CNC Thread Milling Calculator

Calculate spindle speed (RPM), feed rate (IPM), helix pitch per revolution, lead-in arc radius, and cutter offset for internal and external thread milling. Includes G-code parameter summary for helical interpolation.

Free Tool · UN / Metric Threads · Internal & External · G-Code Params · Inch & Metric

Thread Standard

Thread Size

Common Thread Presets

Thread Type

Thread Mill Cutter

Cutter Diameter

⌀ in

OD of the thread mill body (not thread profile diameter).

Number of Flutes

Z fl.

Cutting Conditions

Cutting Speed

SFM

Chipload (fz)

fz in/tooth

Thread milling uses lower chiploads than endmilling. Typical: 0.0005–0.002 in/tooth for carbide in steel; 0.001–0.003 in/tooth in aluminum.

Results

Spindle Speed

—

RPM

Feed Rate

—

IPM

Helix Pitch / Rev

—

Z rise per cutter revolution

Thread Pitch

—

in (1/TPI)

Cutter Offset (R)

—

Helical arc radius

Lead-In Arc Radius

—

90° or 180° lead-in

Z Rise per 360° Pass

—

Full thread helix Z per pass

Cycle Time (1 pass)

—

Approx. sec for 360° pass

Ready Select thread size and cutter, then click Calculate.

G-Code Parameter Summary

; Run calculator to generate G-code parameters

Detailed Summary

Thread Geometry
Thread size	—
Thread type	—
Thread pitch	—
Thread major diameter	—
Thread minor diameter (approx.)	—
Cutter / Toolpath
Cutter diameter	—
Cutter offset (helical arc radius R)	—
Lead-in arc radius	—
Helix pitch per cutter rev	—
Z per 360° pass (= thread pitch)	—
Speeds & Feeds
Cutting speed	—
Spindle speed (RPM)	—
Chipload per tooth	—
Feed rate	—
Approx. cycle time (1 pass)	—

Thread Milling Toolpath Diagram — Top View & Helix Profile

The cutter follows a helical arc around the thread axis. One full 360° revolution advances exactly one thread pitch in Z. The cutter offset R = (thread_dia − cutter_dia) / 2 for internal threads.

How CNC Thread Milling Works

Thread milling uses a rotating thread mill cutter that travels in a helical interpolation path (G2 or G3 arc with simultaneous Z movement). In a single 360° helical revolution, the cutter cuts a full thread profile and advances exactly one pitch in Z. Thread milling offers major advantages over tapping: it works in blind and through holes with the same cutter, creates no axial thrust, allows thread size adjustment with cutter offset, and is much safer in hard or exotic materials where taps often break.

1 Spindle Speed & Feed Rate

RPM is calculated from the cutter diameter (not the thread diameter) and the surface footage for your material. Feed rate (IPM) is standard chipload × flutes × RPM — same as any milling operation.

RPM = (SFM × 3.82) / Dc (Dc = cutter diameter, not thread dia) Feed Rate: IPM = RPM × fz × Z fz = chipload per tooth (in) Z = number of flutes Metric: RPM = (Vc × 1000) / (π × Dc) mmpm = RPM × fz_mm × Z

2 Cutter Offset & Helix Radius

The cutter center travels on a circle offset from the thread axis. For internal threads, the offset R = (thread_major_dia − cutter_dia) / 2. This is the arc radius used in the G2/G3 block. For external threads, the math inverts.

Internal Thread Offset: R = (D_thread − D_cutter) / 2 External Thread Offset: R = (D_thread + D_cutter) / 2 D_thread = thread major diameter D_cutter = cutter body diameter Example (½-13 internal, ⅜" cutter): R = (0.500 − 0.313) / 2 = 0.094" This R value goes in G2/G3 block: G91 G2 X0 Y0 Z-0.077 R0.094 F12

3 Helix Pitch per Revolution

In one full cutter revolution around the thread axis (360° of arc), the tool must descend exactly one thread pitch in Z. For a multi-start thread mill (multiple rows of teeth axially), a single helical pass cuts the full thread depth in one 360° revolution. For a single-tooth cutter, multiple passes with Z offset are needed.

Thread Pitch (inch): P = 1 / TPI Thread Pitch (metric): P = as specified (mm) Z per 360° helical pass = P Helix pitch per cutter revolution: Z/rev = P × (RPM × circumference / IPM arc) = P (exactly — by definition) For ½-13 UNC: P = 1/13 = 0.07692" Z per 360° pass = 0.07692"

4 Lead-In Arc

The cutter must enter the thread arc tangentially — not straight-line plunge — to avoid a witness mark or gouging. A 90° or 180° lead-in arc at half the cutter offset radius brings the cutter smoothly onto the thread circle before the helical cut begins.

