5 Thread Treatment Methods in CNC Machining Centers

• 1
  Key takeaways
• 2
  Rigid tapping: the default thread treatment method in CNC for small holes
• 3
  Thread milling: one tool, any diameter, safer in blind holes
• 4
  Single-point turning: external and large internal threads on the lathe
• 5
  Thread forming: no chips, stronger threads in ductile metal
• 6
  Thread whirling: long, thin threads in hard material
• 7
  Step by step: picking and proving a thread method
• 8
  Thread method comparison by part geometry and material

Rigid tapping is the thread treatment method in CNC shops reach for first. The tap is held in a synchronous holder or directly in the spindle, and the machine feeds it at exactly the pitch you program. On a modern machining center the spindle encoder and the Z axis stay locked, so there is no floating holder to compensate for mismatch. That makes the process fast and repeatable, and a single M8 tap can cut hundreds of holes before it needs to be replaced.

Setup starts with the tap drill. For a cut thread, the drill diameter is the nominal diameter minus the pitch. An M8 × 1.25 tap takes a 6.8 mm drill. For a forming tap, add roughly half the pitch instead, so an M8 × 1.25 forming tap takes a 7.4 mm hole. Getting this wrong is the most common cause of a broken tap: too small and the torque climbs until the tap snaps, too large and the thread comes out with a flat crest.

Cutting speed depends on material. In 6061 aluminum we run 15–25 m/min with a spiral-flute tap and plenty of coolant. In 304 stainless that drops to 5–8 m/min. Cast iron runs dry at 8–12 m/min. Peck tapping is not needed in aluminum, but in deep holes in stainless, program a retract every 1.5 × D to clear chips.

The method has hard limits. Threads closer than about 1.5 mm to a shoulder need a spiral-point tap and a clearance groove, or you will not reach full depth. Threads below M3 in hard steel break taps often enough that thread milling is cheaper in the long run. And a tap cannot correct a hole that is out of position, so drill accurately first.

• 1
  Tap drill for cut threadNominal diameter minus pitch (M8 × 1.25 → 6.8 mm).
• 2
  Tap drill for formingNominal diameter minus pitch plus half pitch (M8 × 1.25 → 7.4 mm).
• 3
  Speed in aluminum15–25 m/min, coolant on, spiral flute.
• 4
  Speed in 304 steel5–8 m/min, retract every 1.5 × D for chip clearing.

Thread milling uses a single-point or multi-tooth cutter that orbits the hole while moving down by one pitch per revolution. Because the tool is smaller than the hole, it never gets wedged. That single fact is why thread milling is the safer thread treatment method in CNC when the hole is blind, deep, or made of a material that grabs a tap.

The programming is a helical interpolation. Feed rate is calculated at the tool center, not the thread crest, so the number you put in the program is lower than the actual cutting speed at the edge. If you skip that correction, the insert chips on the first pass. A 16 mm thread mill cutting a 0.5 mm radial step at 100 mm/min feed works well in 6061; drop to 40–60 mm/min in 4140 steel.

The payback is tool life and flexibility. One 16 mm thread mill covers M14 through M20 in coarse and fine pitch, so you do not stock a tap for every size. If a thread is gaged undersize, you re-run the helix with a larger offset instead of scrapping the part. In a job shop running mixed lots, that flexibility often beats the raw speed of tapping.

Thread milling is not the right answer for every hole. In a hole smaller than about M6, the tool is too slender to survive, and tapping wins. It is also slower per hole, so a part with 60 identical M8 holes is better tapped. Use thread milling when the part is expensive, the hole is blind, or the material is hard.

• 1
  Best hole rangeM6 and larger; below M6 the cutter is too weak.
• 2
  Feed in aluminumAbout 100 mm/min at tool center with a 0.5 mm radial step.
• 3
  Feed in 414040–60 mm/min, climb direction, air blast.
• 4
  Main advantageAdjustable offset lets you save an undersize thread without scrapping the part.

On a lathe, single-point threading is the standard thread treatment method in CNC turning. A 60° insert traverses along the part at the thread pitch while the spindle rotates, cutting one flank at a time. The tool is cheap, the geometry is easy to inspect, and the method handles thread pitches and diameters that no tap or mill can reach, including 4,000 mm long shafts on our mill-turn centers.

