← AskMachinist · Guides · Calculator · 🔎 Search

How to Cut a Dovetail

Guide · Updated October 28, 2026

Dovetails make slides and clamps that lock in one direction. On a mill they are roughed with an end mill, then finished with a dovetail cutter and measured over pins.

Measure over pins

Measure over pins with a mic you've verified against gage blocks; the free Gage Block Calculator builds the stack.

Step by step

Indicate the vise: True the vise and tram the head.
Rough with an end mill: Rough out the slot or step with an end mill, leaving material on the angled walls.
Mount the cutter: Hold the dovetail cutter short in a collet; they are fragile.
Slow down: Run about half the speed of an end mill of the same diameter.
Cut the angle: Take light radial passes into each wall at full depth.
Measure: Measure over pins and adjust the final pass.
Finish: Take a light finishing pass and deburr the sharp edges.

Worked example: measuring a 60° dovetail over pins

Here the dovetail angle α is the angle between the base (shoulder) and the flank, so a 60° dovetail has its flanks 30° from vertical. Use the same pin size on both sides. Check the pins with a mic before you start.

Formulas (D = pin diameter, α = dovetail angle):

Male (tongue), measured over pins: X = c + D × (1 + cot(α/2)), where c is the narrow width at the root (where the flanks meet the shoulders).
Female (slot), measured between pins: Y = b − D × (1 + cot(α/2)), where b is the wide width at the bottom of the slot.

For α = 60°: cot(30°) = 1.7321, so 1 + cot(30°) = 2.7321. With 0.2500 in pins the pin constant is 0.2500 × 2.7321 = 0.6830 in.

Male part. Tongue 0.375 in tall, 1.500 in wide at the root. Top width = 1.500 + 2 × 0.375 × cot(60°) = 1.500 + 2 × 0.375 × 0.5774 = 1.933 in. Over pins: X = 1.5000 + 0.6830 = 2.1830 in.

Mating female slot. Make the bottom width 1.938 in (0.005 in over the male top width, which leaves room for the gib). Between pins: Y = 1.9380 − 0.6830 = 1.2550 in. A 1–2 in mic or gage blocks plus a test indicator will read it.

Check the pins clear the flank. The pin touches the flank 0.2500/2 × cot(30°) = 0.2165 in from the corner, which is 0.2165 × sin(60°) = 0.1875 in up. The pin top sits 0.250 in up. Both are under the 0.375 in depth, so the pins sit on the flank and not on the top edge. On a shallow dovetail, drop to a smaller pin.

Dialing in the last pass. Suppose the male reads 2.1890 over pins. That is 0.0060 in large, so each flank has to move in 0.0030 in horizontally. With a 60° cutter that is a cut of 0.0030 × sin(60°) ≈ 0.0026 in square to the flank. On the mill it is simpler to move the table 0.0030 in in X for each side and take a spring pass. Measure again before the final pass.

Corners: the pins locate on the sharp corner where the flank meets the base. A relief groove or a cutter tip radius there is fine, because the pin never touches it. A burr or chip in the corner gives a false reading, so clean and deburr before you measure.

Why dovetail cutters break

They have a thin neck and many teeth engaged. Heavy feed, chips packing the teeth or a full-width first pass snap them. Rough first and clear chips.

Gib clearance

A sliding dovetail needs a gib strip on one side. Leave room for it and adjust it with screws for a smooth fit.

Tips

Tram first: tramming a mill.
Use milling speeds and feeds, then slow down.
Pins from a pin gage set work for measuring.
Blow chips out between passes.

FAQ

What angle are dovetails?

45°, 55° and 60° are common; 60° is the most common machine slide angle.

How do I measure a dovetail?

Over (or between) precision pins with a micrometer, using the pin formula for the angle.

Why do dovetail cutters break?

Thin necks, too much feed, and packed chips.

Should I rough a dovetail first?

Yes, rough with an end mill and leave only the angle for the dovetail cutter.

What speed for a dovetail cutter?

About half the RPM of an end mill of the same diameter.

Related guides and calculators

Build your stack in seconds

The free Gage Block Calculator finds the fewest-block combination for inch and metric sets, with wear blocks. No login.

Questions? Ask a machinist.

General shop information only — follow your machine and tooling manufacturer's instructions and your shop's safety rules.