📐 Free Gage Block Calculator — no login. Open it →

← AskMachinist · Guides · Calculator · 🔎 Search

How to Use a Thread Mill

Guide · Updated October 28, 2026

A thread mill cuts threads with helical interpolation: the cutter orbits the hole while moving one pitch down per revolution. One tool cuts many sizes of the same pitch, left or right hand, and a broken thread mill is easy to remove.

Check with a gage

Check the thread with a plug gage. The free Gage Block Calculator builds the stack.

Step by step

  1. Pick the cutter: Smaller than the minor diameter for internal threads.
  2. Drill: Drill to the tap drill size.
  3. Program the helix: Use the control cycle or CAM: one pitch per orbit.
  4. Climb mill: Internal right-hand thread: start at the bottom and climb up (G03).
  5. Compensate feed: Program the centerline feed so the edge feed is correct.
  6. Size with offsets: Adjust radial wear offset to size the thread.
  7. Gage: Check with a GO/NO-GO plug gage.

Worked example: 1/2-13 internal, 0.375 in thread mill

Feed compensation for internal thread milling: centerline feed = edge feed × (D − d) ÷ D, where D is the thread major diameter and d the cutter diameter. With D = 0.500, d = 0.375 and a desired edge feed of 10 in/min: 10 × (0.500 − 0.375) ÷ 0.500 = 2.5 in/min at the centerline. Orbit radius = (0.500 − 0.375) ÷ 2 = 0.0625 in at full depth. Z moves one pitch, 1 ÷ 13 = 0.0769 in, per 360° orbit.

Single vs multi-form

Single-form cutters cut one thread per orbit and need many orbits; multi-form cutters cut the whole length in about one orbit but deflect more.

Sizing

Start with the radial offset slightly small, check with the NO-GO gage, then increase in small steps until the GO enters.

Common problems

Tapered thread: deflection; add a spring pass. Wrong pitch: Z move per orbit wrong. Bad finish: edge feed too high, forgot compensation.

Worked example: arc length and time

The cutter center orbits a 0.0625 in radius, so one orbit is 2π × 0.0625 = 0.3927 in of centerline path. At 2.5 in/min that is 0.157 min, about 9.4 s per orbit. For 0.500 in of thread at 0.0769 in per orbit you need 0.500 ÷ 0.0769 = 6.5 orbits, so about 61 s plus the lead-in arc.

Climb or conventional?

For a right-hand internal thread, starting at the bottom and moving up with a counterclockwise orbit (G03) gives climb milling, the usual choice. Top-down with G02 also gives a right-hand thread but in conventional milling.

More common problems

Thread tight on the gage: tool deflection; add a spring pass or reduce the radial step. Taper in the thread: long overhang. Wrong hand: G02/G03 reversed relative to Z direction.

Tips

FAQ

What is thread milling?

Cutting threads by helical interpolation.

Climb or conventional?

Usually climb.

Why compensate feed?

So the edge feed is correct.

What is the formula?

Edge feed × (D − d) ÷ D for internal.

How do I size it?

Radial offset adjustments with gages.

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.