Path Milling - Cycle72 - Siemens Sinumerik 840D sl Programming Manual

16.1.27

Path milling - CYCLE72

Programming
CYCLE72(STRING[141] _KNAME, REAL _RTP, REAL _RFP, REAL _SDIS, REAL
_DP, REAL _MID, REAL _FAL, REAL _FALD, REAL _FFP1, REAL _FFD, INT
_VARI, INT _RL, INT _AS1, REAL __LP1, REAL _FF3, INT _AS2, REAL _LP2,
INT _UMODE, REAL _FS, REAL _ZFS, INT _GMODE, INT _DMODE, INT _AMODE)
Parameters
Param Param
No.
Mask intern
1
_KNAME
2
RP _RTP
3
Z0 _RFP
4
SC _SDIS
5
Z1 _DP
6
DZ _MID
7
UXY _FAL
8
UZ _FALD
9
FX _FFP1
10
FZ _FFD
11
_VARI
Job planning
Programming Manual, 02/2011, 6FC5398-2BP40-1BA0
Explanation
Name of the contour subroutine
Retraction plane (abs)
Reference point of tool axis (abs)
Safety clearance (to be added to reference point, enter without sign)
End point, final depth (abs/inc), see _AMODE
Maximum depth infeed (inc; enter without sign)
Finishing allowance, plane (inc), allowance at edge contour
Finishing allowance depth (inc), allowance at base (enter without sign)
Feedrate on contour
Feedrate for depth infeed (or spatial infeed)
Machining type
UNITS: Machining
1 = Roughing
2 = Finishing
5 = Chamfer
TENS:
0 = Intermediate travel with G0
1 = Intermediate travel with G1
HUNDREDS:
0 = Retraction at the end of contour to reference point
1 = Retraction at the end of contour to reference point +_SDIS
2 = Retraction by _SDIS at the end of contour
3 = No retraction at the end of contour, approach next start point with contour feed
THOUSANDS: Reserved
TEN THOUSANDS:
0 = Machine contour forward
1 = Machine contour backward
Restrictions with backward machining:
• Max 170 contour elements (including chamfers or rounding)
• Only values in the (X/Y) and F planes are evaluated
Programming cycles externally
16.1 Technology cycles
791