G75 Cycle | Grooving and Parting Off

G75 Grooving Cycle

G75 is a CNC code and used to grooving for CNC lathe machines.

G75 grooving cycle also a very simple cycle, designed to break chips during a rough cut along the X axis used mainly for a grooving operation. The G75 cycle is identical to G74 cycle, except the X axis is replaced with the Z axis.

G75 Grooving Cycle Format

In CNC lathe, the G75 cycle can be written as one or two lines, depending on the model of the control unit. While a single line format is used in the old generation controls for G75 CNC Code, it is written in a two line format in the new generation control units. If your control unit is too old, you may consider the one-line (Type1) format, but if you are not sure which format to use, use the two-line (Type2) format. The “two-line” format is used in the control units that have been available on the market for the last 20-25 years.

G75 Grooving Cycle for Fanuc 6T/10T/11T/15T

The one-block programming format (Type1) for G75 cycle is:
G75 X…(U…) Z…(W…) I… K… D… F… S… ;

Parameters

X(U) : Final groove diameter to be cut
Z(W) : Z-position of the last groove (for multiple grooves only)
I : Depth of each cut (no sign)
K : Distance between grooves (no sign) (for multiple grooves only)
D : Relief amount at the end of cut (must be zero or not used for face groove)
F : Groove cutting feedrate (in/rev or mm/rev)
S : Spindle speed (ft/min or m/min)

G75 Grooving Cycle for Fanuc 0T/16T/18T/20T/21T

The two-block programming format (Type2) for G75 cycle is:
G75 R… ;
G75 X…(U…) Z…(W…) P… Q… R… F… S… ;

Parameters

First block:
R : Return amount (relief clearance for each cut)

Second block:
X(U) : Final groove diameter to be cut
Z(W) : Z-position of the last groove
P : Depth of each cut (no sign)
Q : Distance between grooves (no sign)
R : Relief amount at the end of cut (must be zero for face grooving)
F : Groove cutting feedrate (usually in/rev or mm/rev)
S : Spindle speed (usually ft/min or m/min)

Note: Do not confuse the R values written in the first line and the second line. Remembering that the R value described in the second line is not used in general, but only in special cases, will prevent you from making mistakes.

Note: If both the Z/W and Q (or K) are omitted in the cycle, the machining is along the X-axis only (peck grooving).

G75 CNC Code Format for Parting Off

G75 CNC Code can also be used for parting off operations by writing with fewer parameters.

The two-block programming format (Type2) for G75 CNC code for parting off:
G75 R… ;
G75 X… P… F… S… ;

Parameters

First block:
R : Return amount (relief clearance for each cut)

Second block:
X(U) : Final parting off diameter to be cut
P : Depth of each cut
F : Cutting feedrate (usually in/rev or mm/rev)
S : Spindle speed (usually ft/min or m/min)

G75 Grooving Cycle Examples

Grooving and Parting off Example with G75 Cycle

Grooving and Parting off Example with G75 Cycle

O3408;
T0505;
G50 S2500;
G96 M4 S90;
G0 X46 Z2 M8;
Z-13;
G75 R1;
G75 X30 Z-16 P2000 Q2800 F0.1;
G0 X46 Z-34;
G75 R1;
G75 X30 Z-37 P2000 Q2800 F0.1;
G0 X46 Z-55;
G75 R1;
G75 X30 Z-58 P2000 Q2800 F0.1;
G0 X200 Z200 M9;
T0909;
G50 S2500;
G96 M4 S90;
G0 X46 Z2 M8;
Z-71;
G75 R1;
G75 X0 P2000 F0.1;
G0 X200 Z200 M9;
M30;

Things to Know

  • P value should be written as microns in G75 CNC code. (If 8mm, P=8000)
  • Q value should be written as microns in G75 CNC code. (If 2,9mm, Q=2900)
  • G41 and G42 tool radius compensation cannot be used in the same block as the G75 cnc code.
  • X and Z values can be programmed either in the absolute or incremental mode.
  • Return amount (clearance for each cut) is only programmable for the two-block method. Otherwise, it is set by an internal parameter of the control system.
  • If the return amount is programmed (two-block method), and the relief amount is also programmed, the presence of X determines the meaning. If the X-value is programmed, the R-value means the relief amount.