Program Structure For Milling - Siemens SINUMERIK 828D Manual

General information on workpiece production
2.3
CYCLE832 can be programmed in the main program or in thesubprogram for the geometry
data. Both versions are briefly described.
CYCLE832 in the main
For machining purposes, a main program is generated
program
main program calls one or more subprograms
of the workpiece. The tool change defines how the content is divided into subprograms.
MAINPROGRAM.MPF
Main program
N10
N20
N30
N40
N50
N60
N65
N70
N80
N90
N100
N110
N120
N130
N140
N150
N160
N170
N180
N190
Subprogram
CAM_rough.SPF subprogram
N10
N20
N30
...
N5046
N5047
N6580
Subprogram
CAM_finish.SPF subprogram
N10
N20
...
N5050
N5060
N6570
N6580
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling

Program structure for milling

1
T1 D1
M6
S10000 M3
G54
CYCLE832 (0.1,_ROUGH,1)
EXTCALL "CAM_rough"
5
CYCLE832(0,_OFF,1)
4
T2 D1
M6
S15000 M3
G54
TRAORI
ORIWKS ORIAXES
CYCLE832(0.005,_ORI_FINISH,0.5)
ORISON
EXTCALL "CAM_finish"
5
CYCLE832(0,_OFF,1)
4
M30
2
G0 X0 Y0 Z10
G1 Z0 F500
G1 X-1.45345 Y0.67878 F10000
...
G1 Z-2.13247 Y=0.34202 F800
...
M17
3
G0 X0 Y0 Z10 A3=0 B3=0 C3=0
G1 Z0 F500
...
G1 X7.60978 Y3.55541 A3=0.34202 B3=0 C3=-0.9396
G0 Z50 A3=0.34202 B3=0 C3=0.93969
TRAFOOF
M17
that includes all technology data. The
1
, that contain only the pure geometric data
2 3
; Tool change
; High Speed Settings
4
; Call subprogram
; Deselect CYCLE832
; Tool change
; Only for 5-axis
; Orientation reference and orientation;
; interpolation, switched optionally in CYCLE832
; High Speed Settings
4
; Orientation smoothing activation
; switched optionally already in CYCLE832
; Call subprogram
; Deselect CYCLE832
; End of program
2.3
6
29