Thread milling

A thread mill, in Allied Machine’s words, “can be thought of as an end mill with the profile of the thread on the side”, and it “has a smaller diameter than the thread size being produced”. The machine moves it in a circle around the thread’s axis and, at the same time, along that axis: a helical interpolation. ISCAR puts the rule in one line: “The cutter movement along the thread length while completing one round around the part is equal to the pitch of requested thread.”

That one rule decides everything else. The thread’s pitch and hand come from the path, not from the tool, so the same cutter can cut many diameters, right- and left-hand, inside and outside. The price is that the machine must be able to interpolate helically; Vargus: “To perform a Thread Milling operation, a helical interpolation movement is required.”

The path, block by block

Full orbit: the threadX

0.5000

Y

0.0000

Z

−0.3750

1. S1000 M03spindle clockwise, 1000 rpm
2. G01 Z-0.5156 F50.feed to the starting depth: −0.5 minus 1/8 of the pitch
3. G41 X0.25 Y-0.25 F10. D01cutter compensation on
4. G03 X0.5 Y0 I0 J0.25 Z-0.5quarter arc into the thread, ramping up 1/8 pitch
5. I-0.5 J0 Z-0.375 F20.one full orbit: Z up one pitch, the whole thread
6. X0.25 Y0.25 I-0.25 J0 Z-0.3594quarter arc out of the thread, up 1/8 pitch
7. …compensation off, retract

Cutting blocks of O60023 as Haas prints them (excerpt). Haas’s next block, G40 G01 X0 Y1, would carry the tool outward through the wall if taken literally (an X0 Y0 was evidently meant); the figure returns the tool to the centre before it retracts, as in ISCAR’s sequence.

ISCAR describes the recommended sequence as rapid approach, an arc into the material, one full orbit of 360°, an arc out and a rapid return. Haas’s program follows the same pattern. The tool goes down to 1/8 of a pitch below the start of the thread (Z−0.5156 for a thread starting at Z−0.5), the quarter arc ramps it up that 1/8 pitch, the full orbit lifts it by one pitch (0.125 in, 8 threads per inch) and the arc out adds another 1/8.

Multi-tooth or single-profile. A multi-tooth cutter carries several thread teeth; in Vargus’s words “every tooth creates one pitch”, and the thread is finished “by one pass only”, in one orbit. A single-profile cutter has one tooth and needs one orbit per pitch of thread length: Haas’s single-point example O60025 repeats its 360° block five times with L5. ISCAR says the thread is done in 1 to 1.3 turns of the tool around the work, the extra 0.3 turn for the plunge to depth and the overlap.

Why mill a thread instead of tapping it

The makers list the same advantages:

Allied explains the low force: “Thread mills only cut a portion of the circumference at a time.” For large parts, Kennametal says thread milling “requires considerably less horsepower compared to other threading methods”, and EMUGE offers thread mills “for threads from 24 mm to infinity”. Vargus adds two cases where a tap struggles: soft materials, “where taps normally tear the material”, and bores with no upper size limit. For tap breakage itself, see tap breakage.

The limits are the machine and the program. The machine needs helical interpolation: WNT’s precondition is a CNC milling machine or machining centre with that function. The tangential entry takes slightly more programming than a straight one (Vargus). And Vargus notes that its insert tools, which cut only once per revolution, are “sensitive to vibrations”. Haas warns that internal threads below 3/8 in “may not be possible or practical”. ISCAR lists “short machining time” among the advantages, but none of the sources we read compares cycle times with tapping.

Tools

ISCAR sorts thread mills into solid tools, tools with indexable inserts and tools with exchangeable heads, built as end mills with a shank or as shell mills with a bore. Its solid carbide MTEC cutters run from 2.2 to 20 mm cutting diameter, the MTECZ with internal coolant from 7.6 to 16 mm, and the MTECS has “a short 3-tooth cutting zone” on a relieved neck, down to M1.4 × 0.3, whose “very short profile exerts a low force which minimizes tool bending.” WNT’s Turkish catalogue lists single-row thread mills, thread mills with a countersinking chamfer, and drill thread mills that make the hole and the thread with one tool; EMUGE’s Thriller drills the core hole, countersinks and mills the thread in one work sequence (“in einem Arbeitsablauf”), with no tool change.

Climb milling and the direction of the path

The sources agree that climb milling is the normal choice. ISCAR: “Climb milling in most cases is the preferred way for machining threads.” Vargus: it “is now generally recommended”. Haas: “Always climb cut the cutter.” Kennametal gives the reasons: “lower cutting forces, better chip development, higher thread surface quality”. Allied adds that with climb milling the chips leave the cutter faster, while conventional milling lets them be recut. The general case is on climb and conventional milling.

ISCAR names the exceptions: “If the machine does not counteract backlash, then conventional milling is recommended”, and conventional milling is also preferable for cast iron and hardened materials. Two documents go further and are worth knowing about: FRAISA’s 2026 catalogue recommends “up-cut milling” (German edition: “Gegenlauf”) for its thread mills, and Vargus’s TM Solid catalogue says “Conventional milling with multiple passes is required” for its multi-pass method, unlike Vargus’s handbook.

