+1 vote
2.2k views
in cnc programming by (9.9k points)

In this article, we describe with examples how to use G92 and G78 cycle to thread cutting on CNC lathe machines which is controlled by Siemens.

For thread cutting operations, four kinds of thread cutting cycles are provided – two kinds of straight thread cutting cycles and two kinds of tapered thread cutting cycles.

Straight Thread Cutting Cycle

With the commands indicated above, straight thread cutting cycle 1 to 4, shown in Fig. 4-6, is executed.
The cycle code can be change due to pre-selected G code system as below ( Selected by machine tool builder by parameter setting).
G code system A = G92
G code system B = G78
G code system C = G21

Fig. 4-6 Straight thread cutting cycle

Format

G… X(U)… Z(W)… F… ;

F = Designation of thread lead (L)
Since G92 (G78, G21) is a modal G code, thread cutting cycle is executed by simply specifying depth of cut in the X-axis direction in the succeeding blocks. It is not necessary to specify G92 (G78, G21) repeatedly in these blocks.

Example

Fig. 4-7 Straight thread cutting cycle (G code system B)

Example of programming
N30 G00 X80. Z76.2 Mxx; Mxx : Thread chamfering ON
N31 G78 X66.4 Z25.4 F6. ;
N32 X65. ;
N33 X63.8 ;
N34 X62.64 ;
N35 G00 X100. Z100. Myy; Myy : Thread chamfering OFF

It is recommended to program the sequence that turns ON and OFF the “thread chamfering input” by using appropriate M codes.

Tapered Thread Cutting Cycle

With the commands of “G… X(U)… Z(W)… R… F… ;” tapered thread cutting cycle of 1 to 4 as shown in Fig. 4-8 is executed.
The cycle code can be change due to pre-selected G code system as below ( Selected by machine tool builder by parameter setting).
G code system A = G92
G code system B = G78
G code system C = G21

Fig. 4-8 Tapered thread cutting cycle

The sign of address R is determined by the direction viewing point A’ from point B. Since G78 (G92, G21) is a modal G code, thread cutting cycle is executed by simply specifying depth of cut in the X-axis direction in the succeeding blocks. It is not necessary to specify G78 (G92, G21) repeatedly in these blocks.

Format

G… X… Z… R… F… ;

Example

Fig. 4-9 Tapered thread cutting cycle (G code system A)

Example of programming

N50 G00 X80. Z80.8 Mxx ; Mxx : Thread chamfering ON
N51 G92 X70. W–50.8 I–1.5 F2. ;
N52 X68.8 ;
N53 X67.8 ;
N54 G00 X100. Z100. Myy ; Myy : Thread chamfering OFF

Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.
...