Siemens SINUMERIK 808D Programming And Operating Manual page 60

R: (e), Retraction amount
This value is modal and remains effective till another value is programmed. The value can also be entered via USER DATA,
_ZSFI[31], but this value is overwritten by the value of the program command.
G71 P... Q... U... W... F... S... T...
P: Starting block for determining the contour
Q: Last block for determining the contour
U: Finishing allowance in X direction (Δu) (diameter -/radius programming)
W: Finishing allowance in Z direction (Δw)
F: Machining feedrate
S: Spindle speed
T: Select the tool
The F-, S- and T-functions printed within an NC program block and specified through the address characters P and Q are
ignored. Only the F-, S- and the T-functions specified in the block with G71 are effective.
Note
Stock removal cycle, longitudinal axis
Δd as well as Δu are specified with the address character U. When the address characters P and Q are specified, Δ"u" is
•
the case.
There are a total of four different cutting sectors. As shown in the figure below, Δ"u" and Δ "w" may have different signs:
•
Note
Stock removal cycle, longitudinal axis
In the block specified through the address P the contour is defined between the points A and A' (G00 or G01). No
•
traversing command can be specified in this block in the Z axis.
The contour defined between the points A' and B must either be a constantly rising or a constantly falling pattern on the
X axis as well as on the Z axis.
Within the range of the NC blocks specified with the address characters P and Q no subroutines can be called.
•
Type II
Contrary to Type I, a constant rise or a constant fall need not necessarily be specified for Type II i.e. pockets are also
possible.
60
Programming and Operating Manual (ISO Turning/Milling)
01/2017