Threading on a CNC Lathe: Single-Point, Thread Types & G76

Threading on a CNC Lathe

Cutting a thread on a CNC lathe is one of the most satisfying — and unforgiving — turning operations. Unlike drilling or facing, threading demands that the tool and spindle stay perfectly synchronised across many passes, each one deepening the same helical groove. Get the synchronisation, depth schedule, or tool geometry wrong and you produce a thread that won't gauge, strips under load, or galls a mating part. This guide covers single-point threading, the common thread standards used in Saudi workshops, and how the G76 cycle does the heavy lifting.

For pipe nipples, fittings, studs, and custom shafts, our precision turning & machining services cut both metric and imperial threads to gauge.

How single-point threading works

In single-point threading, a tool with a profile ground to the thread form is fed along the workpiece in time with spindle rotation. The control reads a spindle encoder so that every pass starts at exactly the same angular position — this is what keeps successive cuts in the same groove. The feed per revolution equals the thread pitch (or lead, on multi-start threads), so an M20 × 2.5 thread feeds the tool 2.5 mm per spindle revolution.

Because removing the full thread depth in one pass would overload the insert, threading is done in multiple passes of decreasing increment, sneaking up on the final crest-to-root depth.

Common thread types

Pipe threads (BSPT, NPT) are tapered, sealing on the flanks as they tighten — these are everywhere in oil, gas, and water systems across the Eastern Province and need the taper programmed into the toolpath.

The G76 threading cycle

Most modern Fanuc-style controls use G76, a two-block canned cycle that handles infeed automatically. A typical pair of blocks looks like:

G76 P010060 Q100 R0.05
G76 X18.4 Z-30.0 P1300 Q300 F2.0

• P010060 — one spring pass (01), 0° pull-out, 60° thread angle.
• Q100 — minimum cut depth (0.1 mm), so passes don't get vanishingly thin.
• R0.05 — finishing allowance.
• X18.4 / Z-30.0 — minor diameter and thread end Z.
• P1300 — total thread height (1.3 mm).
• Q300 — first-pass depth (0.3 mm).
• F2.0 — pitch (2.0 mm).

G76 uses a radial / flank infeed that loads only one side of the insert, keeping chips controlled and tool life longer than straight plunge infeed.

Choosing infeed method and pass count

• Radial (straight) infeed loads both flanks equally — simple but generates a tougher V-chip; fine for fine pitches.
• Flank infeed (built into G76) cuts on one flank, like turning, giving better chip flow on coarse pitches and stainless.
• Pass count: as a guide, fine pitches need 5–8 passes, coarse pitches 10–16. The control divides total depth so each pass removes roughly constant area, which is why early passes are deep and later ones shallow.

Practical tips from the floor

• Single-point inserts come as full-profile (cuts crest and root, pitch-specific) or partial-profile (one insert covers a pitch range but you must control major diameter separately). Full-profile gives the cleanest, gauge-correct thread.
• Cut the major diameter first to the correct turned size; the thread tool only forms the flanks and root.
• Leave a relief groove at the thread end so the tool has somewhere to retract — threading into a shoulder with no run-out groove risks a crash.
• Use a thread ring or plug gauge, not a mating part, to verify — a "go/no-go" check is the only honest test.
• Stainless and titanium work-harden; keep speed moderate, never let the tool dwell, and add a generous spring (no-cut) pass to clean the flanks.
• Coolant matters — flood threading coolant on aluminium and stainless prevents built-up edge that ruins the flank finish.

A safe starting sequence

1. Turn and chamfer the major diameter; cut the relief groove.
2. Select the insert and confirm it matches the pitch and profile.
3. Program G76 with pitch, depths, and a finishing allowance.
4. Run a single pass at a safe Z, dry, to confirm position.
5. Cut, gauge, and add a spring pass if the gauge is tight.

Conclusion

CNC threading rewards preparation: correct major diameter, the right insert profile, a relief groove, and a well-chosen G76 schedule. With the spindle encoder keeping every pass in the same groove, the operation becomes repeatable and reliable. For threaded shafts, fittings, and fasteners cut to metric or imperial gauge, see our precision turning & machining services or browse the Industrial Knowledge Base.