G75 Multiple Repetitive Grooving and Cut-Off Cycle: Format, Parameters, Alarm

G75 is a multiple repetitive grooving cycle used on FANUC-controlled CNC lathes to cut a groove wider than the tool width or to cut safely in deep grooves by breaking the chip. G75 both breaks the chip by pecking in the radial direction (X axis) and automatically clears wide grooves by shifting sideways by the tool width in the axial direction (Z axis).

📷 IMAGE AREA — G75 wide grooving: radial pecking (X), bottom relief and sideways shift in Z
Suggested alt text: G75 multiple repetitive grooving cycle diagram

1. The basic purpose and working logic of G75

When a groove wider than the tool width must be cut in one operation, or when deep grooves must be cut safely by breaking the chip, the G75 multiple repetitive grooving cycle is used. The most common applications are:

Cutting wide and deep ring/groove channels on the outside diameter,
Inside-diameter (in-bore) grooving operations,
Safely parting off the workpiece with a cut-off blade after machining (part-off),
Radial pecking on hard materials to prevent the chip from continuously coming off and wrapping around the tool.

2. The two-line standard FANUC G75 format and parameter details

On current FANUC control systems (0i-C, 0i-D, 21i-B, etc.) the G75 cycle is programmed in two lines:

G75 R(e) ;
G75 X(U) Z(W) P(Δi) Q(Δk) R(Δd) F(f) ;

Address	Technical name	Meaning and input format
R(e) on the first line	Radial retract amount	How many mm the tool retracts upward to break the chip after each plunge (peck). Written with a decimal (e.g. R0.5). If omitted, the default value in parameter 5139 is active.
X(U)	Groove bottom diameter	The final diameter to which the groove descends. X is absolute; U is incremental from the start point.
Z(W)	Groove width limit	The Z point where the groove ends. Z is absolute, W incremental. If a single groove is cut with no sideways shift, Z is not written.
P(Δi)	X-axis peck amount	The X depth of cut on each plunge. No decimal point; written in microns; a radius value. For 2 mm pecking, P2000.
Q(Δk)	Z-axis sideways step	How far the tool shifts in Z to the next pass. No decimal, in microns. For 1.5 mm shift, Q1500. Must be chosen smaller than the tool width.
R(Δd) on the second line	Safety clearance at the groove bottom	The safe relief amount when the groove reaches the bottom or on sideways-shift returns. Its sign is always positive. If Z(W) and P are not written, this R sets the support direction in the cutting direction.
F(f)	Feed rate	Cutting feed in mm/rev. Because grooving inserts are delicate, it is set lower than in normal turning (e.g. F0.08).

3. Step-by-step working algorithm of the G75 cycle

When the machine reads the G75 command line, it automatically follows this sequence:

Approach to the start point: the tool first positions at the safe start point (point A) written by the programmer before G75. This point must be larger than the part outside diameter and at the groove-start Z surface.
Radial plunge and pecking: the tool plunges in X by P(Δi) from the first line, then retracts upward by R(e) from the first line to break the chip. This repeats until the target X bottom diameter is reached.
Dwell at the bottom and relief: when the groove bottom is reached (it dwells if G04 is in the program), the tool moves slightly away from the groove bottom by R(Δd) from the second line and rapidly (G00) returns to the start X level.
Axial sideways shift: the tool shifts sideways in Z by the Q(Δk) distance.
Loop repeat: at the new position it pecks down again; this continues until the final limit dimension in Z is reached.
Return to the start point: once the whole width is cleared, the tool automatically returns to the first safe point A where the cycle was called.

4. Fully detailed OD wide-grooving program example

Let us cut, on a Ø68 mm shaft, an outside-diameter groove starting at Z-25 and extending to Z-45 (20 mm wide) with a Ø50 mm bottom diameter. The groove tool (insert) width is 4 mm. Critical calculations: the groove starts at Z-25 and is 20 mm wide, so the end is Z = -25 + (-20) = -45 mm; Z-45.0 is written directly. Sideways shift (Q): the tool width is 4 mm; to make the corners overlap and not leave a straight wall, always shift by less than the tool width — 3 mm is chosen for safe chip evacuation → Q3000. Pecking (P): radial 1.5 mm → P1500.

