Siemens SINUMERIK 808D Programming And Operating Manual page 55

With the commands "G... X(U)... Z(W)... R... F... ;", a cycle for cutting taper threads is executed as per the sequence 1-4
given in the figure below.
The sign before the address character R depends on point A' of the viewing direction from point B. Since G92 (G78, G21) is
a modal G function, the thread cutting cycle is executed within the cycle by specifying only the cutting depth in the direction
of the X axis in the subsequent blocks. In these blocks G92 (G78, G21) need not be specified again.
Cycle for cutting a taper thread (G code system A):
When the cycle with G92 (G78, G21) is executed with activated single-block mode, the cycle does not wait on the halfway,
but stops after the end of the cycle, which comprises of the sequence 1-4.
The functions S, T and M, which are used as cutting conditions for the execution of G92 (G78, G21), are to be specified in
the blocks before the block G92 (G78, G21). When these functions are specified in a block with the travel of axes, then the
functions act only when the block is specified in the range of the operation with G92 (G78, G21).
If at the moment, when the cutting tool is at the starting point A or at the chamfering completion point B, the following key is
pressed, then the suspended cycle is executed once again from the beginning.
If the option "thread cutting feedrate halt" is not selected, then the thread cutting cycle is continued when the following key is
pressed during the execution of the thread cutting cycle. In this case the machining is halted till the tool is retracted again
after the completion of the thread cutting cycle.
Programming and Operating Manual (ISO Turning/Milling)
55
01/2017