Siemens CNC Lathe | G78 – G92 Cycle | Thread Cutting

In this article, we describe how to use G92 (G78 or G21) for thread cutting in Siemens CNC controlled turning (lathe) machines with all details and examples.

0
676

Thread Cutting Introduction

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. It’s called as G92 most of time but also possible as G78 or G21 in Siemens CNC controller.

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

You may be interested also:
“Siemens CNC Lathe | G77 and G90 Cycle | Cutting”

Straight Thread Cutting 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.

Straight Thread Cutting Example

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

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 cycleThe 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.

Tapered Thread Cutting Format

G… X… Z… R… F… ;
F = Designation of thread lead (L)

Tapered Thread Cutting Example

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

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


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 articleSiemens CNC Lathe | G77 – G90 Cycle | Cutting
Next articleSiemens CNC Lathe | G79 – G94 Cycle | Facing