Siemens SINUMERIK 808D Programming And Operating Manual page 63

Note
Stock removal cycle transverse axis
The contour between the points A and A' is defined through the block specified with the address character P (G00 or
•
G01). No traversing command can be specified in this block in the X 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.
The machining is executed with the cycle with the command G73 and the specification of P and Q. The four cutting
•
sectors will be discussed in more detail below. Please pay special attention to the signs of Δu, Δw, Δk and Δi. As soon as
the execution cycle has ended, the tool returns to the point A.
Closed cutting cycle (G73)
The closed cutting cycle G73 is more effective, when a workpiece is machined, which has a form similar to that in the
finishing cut i.e. cast-iron or forged workpieces.
Cutting path in the closed cutting cycle:
Format
G73 U... W... R... ;
U: Distance (Δi) from the starting point to the current tool position in the direction of the X axis (in radius programming).
This value is modal and remains effective till another value is programmed. The value can also be entered via USER DATA,
_ZSFI[32], but this value is overwritten by the value of the program command.
W: Distance (Δk) from the starting point to the current tool position in the direction of the Z axis.
This value is modal and remains effective till another value is programmed. The value can also be entered via USER DATA,
_ZSFI[33], but this value is overwritten by the value of the program command.
R: Number of cuts parallel to the contour (d).
This value is modal and remains effective till another value is programmed. The value can also be entered via USER DATA,
_ZSFI[34], but this value is overwritten by the value of the program command.
G73 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 of the X axis (Δu) (diameter -/radius programming)
W: Finishing allowance in the direction of Z axis (Δw)
F: Machining feedrate
S: Spindle speed
Programming and Operating Manual (ISO Turning/Milling)
01/2017
63