G92 is the threading canned cycle — a single canned cycle that reduces the approach, cut, radial retract from the part and rapid return moves of thread cutting to a single line in CNC lathe programming. Instead of writing codes such as G00, G32 and G01 one by one for each longitudinal thread pass, G92 simplifies the process by having the tool follow a rectangular or trapezoidal motion template.
📷 IMAGE AREA — G92 threading cut model: X plunge (rapid), Z cut synchronised with the pitch, radial retract and rapid return to the start length
Suggested alt text: G92 threading canned cycle four-move diagram
1. The basic purpose and cut model of the G92 cycle
When the G92 command line is read, the cutting tool performs the following four automatic moves in sequence from the start point:
- Move (rapid – R): plunges in X to the programmed target thread-pass diameter (G00).
- Move (cut – F): cuts up to the specified Z length at the thread pitch (F) speed, fully synchronised with the spindle rotation.
- Move (rapid – R): when the thread length (final Z) is reached, it retracts radially and rapidly outward from the thread profile.
- Move (rapid – R): at G00 speed it automatically returns to the first safe start length where the cycle was called (travelling back in Z).
G92 is a modal code. Once the cycle is called, writing only the decreasing new X diameter values on the following lines makes the machine keep threading automatically at the same length (Z) and the same pitch (F).
2. Cycle code name by G-code system (A/B/C)
Depending on the FANUC configuration (A, B or C code systems), the code name of this canned cycle changes:
| Code system | Threading cycle code |
|---|---|
| System A (most common) | G92 |
| System B | G78 |
| System C | G21 |
On the vast majority of industrial machines System A (G92) is active; however, when a program is taken from another machine, the code system must always be verified.
3. Standard syntax and address details
A) Straight (cylindrical) threading:
G92 X(U)_ Z(W)_ F_ Q_ ;
B) Taper (tapered / pipe-type) threading:
G92 X(U)_ Z(W)_ I_ F_ ;| Address | Function |
|---|---|
| X | The absolute target diameter where the thread pass ends (reduced toward the root on each line). |
| U | The incremental radial distance relative to the start point. |
| Z | The absolute final axial coordinate where the thread ends. |
| W | The incremental axial length relative to the start point. |
| I | On tapered threads, the taper difference of the section narrowing toward the end along the X axis (radius). Omitted on straight threads. |
| F | The thread pitch (mm distance between two threads). |
| Q | On multi-start threads, the shift of the thread-start angle (angular offset). Not written on single-start threads. |
4. System parameters that directly affect the G92 cycle
4.1 Thread-end run-out curve and smoothing parameter
Related parameter (0i-C / 0i-D): No. 5130 (thread chamfer / run-out time). When the tool reaches the final Z coordinate, if it stops suddenly and lifts in X, a notch or insert-tip breakage can occur at the thread end. This parameter sets how damped and smoothly the X and Z axes separate at the end of G92, as a millisecond value or pitch multiplier.
4.2 Data-clearing rule in canned cycles
While in G92 mode, if any one-shot G code other than dwell (G04) or a G90/G94 command from Group 01 is issued, the control clears the modal Z, W and modal F feed data belonging to G92 from memory entirely for safety. If threading is to be resumed, all addresses must be defined again.
4.3 Tool-nose radius compensation rule
While the G92 cycle runs, tool-nose radius compensation (G41 / G42) can be excluded from the calculation by the system, or, depending on the control generation, subjected to the same compensation parameter bit as G71–G76 (No. 5102#4 RFC). Because the tip geometry of threading inserts is special, cancelling compensation with G40 before the cycle is recommended for machining safety.
5. Fully detailed example program (M30x2 metric thread)
Let us cut a 2 mm pitch (M30x2) straight metric thread on a Ø30 mm cylindrical shaft, from Z-2.0 to a length of Z-40.0. For a metric 2 mm pitch, the single-flank thread height is about 1.226 mm; the root diameter ≈ 27.54 mm. Thanks to the modal structure, after the first pass only the decreasing X diameter values are written.
%
O9201 (G92 METRIC THREADING PROGRAM) ;
G21 G18 G40 G99 ;
G50 S1500 ;
T0202 ;
G97 S700 M03 ; (G97 constant rpm is MANDATORY for threading! G96 spoils the pitch)
M08 ;
(SAFE APPROACH POINT BEFORE G92)
G00 X34.0 Z5.0 ; (Part O30, safe X34 and Z5 in front of the thread)
(G92 CYCLE FIRST PASS)
G92 X29.4 Z-40.0 F2.0 ;
(MODAL REPEAT: ONLY DECREASING DIAMETER PASSES)
X29.0 ;
X28.6 ;
X28.2 ;
X27.8 ;
X27.54 ; (Final root diameter reached)
(EXIT G92 MODE)
G00 X200.0 Z200.0 M09 ;
M05 ;
M30 ;
%📷 IMAGE AREA — M30x2 metric thread: crest Ø30, root ≈Ø27.54, pitch 2 mm and the decreasing X29.4→X27.54 pass distribution
Suggested alt text: G92 M30x2 decreasing thread passes and root diameter
6. Safe test and operator checklist
- G97 requirement: if G96 (constant surface speed) stays active before G92, the rpm changes as the tool approaches the centre; the changing rpm distorts axis acceleration, spoils the pitch and scraps the thread. G97 must absolutely be used.
- Acceleration (approach) distance: the thread start point must not be chosen too close to the part zero. So the axes can synchronise with the spindle rotation and catch the pitch, start at least 3–4 pitches away (about 6–8 mm ahead for a 2 mm pitch).
- Manual data-entry risk: because you set the diameter on each G92 pass, do not plunge after roughing without measuring the real diameter with a caliper/micrometer and setting the first pass to that diameter.
🖥️ Related tool: G92 Threading Simulator and NC Code Generator →
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.