G75 Cycle | Grooving and Parting Off

In this article, we describe how to use G75 cycle for grooving in CNC lathe machines with all details and examples.

0
2402

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
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;

 

“Click here to see all G75 Grooving Cycle Examples”

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.

Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleG74 Cycle | Peck Drilling and Face Grooving
Next articleG73 Cycle | Pattern Repeating