G76 is the multiple repetitive threading cycle — the most advanced and safest thread-cutting cycle in CNC lathe programming, in which the operator does not have to calculate each pitch and pass by hand; the control unit computes all the cutting steps automatically. Instead of writing depth of cut on each pass, the end chamfer and the finishing pass one by one with codes such as G32 or G92 when cutting straight, tapered, metric or inch threads with a single-point threading insert, G76 manages all of this with a single two-line block.
📷 IMAGE AREA — G76 threading: thread height, progressively decreasing passes, single-flank following and the thread-end chamfer
Suggested alt text: G76 multiple repetitive threading cycle pass diagram
1. The basic purpose and logic of the G76 cycle
When G76 is used, the control unit automatically calculates all the remaining roughing steps based on the thread height and the first pass depth; it performs automatic chamfering at the end of the thread so the thread runs out cleanly; and it applies a safe cutting algorithm that follows one flank of the thread angle (usually the 60° or 55° side face) to preserve insert life. This way a safe two-line block is used instead of long, error-prone lines.
2. The two-line standard FANUC G76 format and address details
G76 P(mmrra) Q(Δdmin) R(d) ;
G76 X(U) Z(W) R(i) P(k) Q(Δd) F(L) ;2.1 First-line address details
The first-line P address is a consecutive 6-digit code combination and by itself controls three vital functions:
| Digits | Function |
|---|---|
| First 2 digits (01–99) | How many times the finishing (final-size) pass is repeated as a spring pass. E.g. if 02 is written, after the thread reaches final size the tool makes 2 full spring passes without cutting to clean up spring-back and burrs. |
| Middle 2 digits (00–99) | The chamfer (run-out) amount at the thread end. The unit is 0.1 × pitch. E.g. if the pitch is 2 mm and 10 is written, the tool makes a safe 45° run-out from Z to X about 1 pitch (2 mm) before the thread end. |
| Last 2 digits | The insert / thread angle. Control units support six angles: 80°, 60°, 55°, 30°, 29° and 0°. Write 60 for metric threads, 55 for Whitworth (inch). |
Example: for 1 finishing pass, chamfer 1× pitch and a 60° thread angle, write P011060. The first-line Q is the minimum depth of cut; while the control reduces the passes automatically, the depth cannot go below this limit (no decimal, microns — e.g. Q100 for 0.1 mm). The first-line R is the finishing pass depth of cut; it can be written with a decimal (e.g. R0.05).
2.2 Second-line address details
| Address | Meaning |
|---|---|
| X(U) | The final diameter where the thread ends (thread root diameter). X is absolute, U incremental. |
| Z(W) | The absolute or incremental coordinate where the thread ends axially. |
| R(i) | On tapered threads, the radius difference between the start and end of the thread (taper amount). On straight threads it is omitted or R0 is written. |
| P(k) | The thread height (radius difference between crest and root). No decimal, microns — e.g. P1280 for 1.28 mm. |
| Q(Δd) | The first pass depth when threading begins. No decimal, microns — e.g. Q350 for 0.35 mm. |
| F(L) | The thread pitch. On metric threads it is the mm distance between two threads. |
3. FANUC parameters that directly affect the G76 cycle
If some values written in the G76 block are omitted in the program, or the default cutting algorithm is to be changed, the system parameters take over. These numbers can differ by control generation (Series 0, 0i-C, 0i-D).
| Parameter (0i-C/0i-D) | Function |
|---|---|
| No. 5130 — Thread chamfer time/distance | Takes over if the middle two digits (chamfer) of the first-line P address are omitted, or if the run-out acceleration at the thread end is to be changed; it sets how quickly / in what pitch ratio the tool moves from Z to X when it reaches the thread end. |
| No. 5141 — Minimum depth of cut (Δdmin) | If Q(Δdmin) is not written on the first line, the control does not error; the micron value in this parameter is taken automatically as the minimum cutting limit. |
| No. 5142 — Finishing allowance (d) | Sets the clean-up allowance left on the last pass when the first-line R(d) finishing depth is not defined. |
| No. 5143 — Thread pass-distribution type | Sets whether the passes are calculated with constant chip volume (the pass depth decreases automatically each step) or with constant depth of cut (equal plunge each step). By default, to preserve tool life, machines keep the chip load constant and reduce the pass depth progressively. |
4. Example program: straight metric thread (M30x2)
Let us cut a 2 mm pitch (M30x2) straight metric thread on a Ø30 mm cylindrical shaft, starting at Z5 and going to Z-40. Technical calculations: thread pitch F2.0. The thread height (radius) for a metric thread is about 1.226 mm → P1226. To make the first plunge safe, the first pass depth is 0.35 mm → Q350. The thread root diameter ≈ 30 – (2 × 1.226) = 27.548 mm → X27.548.
%
O7602 (MENTOR CNC - G76 METRIC THREADING) ;
G21 G18 G40 G99 ;
G50 S2000 ;
T0404 ;
G97 S800 M03 ; (G96 is NOT used for threading! G97 constant rpm is mandatory)
M08 ;
(SAFE START POINT BEFORE G76)
G00 X35.0 Z5.0 ;
(G76 CYCLE STARTS)
G76 P011060 Q100 R0.05 ;
G76 X27.548 Z-40.0 R0 P1226 Q350 F2.0 ;
(TOOL AUTOMATICALLY RETURNS TO X35 Z5)
G00 X200.0 Z200.0 M09 ;
M05 ;
M30 ;
%G76 P011060 Q100 R0.05— P01: 1 finishing pass, 10: chamfer 1× pitch, 60: 60° metric thread angle; Q100: min pass 0.1 mm; R0.05: finishing pass allowance.G76 X27.548 Z-40.0 R0 P1226 Q350 F2.0— root diameter Ø27.548, thread length Z-40, R0 straight thread, P1226 thread height (microns), Q350 first pass (microns), F2.0 pitch 2 mm.
📷 IMAGE AREA — M30x2 metric thread: crest Ø30, root Ø27.548, pitch 2 mm and the safe Z start (acceleration) distance
Suggested alt text: G76 M30x2 metric thread dimensions and start distance
5. Safe test and operator checklist
- G97 check: constant surface speed (G96) must absolutely not be active before the cycle. If the rpm fluctuates the pitch is spoiled; constant rpm must be given with
G97. - Z start distance: the thread start point must be at least 3–4 times the pitch away from the first thread face (if the pitch is 2, start at least at Z6.0–Z8.0). This acceleration distance is required for the axes to synchronise with the thread lead.
- Graphics simulation: on the first trial, dry-run without clamping the part or watch the tool path on the graphics screen.
Related tool: If the tool chatters or the insert breaks on coarse-pitch, trapezoidal or multi-start threads, the FANUC Macro Threading Simulator and NC Code Generator gives you a load-split pass plan and ready-to-check G32 code.