Thread manufacturing

Why it matters

Threads hold machines together and turn rotation into precise linear motion (lead screws, ball screws, micrometers). Billions of fasteners are rolled every year, while lead screws and gauges are ground; choosing the right method decides strength, accuracy and cost, and setting a lathe for the right lead is a basic shop-floor skill.

Key ideas

Thread terms (ISO metric, 60° V-thread)

• Major diameter d (nominal size, e.g. M20), minor diameter (root of the bolt d3, crest of the nut D1) and pitch (effective) diameter d2, where thread and groove widths are equal.
• Pitch P = axial distance between adjacent threads; lead L = axial advance in one revolution; for an n-start thread L = n·P.
• Fundamental triangle height H = 0.866·P; basic profile dimensions follow from it (see Formulas). Standard designation: M20 × 2.5 (coarse pitch is implied when omitted, e.g. M20 = 2.5 mm pitch). Inch threads are specified in threads per inch (TPI): P = 25.4/TPI mm.

Thread cutting on a lathe (single-point screw cutting)

• The carriage is driven by the lead screw through change gears (or a quick-change gearbox) so that the tool advances exactly one lead per spindle revolution. The half-nut is engaged; a thread-chasing dial lets the operator re-engage at the right position on each pass.
• The tool is ground to the thread form (60° for metric), set square to the work with a centre gauge, and the depth is reached in several passes. Feeding the compound slide at about 29–30° makes the tool cut mainly on one flank and reduces chatter.
• Flexible, cuts any pitch, internal or external, multi-start (index the work by 360°/n or advance the tool by one pitch between starts), but slow.

Taps and dies — taps cut internal threads (taper, intermediate/second and plug/bottoming taps used in sequence for blind holes); dies cut external threads. The hole is first drilled with the tap drill, roughly D − P for metric threads. Self-opening die heads and collapsible taps on automatics avoid reversing.

Thread milling — a single-form disc cutter (for long, large-pitch threads such as lead screws) or a multi-form cutter (short threads, one revolution of the work plus a little overlap); on CNC machines, helical interpolation with a thread mill cuts internal threads of any diameter above the tool size.

Thread grinding — a single-rib or multi-rib wheel dressed to the thread form; used after hardening for gauges, taps, lead screws and precision threads; the most accurate method. Centreless thread grinding is used for headless set screws.

Thread rolling — a cold-forming process: the blank is rolled between flat reciprocating dies, or two or three cylindrical dies, which displace material into the thread form. No chips, very high production rates, unbroken grain flow, work-hardened roots and compressive residual stress, so fatigue strength is higher than for cut threads. The blank diameter is approximately the pitch diameter, because metal displaced from the grooves forms the crests. Limited to ductile materials (elongation of more than about 12 %) and external threads mainly; hardness is limited (roughly up to about 40 HRC).

Other methods: thread whirling (fast, for bone screws and long screws), casting and moulding, die casting and plastic moulding of threads.

Formulas

• L = n·P — lead, mm; n = number of starts.
• P = 25.4 / TPI — pitch in mm for an inch thread.
• H = 0.866·P — height of fundamental triangle.
• d2 = d − 0.6495·P — pitch diameter, mm.
• D1 = D − 1.0825·P — basic minor diameter of the internal (nut) thread, mm.
• d3 = d − 1.2269·P; h3 = 0.6134·P — minor diameter and thread depth of the external (bolt) thread, mm.
• Tap drill ≈ D − P — mm (about 75 % thread engagement for ISO coarse threads; take exact sizes from a data book).
• Driver teeth / Driven teeth = Lead to be cut / Lead of lead screw — simple change-gear train (intermediate idlers do not change the ratio).
• t = L_thread / (L·N) — time for one cutting pass, min; L_thread threaded length in mm, L lead in mm/rev, N spindle speed in rev/min.

Worked examples

Example 1 (standard) — dimensions and change gears for M20 × 2.5.

1. H = 0.866·P = 0.866 × 2.5 = 2.165 mm.
2. d2 = 20 − 0.6495 × 2.5 = 18.376 mm.
3. d3 = 20 − 1.2269 × 2.5 = 16.933 mm; depth h3 = 0.6134 × 2.5 = 1.534 mm.
4. D1 = 20 − 1.0825 × 2.5 = 17.294 mm; tap drill ≈ 20 − 2.5 = 17.5 mm.
5. Lathe lead screw 6 mm pitch: driver/driven = 2.5/6 = 5/12 = 50/120 (50-tooth gear on the spindle stud, 120-tooth on the lead screw).

Example 2 (GATE level) — cutting a two-start thread. A two-start external metric thread of pitch 2 mm and threaded length 50 mm is cut on a lathe at 80 rev/min with a 6 mm lead screw. The radial infeed per pass is 0.1 mm; the return stroke takes as long as the cutting stroke. Find the change gears and the total machining time.

1. Lead L = n·P = 2 × 2 = 4 mm. Gear ratio = 4/6 = 2/3 = 40/60.
2. Thread depth h3 = 0.6134 × 2 = 1.227 mm → passes per start = ⌈1.227/0.1⌉ = 13.
3. Time per stroke t = 50/(4 × 80) = 0.15625 min.
4. Total strokes = 2 starts × 13 passes × 2 (cut + return) = 52.
5. Total time = 52 × 0.15625 = 8.125 min. Note that the tool feeds one lead (4 mm), not one pitch, per revolution.

Common mistakes

• Setting the change gears for the pitch of a multi-start thread instead of its lead.
• Treating 1/TPI as millimetres; it is inches — multiply 25.4 by 1/TPI.
• Using D − 1.0825P (nut minor diameter) for the bolt root; the bolt minor diameter is d − 1.2269P.
• Choosing the major diameter as the rolling blank size; it is close to the pitch diameter.
• Expecting rolled threads on brittle cast iron or hardened steel — rolling needs ductility.
• Disengaging the half-nut at a random point and re-engaging without the chasing dial — the tool will split the thread.

For GATE PI

• MCQs: rolling vs cutting (strength, grain flow, chips, blank size), which process for hardened/precision threads, multi-start threads.
• NAT on lead, change-gear ratios, pitch and minor diameters, tap-drill sizes, number of passes and threading time.
• Links: thread measurement (wire method) is in metrology; lathe screw cutting links to the lathe topic.

Quick check

1. A three-start thread has a pitch of 1.5 mm. What is its lead?
2. Pitch of a 16 TPI thread in mm?
3. Change gears to cut 1.75 mm pitch with a 6 mm lead screw?
4. Approximate blank diameter for rolling M16 × 2?
5. Why are rolled threads stronger in fatigue?

Answers: 1. 4.5 mm. 2. 25.4/16 = 1.5875 mm. 3. 1.75/6 = 7/24 = 35/120. 4. About the pitch diameter, 16 − 0.6495 × 2 ≈ 14.70 mm. 5. Unbroken grain flow, work-hardened roots and compressive residual stresses.