Detailed Explanation of Seven Thread Processing Methods

• 1
  Key takeaways
• 2
  How the Seven Thread Processing Methods Differ
• 3
  Turning, Tapping and Thread Milling in Practice
• 4
  Rolling, Grinding, Whirling and Die Heads
• 5
  Step by Step: Choosing a Method from the Drawing
• 6
  Seven Thread Processing Methods Compared

Threading is not one operation. It is a family of seven methods, and each one removes or forms material in a different way. Single-point turning rotates the workpiece while a shaped insert travels along the axis. Thread milling orbits a smaller cutter around a bore. Tapping drives a multi-edge tool straight in. Rolling squeezes the blank between two dies. Grinding removes a small amount with a profiled wheel. Whirling spins a cutter ring around a rotating bar. Die heads cut external threads in one pass on a lathe or screw machine.

The choice is driven by four numbers on the drawing: thread size, pitch, tolerance class and material hardness. Add the annual volume and the answer is usually obvious. A Ø10 mm internal thread in aluminium at 5,000 pieces per year goes to tapping without discussion. The same thread in Inconel at 50 pieces per year goes to thread milling, because a broken tap in that material costs more than the cycle time saves.

One rule holds across all seven methods: the tool must match the flank angle and the pitch. A 60° insert cannot cut a 55° Whitworth thread correctly, and a roll-forming die will not reproduce a truncated root. Check the callout before you check the tool crib. Most thread defects we see start with a mismatch that was never noticed at setup.

Datum matters too. Threads are measured from a face or a shoulder, and that reference must be cut in the same setup if the drawing calls for a position tolerance. Re-chucking a part to add a thread after the fact is a common source of pitch-line runout. Where runout matters, keep the thread and its datum on one operation.

• 1
  External, large batchTurning or rolling
• 2
  Internal, small diameterTapping or thread milling
• 3
  Hardened materialGrinding or whirling
• 4
  Long slender barWhirling or die head

Single-point turning is the workhorse. A 60° insert with a partial profile or full profile cuts any pitch within its range, and the operator can adjust the minor diameter with offsets. On aluminium we run 200–350 m/min surface speed and take a 0.05–0.15 mm depth per pass over six to eight passes. On 304 stainless, drop to 60–100 m/min and expect work hardening if the insert rubs instead of cuts. Never dwell at the end of the pass.

Tapping is the fastest internal method below roughly Ø16 mm, and rigid tapping on a CNC synchronizes spindle and feed so the tap enters once. Cutting taps need a hole diameter that gives 60–75% thread height, not 100%. Form taps need a larger pilot hole and only work in ductile material below about 32 HRC. The classic failure is chip packing in a blind hole. Stop the hole 3–5 threads deeper than the callout, or use a spiral-flute tap that lifts chips out.

Thread milling uses a single cutter on a helical path, so one tool covers a range of diameters and both hands. It produces no axial thrust, which makes it safe on thin walls and long reach. Run 100–200 m/min in steel with 0.02–0.05 mm radial stepover per orbit. It is slower than tapping per hole, but it never gets stuck. For a Ø4 mm thread in a die-cast housing, that reliability is worth the extra cycle time.

All three methods depend on the same starting condition: a true pilot hole or a clean turned diameter. Drill runout shows up directly in the thread. Spot the hole, check the drill, and measure the pilot before the threading tool touches the part. We inspect pilot diameter on first article and monitor it in process, because a drill that wears 0.05 mm undersize will break a form tap before the thread gauge ever tells you why.

• 1
  Turning speed, aluminium200–350 m/min, 0.05–0.15 mm per pass
• 2
  Turning speed, 304 stainless60–100 m/min, avoid rubbing
• 3
  Thread milling stepover0.02–0.05 mm radial per orbit
• 4
  Blind hole clearance3–5 threads deeper than callout

Thread rolling forms the thread by cold working. Two or three dies press into the blank and displace metal into the crest. The result is a thread with a continuous grain flow at the root and better fatigue life than a cut thread. It needs ductile stock: low-carbon steel, aluminium, brass, and 303 stainless all roll well. High-carbon and hardened material will crack at the crest. Blank diameter must be controlled to about ±0.02 mm, because the die does not remove material, it moves it.

Thread grinding is the answer when the thread is already heat treated. A profiled wheel removes a few hundredths of a millimeter per pass and holds pitch accuracy that cutting cannot. It is slow and it costs more per part, but it is the only method that will hold a tight lead tolerance on a 58 HRC shaft. Dress the wheel often and keep coolant clean, or the profile will burn the flank.

Whirling uses a rotating cutter head with several inserts spinning around a slowly rotating bar. The cutting action is interrupted, so the chips are short and heat leaves with them. It suits long, slender threaded shafts such as feed screws and bone screws, where the axial load of a die head would bend the part. It also handles hardened material and deep profiles. Setup is the expensive part, so whirling pays off at medium to high volume.

Die heads cut external threads in a single pass on a lathe or screw machine and are common on high-volume fasteners and fittings. The head carries four chasers, and they can be adjusted for size without touching the program. They are fast and repeatable, but each head covers a narrow thread range. If you need three diameters in one run, thread milling or turning will be cheaper than buying three heads.

• 1
  RollingDuctile stock, blank ±0.02 mm
• 2
  GrindingPost-heat-treat, tight lead tolerance
• 3
  WhirlingLong slender shafts, interrupted cut
• 4
  Die headsOne-pass external, narrow range