G76 Threading Cycle Simulator and NC Code Generator (FANUC Lathe)

With this free G76 threading cycle simulator and NC code generator you can enter the nominal thread diameter and pick a standard (pitch and angle fill in automatically), set the first pass depth and finish allowances, watch the live toolpath simulation and instantly generate the FANUC 0i-TC compatible two-block G76 program. For the theory see our G76 Threading Cycle guide, for the simple single-block alternative the G92 Threading Simulator, and for thread calculation the Thread Calculator.

What the G76 threading cycle does and when to use it

G76 is the FANUC multiple repetitive threading cycle. You give it the major diameter, the minor (root) diameter, the lead and the first pass depth; the control works out the number of passes, the depth of every pass and the flank infeed, then cuts the whole thread from one two-block command. Doing the same job with G92 means writing every pass by hand.

G76 is the right choice for a CNC threading cycle program when:

• The pitch is 1.5 mm (16 TPI) or coarser — the pass count grows quickly and hand-written G92 blocks become long and error-prone.
• You want flank (angled) infeed — G76 shifts the tool along the thread angle (29–30°) on every pass so the chip comes off one flank and chatter drops.
• The part runs in production — all threading parameters sit in two blocks, so the program is easy to read, check and adjust at the machine.

G92 or G76? Decision table

Rule of thumb: under 1.5 mm pitch with 3–4 passes, G92 is fine; anything coarser, use G76. You can try the single-block version in the G92 Threading Cycle Simulator.

How to use the simulator step by step

1. Nominal diameter and standard: enter the major diameter and pick metric, UN or Whitworth. Pitch and thread angle fill in automatically; overwrite the pitch for a special thread.
2. Thread start and end Z: start at least 2–3 pitches in front of the face (e.g. Z3 to Z5) so the slide reaches full feed before the first turn; the end Z is the end of the thread length. With no relief groove, set a pull-out chamfer with r.
3. First pass depth Δd: 0.3–0.6 mm in steel, 0.5–0.8 mm in aluminium. This value sets the pass count (see the √n rule below).
4. Minimum pass depth Q: the floor for the ever-shallower passes near the root. Stay above 0.05–0.1 mm; below that the insert rubs and the flank finish suffers.
5. Finish allowance R and spring passes m: R 0.03–0.08 mm, m usually 1. For a critical flank finish set m=2 and let the last pass run "empty".
6. Vc, n and G50: the simulator derives rpm from Vc but writes a constant spindle speed (G97) into the code. Cap the chuck speed with G50; rpm must not change while threading.
7. Run the simulation, download the code: watch each pass depth and the flank infeed in the live toolpath, download the .nc file and prove it out in single block before cutting metal.

Reading the two blocks the simulator generates

G76 P(m)(r)(a) Q(Δdmin) R(d) ;
G76 X(U) Z(W) R(i) P(k) Q(Δd) F(L) ;

For the link between these addresses and the FANUC parameters (No. 5130, 5140–5145) and for the single-block FS10/11 format, see the G76 Threading Cycle guide; here we only cover what you need to read the generated code.

How the pass depth is distributed: the √n rule

G76 removes a constant chip area on every pass. Because the thread groove widens as it gets deeper, the passes get progressively shallower. The total depth of pass n, measured from the crest:

d(n) = Δd × √n        →   number of passes ≈ (k / Δd)²

Two practical consequences. First, halving Δd quadruples the pass count, so do not make Δd needlessly small on a coarse pitch. Second, once the calculated pass drops below Q(Δdmin) the control clamps it to Δdmin; a large Δdmin therefore makes the last passes deeper than you expect.

Worked example: M20×2.5 external thread, 35 mm long

A 2.5 mm pitch metric thread on Ø20 bar. Thread height k = 0.6134 × 2.5 = 1.534 mm; minor diameter X = 20 − 2 × 1.534 = 16.93 mm. First pass 0.5 mm, minimum pass 0.1 mm, finish allowance 0.05 mm, one spring pass, one-lead pull-out. With those values the simulator generates:

O0076 ;
G21 G40 G99 ;
T0303 ;                     (60° external threading insert)
G97 S900 M03 ;              (constant rpm - never G96 for threading)
G00 X26.0 Z5.0 M08 ;        (two pitches in front of the face)
G76 P011060 Q100 R0.05 ;    (m=01, r=1.0 lead, a=60°)
G76 X16.93 Z-35.0 P1534 Q500 F2.5 ;
G00 X100.0 Z100.0 M09 ;
M30 ;

Pass distribution the control calculates (radius values from the crest):

Roughing stops at 1.48 mm (thread height minus finish allowance) and the spring pass takes the last 0.05 mm. The first pass removes 0.5 mm, the ninth only 0.07 mm, yet the chip area is the same on every pass. If the insert chips on the first pass, the problem is not the pass count but Δd being too large for the nose radius: drop Δd to 0.4 and accept the extra passes.

Taper and multi-start threads

Taper threads (NPT, BSPT): R(i) in the second block is the radius difference between the thread start and end: R(i) = (D − d) / 2. The sign is positive when the tool touches the small diameter first and negative when it touches the large diameter first; an external taper thread cut from large to small diameter is therefore usually written with R-.

Multi-start threads: the G76 blocks stay the same; only the start Z of each extra start is shifted by lead / number of starts. On an M16×4 P2 thread (two starts, 4 mm lead) the first start begins at Z0 and the second at Z2, with F4 in both calls. The same cycle is simply called twice from different start points. For the full calculation of multi-start and taper threads use the Thread Calculator and NC Program Generator.

Typical alarms and shop-floor problems

Six common mistakes

• Writing P(k) and Q with a decimal point. These addresses take microns: P1534 for 1.534 mm, Q500 for 0.5 mm. P1.534 gives you a thread 1.5 microns deep.
• Using the nominal diameter as X. X is the minor diameter, not the major. For M20×2.5 it is X16.93, not X20.
• Threading in constant surface speed. Never thread under G96; the changing rpm ruins the lead.
• r=00 with no relief groove. The tool runs into the shoulder. Without a groove use a pull-out of at least one lead.
• Mixing up the two Q addresses. Q in the first block is the minimum pass depth, Q in the second is the first pass depth; both in microns, different meanings.
• First run at full speed. Prove a new program in single block at 50% rapid with the tool offset clear of the part and watch the toolpath.

Frequently asked questions

Which FANUC controls run the code this simulator generates?

The two-block format runs on FANUC 0i-T (0i-TB/TC/TD/TF), 16i/18i/21i-T and 30i/31i/32i-T. FS10/11 and some Mitsubishi controls use a single-block G76 with A, D, K and I instead of the Q and P addresses. Compare with the G76 example in your machine's programming manual before the first run.

Can G76 cut internal threads?

Yes. X then becomes the major diameter of the internal thread and the start X sits inside the minor diameter; the control reads the infeed direction from the sign of the X move. Use a short, rigid internal threading bar and reduce Δd by about 30% compared with an external thread.

Why is the thread height 0.6134 × pitch?

That is the practical depth for a 60° external metric thread cut with a sharp-point (partial profile) insert. Full-profile inserts use the manufacturer's catalog value, typically around 0.54–0.58 × pitch. You can overwrite the thread height in the simulator; check with a thread gauge and adjust the last pass accordingly.

Is G76 enough for trapezoidal (Tr) threads?

With a 30° angle G76 will cut a trapezoidal thread, but on 6–8 mm pitches the groove is so wide that even flank infeed does not lower the insert load enough. For those jobs use the FANUC Macro Threading tool, which splits the groove in both depth and width.