8 Thread Processing Methods: What You Need to Know When Machining

• 1
  Key takeaways
• 2
  How thread processing methods differ at the cutting edge
• 3
  Thread processing methods for internal threads
• 4
  Thread processing methods for external threads
• 5
  When a thread processing method is the wrong choice
• 6
  Step by step: choosing and cutting a thread
• 7
  Eight thread processing methods compared

Every thread processing method removes or displaces material along the same helical path. The difference is how the tool meets the material. Cutting methods (tapping, turning, milling, grinding) shear chips away. Forming methods (rolling, forming taps) push metal into shape. Casting and additive methods create the thread as part of the part itself.

That single difference drives most decisions. A forming tap needs a hole about 0.1–0.2 mm larger than a cutting tap of the same size, because the material has to flow into the flanks. A rolled external thread needs a blank diameter close to the pitch diameter, not the major diameter. Get those blank sizes wrong and no amount of tool pressure will save the part.

Cutting methods also fail differently. A tap breaks inside the hole and you may lose the part. A thread mill breaks and you change the tool. For a one-off prototype in titanium, that difference matters more than cycle time.

In our shop, 127 high-precision CNC machines run these methods daily, from M1.6 electronics threads up to Ø400 mm rotary table work. The method choice is made in DFM, before the first chip.

• 1
  CuttingTap, turn, mill, grind. Chips form, tool wear is measurable, thread depth is predictable.
• 2
  FormingRoll, form tap. No chips, stronger grain flow, tighter blank control required.
• 3
  Additive / castingThread printed or cast in. Low strength, needs cleanup with a tap or reamer.

Internal threads are where most scrap happens. Tapping is the fastest method and still the default for holes from M2 to M20 in aluminum, brass and mild steel. On a CNC mill, rigid tapping with synchronized feed at 300–800 rpm works well in aluminum; drop to 100–200 rpm in stainless 316 or Inconel, and use a spiral-flute tap for blind holes so chips come out of the hole, not down into it.

Thread milling is the method we recommend for anything above M6, for difficult materials, or for large threads on expensive parts. A single-point or multi-flute thread mill helically interpolates the thread. If the tool breaks, you extract it and keep the part. One tool can cut several pitches by changing the program, which cuts tooling cost on low-volume jobs.

A blind hole needs thread depth plus clearance. Rule: drill depth = thread depth + 0.5 × diameter, and leave a chip pocket. A bottoming tap still needs 1–2 mm of clearance, and a thread mill needs enough room for the tool nose to exit the helix.

For threads smaller than M2, or in hardened steel above 45 HRC, standard tapping becomes unreliable. We use micro thread milling or EDM-cut threads in those cases, with a pre-drilled minor diameter held to ±0.01 mm.

• 1
  Tapping speedsAluminum 400–800 rpm; stainless 100–250 rpm; titanium 80–150 rpm.
• 2
  Thread millingBest above M6, in hard material, or when the part value is high.
• 3
  Blind hole ruleDrill depth = thread depth + 0.5 × Ø. Always add a chip pocket.

Single-point turning on a lathe is the most flexible external method. It handles odd pitches, tapered threads and large diameters up to 4,000 mm on our mill-turn and turning centers. Threading inserts are ground to a specific pitch, so a program change is a tool change. For a 1/2-20 UNF in 4140 steel, typical speed is 150–250 m/min surface speed with a 0.05–0.1 mm depth of cut per pass and 4–6 passes.

Thread rolling displaces material between two or three dies. The grain flow follows the thread profile instead of being cut, so fatigue strength improves. It is fast, chipless and produces a mirror-like flank. The catch: the blank diameter must be close to the pitch diameter, roughly major diameter minus 0.7 × pitch for UN threads. Roll too large and the dies overload; too small and the crest is incomplete.

Thread rolling only works on ductile materials. Aluminum 6061 and 7075 roll well. 303 stainless rolls well. Hardened steel above 40 HRC, cast iron and most titanium grades should be cut, not rolled.

For very long threads or thin-walled tubes, we use a die head or a chasing method on a lathe. Both need support on the free end, or the part will deflect and the pitch will drift.

• 1
  TurningAny pitch, any diameter, best for one-offs and large parts.
• 2
  RollingStronger thread, faster cycle, needs ductile material and correct blank Ø.
• 3
  Die head / chasingLong threads and thin walls; support the free end.

Tapping a hardened tool steel part is a losing game. Above 45 HRC the tap dulls in a few holes and the pitch diameter drifts. Either thread mill before heat treat and accept the distortion, or grind the thread after hardening. For a mold core at 52 HRC, thread grinding is the only method that holds class 6H.

Thread rolling a thin-wall aluminum tube sounds efficient until the wall collapses between the dies. Below about 1.5 × pitch wall thickness, switch to thread milling or turning. The same applies to hollow parts with a wall under 2 mm.

3D-printed threads are for fit checks, not for load. FDM and SLA threads typically come out undersized and with a rough flank. Print them 0.2–0.3 mm oversize on the pitch diameter if you plan to chase them with a tap. For functional threads, print the pilot and cut the thread.

Finally, do not mix thread standards on one part without a note. A 1/4-20 UNC hole and an M6 hole are close in size and easy to confuse. Mark the drawing with the standard, class and depth on every threaded feature.

• 1
  Above 45 HRCGrind the thread. Cutting tools will not hold class.
• 2
  Wall under 1.5 × pitchDo not roll. Mill or turn instead.
• 3
  Printed threadsUse for fit checks only; cut functional threads.