Siemens Sinumerik 802D sl Programming Manual page 106

Enhanced Level Commands
4.1 Program support functions (1)
Format
G72 W... R... ;
The meaning of addresses W (Δd) and R (e) are basicly the same as U and R in
the G71 cycle.
G72 P... Q... U... W... F... S... T... ;
The meaning of addresses P, Q, U (Δu), W (Δw), F, S, and T are the same as
those in the G71 cycle.
Contour repetition (G73)
The G73 contour repetition cycle is more effective when machining a workpiece
that has a similar shape to the finishing shape, like a cast and forged workpieces.
Programmed contour: A → A'
Fig. 4-20
Format
G73 U... W... R... ;
U: Distance (Δi) in the X axis direction from the start point to the current tool posi-
tion (radius designation). This value is modal and can also be preset using GUD7,
ZSFI[32]. The value set here can be overwritten by the NC program command.
W: Distance (Δk) in the Z axis direction from the start point to the current tool posi-
tion. This value is modal and can also be preset using GUD7, ZSFI[33]. The value
set here can be overwritten by the NC program command.
R: Number of cuts parallel to the contour (d).
This value is modal and can also be preset using GUD7, ZSFI[34]. The value set
here can be overwritten by the NC program command.
4-106
B
Cutting path in contour repetition
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Δk + Δw
Δw
D
Δu/2
C
A
(R)
Δu/2
A'
Δw
© SIEMENS AG 2007 All rights reserved
04.07
Δi + Δu/2