%
O7501 (MENTOR CNC - G75 WIDE GROOVING TRAINING) ;
G21 G18 G40 G99 ;
G50 S1200 ;
T0303 ;
G96 S100 M03 ;
M08 ;
(SAFE START POINT BEFORE G75)
G00 X72.0 Z-25.0 ;
(G75 CYCLE STARTS)
G75 U0.8 R0.5 ;
G75 X50.0 Z-45.0 P1500 Q3000 R0.1 F0.08 ;
(CYCLE DONE, TOOL RETURNS TO X72 Z-25)
G00 X150.0 Z150.0 M09 ;
M05 ;
M30 ;
%

G50 S1200 limits the maximum spindle speed to 1200 rpm for safety; G96 S100 M03 100 m/min constant surface speed.
G00 X72.0 Z-25.0 for a Ø68 part, a safe X72 and the groove-start position Z-25.
G75 U0.8 R0.5 U0.8 retract allowance at the groove ends, R0.5 chip-break retract on each plunge.
G75 X50.0 Z-45.0 P1500 Q3000 R0.1 F0.08 bottom diameter Ø50, Z limit -45, radial 1.5 mm pecking, axial 3 mm sideways step, bottom clearing relief 0.1 mm, feed 0.08 mm/rev.

📷 IMAGE AREA — G75 wide-groove example: Ø68 raw diameter, Ø50 bottom, Z-25/Z-45 groove limits and the tool-width / sideways-shift relationship
Suggested alt text: G75 OD wide grooving example dimensions

5. G75 inside-diameter (in-bore) grooving rules

If a single groove is cut (no sideways shift), the Z and Q addresses on the second line are removed entirely; the machine pecks down and up at a single point. In the bore the logic is the same, but the start point must be smaller than the bore diameter. Vital rules for in-bore ring grooves or channels:

Start-point check: before G75 is called the tool must be positioned inside the bore (at a smaller diameter). If the bore is Ø40 mm, the start should be X36.0 or X37.0.
X-axis direction: in the bore the tool moves from the centre outward, so the target X is always larger than the start X (e.g. from X36 to the X44 bottom diameter).
Chip-packing risk: chips cannot be expelled easily inside the bore; choosing the first-line retract R(e) a little larger (e.g. R0.8) helps the chip break and fall out.

6. G75 grooving cycle alarm and troubleshooting list

P/S 065 (no G00/G01 in the first block): occurs when a linear positioning move is not given right before G75. Make sure the line before the cycle contains a clear coordinate such as G00 X.. Z...
P/S 067 (MDI mode error): multiple repetitive cycles including G75 cannot be run directly in MDI mode. Write the cycle in a program in EDIT mode and run it in MEMORY/AUTO mode.
Slope or step left on the groove walls: if the Q sideways shift is written larger than the tool insert width (W_tool), the machine leaves material between passes and the tool can break. Always check the Q < W_tool condition.
Axis crash or excessive-plunge alarms: check whether a decimal point was accidentally added to the end of the P or Q value. The point-free micron format is mandatory.

Mentor CNC Safety Notice
This page is training content prepared by Mentor CNC. The G75 programs, parameter numbers, calculation examples and alarm descriptions here are for training purposes. The model of the FANUC control, the software version, the increment system, the G-code system and the machine builder settings can change the behaviour of the same command. Before running the program, it must be checked that the P and Q values are without a decimal and suit the input unit, that Q is chosen smaller than the tool width, that the two R addresses are used for the correct purpose, and that the bottom diameter/Z limit are correct. The first trial must be run with graphics, machine lock, dry run, single block and a low feed override. CNC and PMC parameters must only be changed by trained and authorised persons, with a backup of the current values taken first. A wrong program or parameter setting can cause damage to the tool, the workpiece or the machine, and serious injury.