Rough Drilling Sequence - Siemens SINUMERIK 840D Programming Manual

03.96
08.99
3
3.15 Pocket milling with islands - CYCLE73, CYCLE74, CYCLE75

Rough drilling sequence

In the first machining section of the rough drilling
operation, a REPEAT command must be used after a
modal call for the drilling cycle to call a sequence of
machining steps with the contents of CYCLE73 and the
contour repetition. The drilling cycle must be deselected
modally before the next tool change. Other drilling
technologies can be programmed subsequently.
The next program section contains CYCLE73 which
contains all necessary parameters as well as the
programs for solid machining and drilling.
Parameter _VARI is the only one to define all solid
machining parameters and it must always be
programmed for this reason.
The cycle now generates the solid machining and
drilling position programs for the pocket. It then calls the
drilling position program and executes it.
If the operation involves several different pockets, it will
be necessary to call the associated contours again in
this section. This block can be omitted if there is only
one pocket.
This entire machining section must be marked by a
skip command to the following "Solid machine
pocket" section.
Example
Rough drill, with solid machining
ACCEPTANCE4_CONT:
CYCLE74("EDGEA01", ,)
CYCLE75("ISL11A01", ,)
CYCLE75("ISL1A01", ,)
CYCLE75("ISL2A01", ,)
CYCLE75("ISL3A01", ,)
ENDLABEL:
T4 M6
D1 M3 F1000 S4000
MCALL CYCLE81(10,0,1,-3)
REPEAT ACCEPTANCE4_MACH
ACCEPTANCE4_MACH_END
MCALL
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
;Marker with name for beginning of pocket
;contour
;Definition of contour for pocket edge
;Definition of contour for 1st island
;Marker for end of a pocket contour
;Modal call of drilling cycle
;Execute drilling position program
;Deselect drilling cycle modally
Milling Cycles
3
3-191