The key parameter is the infeed strategy. Plunge straight in and the chip gets wide and the insert breaks. Use flank infeed or alternating flank infeed, which spreads the cut across both edges. A typical 60° insert in 1045 steel runs at 120–180 m/min with a 0.05–0.15 mm depth per pass. In 316 stainless, 80–120 m/min and 0.05–0.10 mm per pass. Always leave 0.02–0.05 mm for a spring pass to clean up the flanks.

The most common error is thread crest width. If the insert tip radius does not match the pitch, the crest comes out flat or sharp. Check the insert chart before you start. The second error is running without enough coolant or air on the leading edge, which work-hardens stainless and tears the thread.

Single-point turning is slow per thread but very accurate. On a good lathe you can hold ±0.02 mm on the pitch diameter and a 0.8–1.6 μm finish. That is why aerospace and hydraulic fittings are almost always single-pointed, even when the thread is small.

• 1
  Infeed methodFlank or alternating flank, never straight plunge on steel.
• 2
  Speed in 1045120–180 m/min, 0.05–0.15 mm depth per pass.
• 3
  Speed in 31680–120 m/min, 0.05–0.10 mm per pass, spring pass 0.02–0.05 mm.
• 4
  Finish targetRa 0.8–1.6 μm with ±0.02 mm pitch diameter.

Thread forming does not cut. The tap has a lobed profile that presses the metal into the thread shape, cold-working the grain around the root. The result is a thread with no chip and a fatigue strength roughly 20–30% higher than a cut thread in the same material. In parts that see vibration, that matters more than the cycle time.

The method only works on ductile material. Aluminum, low-carbon steel, copper and brass all form well. Cast iron, titanium and hardened steel do not, because they either crumble or spring back. If you are not sure, check elongation: above about 12% is usually safe to form.

The forming tap needs a larger hole and more torque. Lubrication must be good, because the metal is being displaced, not sheared. In 6061 aluminum, run 20–30 m/min with a forming lubricant. In 1018 steel, 8–12 m/min. The hole must be drilled accurately; a tapered or oversized hole makes the formed crest lopsided.

One warning: forming taps are expensive and less forgiving of hole size than cutting taps. If the hole is 0.1 mm too small, the tap will break. If it is 0.1 mm too large, the thread will be weak. We usually prove the process on a scrap part before running a batch.

• 1
  Works on6061, 2024, 1018, 1045, copper and brass with elongation above 12%.
• 2
  Does not work onCast iron, titanium, hardened tool steel.
• 3
  Speed in 606120–30 m/min with forming lubricant, larger tap drill.
• 4
  Strength gainAbout 20–30% higher fatigue strength than a cut thread.

Thread whirling is the least common thread treatment method in CNC, and the one most people have never seen. The workpiece rotates slowly while a ring of inserts orbits around it at high speed. The inserts only touch a short arc of the thread at a time, so the cutting force is spread and the part does not deflect. It is the standard method for bone screws and small lead screws in 17-4PH or titanium.

Whirling is done on a dedicated whirling head mounted on a Swiss-type lathe or a mill-turn center. The inserts are ground to the exact thread profile, so the thread form is generated in one pass. Parameters depend on the head, but typical whirling runs at 1,000–3,000 rpm on the cutter ring with a slow workpiece rotation. The result is a thread with a fine, uniform surface and no burr.

The trade-off is setup. Each thread profile needs its own insert set, and the head must be dialed in. For a one-off part, that setup costs more than the part is worth. For a run of a few hundred bone screws, whirling is faster and more consistent than single-point turning, and it leaves a cleaner root radius.

Use whirling when the thread is long relative to its diameter, the material is hard, or the root radius must be controlled for fatigue. Do not use it for a standard M8 hole in an aluminum bracket. That is a tapping job.

• 1
  Typical partsBone screws, lead screws, long thin threads in 17-4PH or Ti-6Al-4V.
• 2
  Why it worksShort arc of contact keeps cutting force low and stops part deflection.
• 3
  Setup costHigh; justified only on runs of a few hundred parts.