With the spindle turning clockwise (M03), climb milling fixes the direction of the orbit, and the direction of Z then fixes the hand of the thread:

Haas: “Use a G03 to cut I.D. threads or a G02 to cut O.D. threads”, and “An I.D. right hand thread will move up in the Z-Axis by the amount of one thread pitch.” By the same geometry (our derivation; the sources show only right-hand examples), a left-hand thread keeps the orbit and reverses Z. ISCAR says the combination of movements depends on whether a left- or right-hand thread is wanted, and Vargus that its tools cut either hand “depending only on the tool path which is programmed.”

Programming

Enter on an arc. “Tangential entering by arc (recommended)”, writes ISCAR, “because the cutter gradually enters the material and the load on the tool increases gradually.” Vargus calls it “The best method!!!” and warns that a straight radial entry may leave “a small vertical mark” at the entry and exit; Harvey Tool asks for an arcing path “to avoid shock loading”. ISCAR keeps a straight tangential entry for external threads only.

Ramp Z on the arc. Allied makes the arc-on radius (major Ø − tool Ø) / 4 and raises Z by pitch / 8 on it; Haas’s program does the same (“Ramps up by 1/8th of the pitch”), and so does ISCAR’s template.

Compensation for wear only. The program describes the path of the tool centre, at a radius of (major Ø − tool Ø) / 2 for an internal thread; ISCAR’s example: an M48 × 2 thread with a Ø29 cutter gives 9.5 mm. ISCAR: “This method of programming needs no tool radius compensation value other than an offset for wear.” Allied: “No diameter value should be stored in the machine’s controller for the thread mill.” Compensation is switched on (G41) before the arc in and off after the arc out.

Taper threads. For pipe threads the path must open up as it climbs. Allied: “Even though the thread mill is tapered, the thread mill must move out in X and Y as it moves up in Z.” Vargus programs parallel threads incrementally and conical threads in absolute coordinates.

Feed: the edge against the centre

The feed per tooth is meant at the cutting edge, but the program runs the tool centre. Inside a hole the centre travels on a smaller circle than the edge, so its feed must be smaller; outside, larger. The edge feed is

$$v_f = f_z \cdot z \cdot n$$

(Allied, Vargus, FRAISA), and the feed to program for the centre is, for an internal thread,

$$v_{fm} = v_f \cdot \frac{D - d}{D}$$

with the thread’s major diameter D and the cutter diameter d (Harvey Tool, Allied). For an external thread Harvey Tool uses (D + d) / D. WNT’s Turkish catalogue makes the same warning: watch whether the contour feed vf or the feed of the centre vfm is meant.

ThreadM6 × 1M8 × 1.25M10 × 1.5M12 × 1.75M16 × 2M20 × 2.5M24 × 3M30 × 3.5M36 × 4M42 × 4.5M48 × 5

Thread type

InternalExternal

Flutes123456Cutter Ø

12

mmCutting speed

100

m/minFeed per tooth

0.050

mm

Spindle speed

2653 rpm

Feed at the cutting edge

531 mm/min

Feed of the tool centre (program this)

212 mm/min

Tool-centre path radius

4.00 mm

Arc-in radius

2.00 mm

Z on the arc

0.313 mm

Cutter / thread Ø

60 %

ISCAR: ≤ 70 % · D

14.0 mm · within

Vargus: < 70 % · D1

12.1 mm · within

FRAISA: ≤ ⅔ · D1

11.5 mm · over

Vargus’s TM Solid catalogue lowers the feed on entry: “set the Feed f [mm/tooth] to 70% lower than the threading Feed”.

Cutter size

A thread mill’s teeth are rings, with no helix, so the profile it cuts is slightly distorted, and the distortion grows with the pitch and with the cutter’s diameter (ISCAR). Hence a limit on the cutter’s size for internal threads:

For an M20 thread ISCAR’s rule gives 14 mm, Vargus’s about 12.1 mm and FRAISA’s about 11.5 mm (70 % and 2/3 of the basic minor diameter, 17.29 mm). For external threads, ISCAR allows more than 70 %, and Vargus says the distortion “is neglected” for ISO, UN and Whitworth threads. Within the limit, ISCAR notes the trade-off: a larger cutter is stiffer and more productive, a smaller one cuts a more accurate profile.

Radial passes

In tough materials or with large pitches the thread is cut in more than one radial pass, each to a larger share of the depth:

A pass at unchanged offset helps when the thread fails the gauge because of tool deflection: Vargus’s remedy is to “execute a ‘zero’ cut”, and ISCAR’s troubleshooting table lists “Use ZERO compensation”.

Cutting data

Thread-milling data are tool-specific, and few makers’ tables could be read cleanly. Allied’s metric table for its solid carbide AccuThread T3 thread mills:

ISCAR gives 0.05 to 0.15 mm per tooth for its indexable inserts in grade IC908, and its solid carbide tables reduce the feed by 40 % for cutters with a long cutting flute. Allied runs its T3 thread mills left-hand cutting (M04) and from the top down, to keep climb milling, so the direction table above does not apply to them as it stands. Kennametal’s catalogue gives 300 to 700 SFM (91 to 213 m/min) for its indexable thread-mill inserts in carbon steels below 187 HB. Vargus starts tests with its insert tools at 100 m/min and 0.05 mm per edge.

Faults

Vargus notes that chatter is easy to recognise: the noise “is extremely loud”.

For the tapped alternative, see tapping; for the threads themselves, ISO metric screw threads.