G74 Cycle | Peck Drilling and Face Grooving

G74 Canned Cycle

G74 Cycle is a CNC code and used to peck drilling and face grooving on CNC lathe machines.

Although the G74 CNC code is frequently used in the market to peck deep holes in CNC lathes, the variables used when writing the cycle can be written differently and can be used for face cutting and face grooving operations.

Peck Drilling with G74 CNC Code

With G74 Cycle, the cutting tool drills the hole with the cutting feedrate (F) during pecking and then quickly returns to the retraction distance (R) specified in the cycle. This movement continues until the hole depth reaches.

G74 Peck Drilling Cycle Format

G74 R… ;
G74 Z… Q… F… ;

Parameters

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

Second Block:
Z : Depth of hole
Q : Distance of each pecking
F : Cutting feedrate

Face Grooving with G74 CNC Code

Although the G74 Cycle is frequently used in the market to peck deep holes in CNC lathes, the variables used when writing the cycle can be written differently and can be used for face cutting and face grooving operations.

G74 Face Grooving Cycle Format

G74 R… ;
G74 X… Z… P… Q… F… ;

Parameters

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

Second Block:
X : Last groove diameter to be cut (For X axis and used if there is groove more than one.)
Z : Depth of groove (For Z axis)
P : Distance between grooves (For X axis and used if there is groove more than one. The value must be entered as a radius.)
Q : Distance of each pecking
F : Cutting Feedrate

G74 Cycle Examples

G74 Peck Drilling Cycle Program Example

G74 Peck Drilling Program Example for CNC Lathe

O1501;
T0202;
G97 M3 S3000;
G0 X0 Z3M8;
G1 Z-3 F0.1;
G0 Z3;
G0 X200 Z200 M9;
T0404;
G97 M3 S1700;
G0 X0 Z3 M8;
G1 Z-63 F0.1;
G0 Z3;
G0 X200 Z200 M9;
T0606; (Ø10 drill)
G97 M3 S850;
G0 X0 Z3 M8;
G74 R1.;
G74 Z-63. Q10000 F0.1;
G0 X200 Z200 M9;
M30;

G74 Single Grooving Cycle Program Example

G74 Single Face Grooving Cycle Program Example for CNC Lathe

Note: In this example, there is no need to use the X and P parameters since only one will be grooving.

N10 G00 X20.0 Z1.0;
G74 R1.0;
G74 Z-10.0 Q3000 F0.1;
G00 X200.0 Z200.0;
M30;

G74 Multi Grooving Cycle Program Example

G74 Multi Face Grooving Cycle Program Example for CNC Lathe

G50 S2000;
G96 S100 M03;
G00 X50.0 Z1.0 T0101;
G74 R1.0;
G74 X10.0 Z-10.0 P10000 Q3000 F0.1;
G00 X200.0 Z200.0;
M30;

Important Note: The reason we write Q3000 (3mm=3000 microns) and P10000 (10mm=10000 microns) in the examples is that these values must be entered in the system in microns. These values may have to be entered as mm in some machines. If you don’t know, please get information from the machine authorized service or from the booklets of the control unit.

Click here to see all examples for G74 Cycle!


Vote to create best CNC source on the web all together!
Do you think the content is understandable, good and contain everything?

  • :white_check_mark: Yes, the article perfect and enough.
  • :memo: No, it’s need to improve.

0 voters

(If a article voted mostly for “need to improve”, we moves article to development category and all members can add-edit to article to create best content. More details)