About the Thread Molding: How a Helical Path Cuts Threads
Thread molding, usually called thread milling on the shop floor, cuts threads with a rotating tool that travels along a helical path instead of a tap that screws itself into the hole. This page covers the kinematics, the tool geometry, the thread forms it suits, and the cases where tapping is still the better call. Read it before you quote a stainless or titanium part with a deep M6 thread.
What we mean by about the thread molding
In thread molding, better known as thread milling, a single-point or multi-flute cutter rotates on its own axis while the machine moves it along a helical path. The helix pitch equals the thread pitch. The cutter radius is smaller than the hole radius, so the tool never fills the thread. Material comes off in many light passes rather than one full engagement.
Because the tool is smaller than the thread, chip load per tooth stays low. A 0.5 mm radial stepover on a 16 mm cutter in 316L stainless is a normal starting point. The same thread cut by a tap would load the full thread flank in one rotation.
The path is defined by the CAM system, not by the tool shape. Change the helix diameter and you change the thread minor diameter without touching the tool. That is the part engineers usually miss on the first quote.
Cutter geometry and what it allows
A thread mill carries either one full-profile insert or several partial-profile teeth. Full-profile tools cut the crest, flank, and root in one helix. Partial-profile tools cut only the flank and leave the crest to the pre-drilled hole, so the hole diameter must be right before the thread mill enters.
Single-point tools are the most forgiving. One tool covers any pitch within its range because the machine controls the helix, not the insert. A shop that runs many thread sizes in low volume keeps a handful of single-point mills instead of a drawer of taps.
Multi-flute mills cut faster because more teeth engage per revolution. They also need a stiffer setup and a more accurate pre-drill. On a 4,000 mm long aluminum extrusion with a thread at each end, the extra rigidity is usually worth it.
Where the process earns its keep
Hard or gummy materials are the classic case. Inconel, Ti-6Al-4V, and 17-4PH stainless work-harden fast under a tap. A tap that stalls for half a second rubs instead of cuts, and the next rotation snaps it. A thread mill makes many shallow passes, so each tooth sees a short, controlled engagement.
Thin-wall parts and large diameters are the second case. A tap pushes radial force into the wall and can distort a 2 mm wall on a tube fitting. A thread mill cuts with light radial engagement and lets the wall hold its roundness. Threads above M20 or 1 in are rarely tapped on a CNC anyway.
Blind holes are the third. A tap needs thread depth plus chamfer plus chip room. A thread mill needs only the thread depth plus a small clearance for the helix entry, often 1–2 mm. On a 12 mm deep M8 blind hole that difference decides whether the part fits.
Cutting parameters and the traps
Surface speed for a carbide thread mill in aluminum runs 150–250 m/min. In 316L stainless it drops to 60–90 m/min, and in Ti-6Al-4V to 40–60 m/min. Feed per tooth stays modest, often 0.03–0.08 mm, because the tool has little core strength.
Climb milling is the default for internal threads. It throws the chip ahead of the cut and keeps the flank clean. Conventional milling on a thread mill rubs the flank and shortens tool life, especially in stainless.
The trap most programmers hit is the entry arc. Plunge straight into the hole and the tool center can pass through the thread crest. Ramp in on a small arc, then start the helix. The other trap is the exit: pull the tool to the hole center before retracting, or the flank drags across the finished thread.
Rigid tapping heads and floating holders solve the wrong problem here. A thread mill runs on the same spindle as any end mill, so the setup is one tool change, not a dedicated holder.
How to check the thread before it ships
A thread mill leaves a thread that is round and on pitch, but the pitch diameter still needs measurement. Plug gauges work for production runs. For large or unusual threads, use thread wires or a three-wire measurement and record the pitch diameter against the drawing.
Surface finish on the flank matters for sealing threads. A thread mill typically leaves Ra 0.8–1.6 μm in stainless without a separate operation. A tap often tears the flank in the same material unless the shop uses a forming tap and the right lubricant.
At GreatLight, threads are inspected as part of the 100% check before shipment, with reports on request. Raw material, in-process, and final inspection all apply to threaded features, not only to the critical diameters.
If a thread fails a gauge, the cause is usually the pre-drill diameter or a worn insert, not the helix. Check the hole first, then the tool offset, then the program.
Thread milling against tapping, by part condition
Pick the row that matches your part.
| Condition | Thread milling | Tapping |
|---|---|---|
| Material above 35 HRC | First choice | High snap risk |
| Titanium and Inconel | First choice | Work-hardening stalls the tap |
| Wall under 3 mm | Low radial force, holds round | Distorts the wall |
| Thread over M20 | Standard practice | Needs a large tap and high torque |
| Blind hole, tight depth | Needs 1–2 mm entry clearance | Needs depth plus chip room |
| Aluminum 6061, M6 through hole | Works, slower cycle | Faster and cheaper |
| One-off or repair work | One tool covers many pitches | Needs the exact tap on hand |
| Deep hole, 3× diameter | Chip evacuation is easy | Chips pack and break the tap |
The short answer on about the thread molding
If the material is hard, the wall is thin, or the thread is large, use thread milling and accept the longer cycle. If the part is soft aluminum with a through hole under M12 and you run thousands of them, tap it.
Common questions
Can a thread mill cut a thread in a hardened part?
Yes, within reason. Carbide thread mills cut materials above 45 HRC if the setup is rigid and the surface speed is low. Below that, the choice between milling and tapping comes down to hole depth and tool cost, not hardness.
For very hard parts, consider whether the thread can be cut before heat treatment. Milling a soft part and then hardening is usually cheaper than milling a hard one.
Does the pre-drill diameter change for a milled thread?
No. The pre-drill is set by the thread form, the same as for a tap. What changes is the tolerance on that hole. A partial-profile thread mill needs the pre-drill closer to nominal, because the crest comes from the hole, not the tool.
A full-profile thread mill cuts the crest itself, so the pre-drill can run a little larger and still pass the gauge.
Why does the cycle time look so long on the quote?
A thread mill makes many light passes instead of one. A 20 mm deep M10 thread might take 30 to 60 seconds of cutting, where a tap takes a few seconds. That is the cost of avoiding a snapped tool and a scrapped part.
On high-volume soft aluminum, tapping still wins on cycle time. On stainless and titanium, the thread mill usually wins once you count the scrap.
Can the same tool cut left-hand and right-hand threads?
Yes. The helix direction is set in the CAM path, not in the tool. One single-point mill can cut a right-hand internal thread on one part and a left-hand external thread on the next.
Multi-flute and full-profile tools are often ground for one hand. Check the tool drawing before you program.
How do I hold a part for external thread milling?
External threads are cut on a rotary table or a 4-axis setup so the helix stays continuous. A Ø400 mm rotary table covers most work up to the size of the table. Larger parts run on a mill-turn center.
If the part is long, support the free end. A 4,000 mm shaft with a thread at each end will deflect under cutting force unless it is steadied.
What tolerance can we hold on a milled thread?
Thread milling holds the same class of fit as a good tap, typically 6H for internal and 6g for external. The pitch diameter comes from the tool offset, so the machine can correct it in small steps without changing the tool.
For critical threads, cut a test part first and adjust the offset from the gauge reading. That step costs one cycle and saves a batch.
Send us the thread callout and the material
Upload the drawing and we return a quotation with a free DFM analysis within 12 hours, including a note on whether the thread should be milled or tapped.
12-hour quote100% inspectionNo minimum order quantity
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
