 22.22 | 0.5312 | 0.1977 / 5.02 | 0.1719 / 4.37 |
Head diameters per ASME B18.6.3 flat head machine screws (82°); clearance holes are the normal-fit series. Depths are computed with D = (head − hole) / (2 × tan(θ/2)).
Countersink angle reference
| Angle θ | tan(θ/2) | Depth factor 1/(2·tan(θ/2)) | Typical use |
|---|---|---|---|
| 60° | 0.57735 | 0.86603 | metric flat-head screws (ISO), deburring |
| 82° | 0.86929 | 0.57518 | imperial flat-head screws (ASME B18.6.3), wood screws |
| 90° | 1.00000 | 0.50000 | metric flat-head screws (ISO 7046/10642), general machining |
| 100° | 1.19175 | 0.41955 | aerospace sheet metal, flush rivets |
| 118° | 1.66428 | 0.30043 | spot drilling with a standard 118° twist drill |
| 120° | 1.73205 | 0.28868 | center spotting, sheet-metal chamfers |
Depth = (OD − ID) × factor. The factor shrinks as the angle opens up, which is why a 120° countersink barely needs any depth at all.
Setting a countersink depth stop
- Calculate first. Get the exact depth from the calculator above, including your flush allowance (0.1–0.2 mm below the surface is the usual target for a clean flush finish).
- Drill press: chuck the countersink, bring the tip down to just touch the workpiece surface, zero the quill depth gauge, then set the depth stop to the target depth. Lock it.
- Hand drill: fit a microstop (cage) attachment and adjust its collar until the cutter's travel from the nosepiece equals the target depth; lock the collar with the set screw.
- Test on scrap. Cut one hole in a scrap offcut of the same material, drive the screw, and check the head with a straightedge. Adjust in 0.1 mm steps — it is easy to take another 0.1 mm off, impossible to put metal back.
- Watch the reference surface. Zero the stop on the actual face being countersunk, not on a burr or a clamped shim; a 0.2 mm chip under the part shows up directly in the depth.
Frequently Asked Questions
What is the countersink depth formula?
The primary formula is D = (OD - ID) / (2 × tan(θ/2)). D is the countersink depth, OD is the screw head (or countersink surface) diameter, ID is the pilot-hole (or screw shank) diameter, and θ is the included countersink angle. A sharper cone needs less depth: for the same head diameter, a 90° countersink is shallower than an 82° one.
What do OD and ID mean in the countersink formula?
OD (outer diameter) is the diameter of the screw head — or, equivalently, the diameter of the conical mouth at the surface of the workpiece. ID (inner diameter) is the diameter of the pilot hole the countersink cone grows out of, usually the screw shank clearance hole. Subtracting ID first matters because the cone only spans the ring between the hole edge and the head edge.
How deep should I countersink an M6 flat head screw?
An ISO 7046 flat head M6 has a head diameter of 11.3 mm and a normal-fit clearance hole of 6.6 mm. With a 90° countersink: D = (11.3 − 6.6) / (2 × tan(45°)) = 4.7 / 2 = 2.35 mm. To land the head flush rather than proud, add about 0.1–0.2 mm, so set the depth stop to roughly 2.5 mm and verify on a scrap piece.
Should I use an 82° or 90° countersink?
Use the angle your screw head was made for: imperial flat head screws and most wood screws are 82° (ASME B18.6.3), metric flat heads are 90° (ISO 7046). A 60° countersink is the metric standard for some ISO designs and deburring, while 100°, 118°, and 120° are common for spot drilling and sheet-metal work. Matching the angle keeps the head bearing evenly on the cone instead of touching on a ring.
How do I get the screw head exactly flush?
Aim for the top of the head to sit flush with the surface, typically 0.1–0.2 mm below it. Drill the countersink to the calculated depth, then sink the screw and check with a straightedge. If the head is proud, add 0.1 mm of depth and re-cut; if it falls below the surface, the countersink is already too deep and the joint should be re-made or the head backed with a washer.
What is a countersink depth stop and how do I set one?
A depth stop sets how far the countersink tool can travel. On a drill press, lock the quill depth stop so the tool advances exactly the calculated depth from the workpiece surface. On a hand drill, use a microstop (cage) attachment: adjust its collar until the cutter's travel equals the target depth, lock it, and test on scrap before cutting the real part.
What is the difference between a countersink, a counterbore, and a spotface?
A countersink is a conical recess that lets a flat head screw sit flush. A counterbore is a cylindrical recess, usually for socket head screws that sit below the surface. A spotface is a shallow flat-bottomed cut that cleans up a rough or angled surface so a fastener bears evenly. Use the countersink for angled heads, the counterbore for cylindrical heads, and the spotface when you only need a clean bearing surface.
Why is my countersink too deep or too shallow?
Usually one of three things: the countersink angle does not match the screw head angle (82° tool vs 90° head), the depth was calculated from the head diameter alone without subtracting the pilot hole, or the depth stop was set from the wrong reference surface. Check the tool angle stamped on the countersink shank, confirm you subtracted the hole diameter, and re-zero the stop on the actual workpiece face.
How do I account for a truncated countersink tool?
If the countersink or spot drill tip is truncated (flat) instead of a sharp point, add the truncation allowance to the calculated travel. For a tool with small-end diameter T and allowance a, the travel from the surface is Z = (D − T) / (2 × tan(α/2)) + a. The Truncated tool tab of this calculator does this for you: enter the small-end diameter and the allowance, and it returns the true tool travel.
How do I calculate countersink depth for imperial screws?
Pick your screw from the imperial table, which uses ASME B18.6.3 head diameters. For example, a #10 flat head screw (0.385 in head, 0.201 in normal clearance hole) with an 82° countersink: D = (0.385 − 0.201) / (2 × tan(41°)) = 0.184 / 1.7386 = 0.1058 in, which is about 2.69 mm. Toggle the unit selector to inches or millimetres at any time; the tables convert both ways.
Can I countersink with a spot drill?
Yes, a spot drill with the same included angle doubles as a countersink cutter for light work, but the tool must be sharp-pointed at the correct angle and the depth computed with the same formula. Dedicated countersink tools give a cleaner finish because their cutting geometry is made for the job, while spot drills are optimized for starting holes.
Is any of my input uploaded to a server?
No. This calculator runs entirely in your browser — every calculation happens in JavaScript on your device. Nothing you type is uploaded, stored, or sent anywhere, and the page works offline after it loads.
Free tool by NRTechStudio