Siemens SINUMERIK 808D Programming And Operating Manual page 59

G code
G77
G78
Note
In the cycle descriptions given above, the G code system A and B are assumed.
Note
Consider the following USER DATA setting requirements when calling a cycle with G71/G72:
_ZSFI[36] = 0: G71/G72 works with additional contour cut.
•
_ZSFI[36] = 1 (default): G71/G72 works without additional contour cut.
•
_ZSFI[35] = 0 (default): G71/G72 works with G41/G42 for roughing and finishing and traverses a two-cut distance in the
•
cycle.
_ZSFI[35] = 1: G71/G72 works with G40 for roughing and traverses a one-cut distance in the cycle.
•
Stock removal cycle, longitudinal axis (G71)
By using the fixed cycles the number of steps in the programming can be reduced considerably owing to the fact that the
roughing and the finishing cycles can be determined simply by determining the finishing cut form and the like. There are two
different types of stock removal cycle.
Type I
The specified area is machined with finishing allowance through Δd (infeed depth during stock removal). Always when the
contours A are written to A' to B by an NC Program, u/2 and Δw continue to be present.
Cutting path of a stock removal cycle, longitudinal axis:
Format
G71 U... R... ;
U: Infeed depth during stock removal (Δd), radius programming
This value is modal and remains effective till another value is programmed. The value can also be entered via USER DATA,
_ZSFI[30], but this value is overwritten by the value of the program command.
Programming and Operating Manual (ISO Turning/Milling)
01/2017
Description
Multiple repetitive grooving cycles in the transverse axis
Multiple thread cutting cycle
59