Lead-in arc radius: r_leadin = R / 2 (half the cutter offset radius) Typical lead-in sequence: 1. Position at thread center X,Y 2. Move to lead-in start (Y + R + r) 3. G2/G3 arc lead-in (quarter circle) 4. G2/G3 full 360° helix (Z = −P) 5. G2/G3 arc lead-out (quarter circle) 6. Return to center, retract Z Total arc = lead-in + 360° + lead-out

Thread Milling vs. Tapping — When to Switch

Thread milling becomes the preferred process when: (1) the workpiece material is hard (>40 HRC) where taps break unpredictably; (2) you're making large diameter threads (over ¾") where rigid tapping torque is excessive; (3) the hole is blind and thread depth control is critical; (4) you need left-hand threads — just reverse the helical direction; (5) materials like titanium, Inconel, or hardened steel make tapping risky and expensive. The trade-off: thread milling requires a correctly programmed helical interpolation path and is slower per hole than a rigid tap cycle. For high-volume production of small threads in aluminum, tapping is usually faster and more economical.

Worked Examples

🔩 1/2-13 UNC in Steel

Thread: ½-13 UNC internal Cutter: 5/16" dia, 4 flutes SFM: 300 (alloy steel) Chipload: 0.0008 in/tooth Offset R: 0.094"

RPM = 3,667 IPM = 11.7
Pitch = 0.0769" Z/360° = 0.0769"

Classic rigid-tapping alternative in medium carbon steel. One helical pass cuts full thread. Use flood coolant and verify cutter offset exactly.

🔩 M10×1.5 in Aluminum

Thread: M10×1.5 internal Cutter: 8mm dia, 4 flutes Vc: 250 m/min (aluminum) Chipload: 0.04 mm/tooth Offset R: 1.0 mm

RPM = 9,947 mmpm = 1,591
Pitch = 1.5mm Z/360° = 1.5mm

Thread milling aluminum at high speed. Small cutter offset (1mm) requires precise setup. Air blast chip evacuation essential at these feed rates.

🔩 3/4-10 UNC in Inconel

Thread: ¾-10 UNC internal Cutter: ½" dia, 4 flutes SFM: 50 (Inconel 718) Chipload: 0.0006 in/tooth Offset R: 0.125"

RPM = 382 IPM = 0.92
Pitch = 0.100" Z/360° = 0.100"

Tapping Inconel risks tap breakage and scrapped parts. Thread milling at very low SFM is safer and controllable. Use TiAlN coated cutter with flood coolant.

Common Thread Milling SFM / Chipload Reference

Material	SFM (Carbide)	Chipload (in/tooth)	Coolant	Notes
Aluminum 6061	600–1,200	0.001–0.003	Air / flood	High speed, good chip clearance
Mild Steel (1018)	250–400	0.0006–0.0012	Flood	Standard thread milling
Alloy Steel (4140)	200–350	0.0005–0.0010	Flood	Reduce SFM for harder variants
Stainless 304/316	100–200	0.0004–0.0008	Flood	Work hardening risk — maintain feed
Hardened Steel (45+ HRC)	60–120	0.0003–0.0006	Oil mist	Use CBN or fine-grain carbide
Titanium Ti-6Al-4V	60–100	0.0004–0.0008	High-pressure flood	TiAlN coating essential
Inconel 718	40–70	0.0003–0.0006	Flood	Very low SFM, sharp edges
Brass / Bronze	400–700	0.001–0.002	Dry / air	Free-machining, excellent tool life

Frequently Asked Questions

For right-hand internal threads: use G2 (clockwise arc when viewed from above) traveling in the −Z direction (downward helix). This produces a conventional climb-milling engagement on the thread profile. For left-hand internal threads: use G3 (counter-clockwise) in the −Z direction. For external threads the directions reverse. Always verify the helical direction by dry-running the program at a safe Z height before cutting. The mnemonic: for right-hand internal threads, think "screw the bolt in clockwise while moving down" — that's G2 with Z−.

Yes — a single-profile thread mill (with one row of cutting teeth matching a specific pitch) can cut any thread diameter that accommodates the cutter body diameter. A ⅜" cutter grinding a ¼-20 pitch profile can also cut ½-20, ¾-20 — any 20 TPI thread — just by adjusting the cutter offset R in the G-code. Multi-form thread mills (multiple rows of teeth) can only cut threads matching their specific pitch. This programmable offset is one of thread milling's key advantages: thread size and fit class can be adjusted in software without changing cutters.

The cutter must physically fit inside the hole. The cutter diameter must be less than the thread minor (root) diameter. As a practical rule, the cutter diameter should be no more than 60–70% of the thread major diameter for internal threads, to allow sufficient room for the cutter to follow the helical arc. For very small threads (under ¼" / M6), thread milling becomes difficult because cutter diameter options are very limited. At those sizes, tapping is usually faster and more economical unless you're in a material where tap breakage is a concern.

Thread fit class is controlled by adjusting the cutter offset (R value) in the G-code. Increasing R moves the cutter further from center, cutting a larger effective thread diameter — creating a looser fit (1B or 2B). Decreasing R cuts tighter. Start with the nominal offset, cut a test thread, and measure with a go/no-go gauge or thread micrometer. Adjust R in increments of 0.0002–0.0005" until the desired fit class is achieved. This is far easier than grinding or sourcing different taps for different tolerance classes. Document the final R value for production repeatability.