Siemens SINUMERIK 840D Programming Manual page 208

3
Milling Cycles
3.15 Pocket milling with islands – CYCLE73, CYCLE74, CYCLE75
GOTOF ACCEPTANCE4_MACH_END
ACCEPTANCE4_MACH:
;REPEAT ACCEPTANCE4_CONT ENDLABEL
CYCLE73(1015,"ACCEPTANCE4_DRILL","ACCEPTANCE4_M
ILL1","3",10,0,1,-12,0,,2,0.5,,9000,400,0,,,,)
ACCEPTANCE4_MACH_END:
T3 M6
D1 M3 S2000
;REPEAT ACCEPTANCE4_CONT ENDLABEL
CYCLE73(1011,"ACCEPTANCE4_DRILL","ACCEPTANCE4_M
ILL1","3",10,0,1,-12,0,,2,0.5,,9000,400,0,,,,)
Sequence for roughing, solid machining
(_VARI=XXX1)
All parameters must be written to the CYCLE73
command again.
The program performs the following machining
steps:
• Approach a manually calculated or automatically
generated start point located on the return plane. G0
is then used to traverse the axis to a reference plane
brought forward by the safety distance.
• Infeed to the current machining depth according
to the selected insertion strategy (_VARI) with
feed value _FFD.
• Mill pocket with islands down to final machining
allowance with feed _FFP1. The machining
direction corresponds to the setting in _CDIR.
The pocket can be split if the ratio between mill
diameter and clearance between islands or
between islands and edge contours is not ideal.
For this purpose, the cycle calculates additional
start points for mill insertion.
• Lift off in accordance with selected retraction
mode and return to start point for next plane
infeed.
3-208
;Branch to Solid machine pocket
;Start of section Generate programs
;Required only if there is more than one pocket
;contour
;End of section Generate programs
;Required only if there is more than one pocket
;contour
;Solid machine pocket
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
08.99
© Siemens AG, 2002. All rights reserved