← AskMachinist · Guides · Calculator · 🔎 Search

Chamfer Mill Basics

Guide · Updated October 28, 2026

A chamfer mill puts a consistent edge break or bevel on a part. The trick is that the cutting diameter changes with depth, so you set depth and offset from the chamfer size, not the tool’s nominal size.

Check the chamfer

Check chamfer size and angle with a chamfer gage or optical comparator. Check it with a mic you've verified against gage blocks; the free Gage Block Calculator builds the stack.

Step by step

Pick the angle: Use a 90° included tool for 45° chamfers; 60° and 82° tools suit other bevels and countersinks.
Know the tip: Note the tip diameter or flat; a pointed tip has almost no cutting speed at the very end.
Pick a depth: Run the tip below the chamfer so the cut happens partway up the flute, not at the point.
Work out the offset: Calculate the tool center offset from the wall for that depth and chamfer size.
Set RPM: Base RPM on the largest effective diameter in the cut.
Cut: Run one pass around the part, climb milling, at a modest feed.
Check: Measure the chamfer leg and adjust Z by the error.

Worked example

0.030 × 45° chamfer with a 1/2 in 90° pointed chamfer mill: set the tip 0.080 in below the top. The cone radius at the top face is 0.080 in, and it has to touch the top face 0.030 in in from the edge, so the tool center sits 0.080 − 0.030 = 0.050 in outside the wall. Program the path with an effective radius of 0.050 in. The largest cutting diameter is 0.160 in, so in aluminum at 600 SFM, RPM ≈ 600 × 3.82 / 0.16 ≈ 14,000, which is often capped by the spindle.

Burrs and rubbing

A tip at the very bottom of the cut has no surface speed and rubs. Drop Z so the edge is cut mid-flute. A burr on the bottom edge also means the chamfer is too small.

Adjusting size

For a 45° chamfer each 0.001 in of Z changes the leg about 0.001 in. Adjust Z rather than the offset for small changes.

Tips

Inspect with checking a chamfer or countersink.
See countersink and counterbore basics.
Hand edge breaks: deburring and breaking edges.
Speeds: milling speeds and feeds.

FAQ

How do I set a chamfer mill depth?

Put the tip below the chamfer so the edge is cut mid-flute, then work out the offset from the wall.

What is the effective diameter of a chamfer mill?

The cutting diameter at the depth where it touches the part; it grows with depth.

What angle chamfer mill for 45° chamfers?

A 90° included angle tool.

Why does my chamfer mill leave a rough finish?

Usually the pointed tip is doing the cutting; drop Z.

Can a chamfer mill spot drill?

Many can spot shallow holes, but check the tip geometry first.

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.