Siemens SINUMERIK 828D Manual page 107

Important functions for 3- to 5-axis machining
CYCLE832 Top Surface programming example
N10 T1 D1
N20 G54
N30 M3 S1200
N40 CYCLE832(0.1,_TOP_SURFACE_SMOOTH_OFF+_ROUGH,1)
N50 ; 3-axis program, tolerance value 0.1, [_TOP_SURFACE_SMOOTH_OFF] = Top Surface active, smoothing off
N55 ; [_ROUGH] = roughing, [1] = standard without ORI
N60 EXTCALL "CAM_ROUGH_0"
N65 CYCLE832(0,_OFF,1)
N70 CYCLE832(0.05,_TOP_SURFACE_SMOOTH_OFF+_SEMIFIN,1)
N80 ; 3-axis program, tolerance value 0.05, [_TOP_SURFACE_SMOOTH_OFF] = Top Surface active, smoothing off
N85 ; [_SEMIFIN] = semi-finishing, [1] = standard without ORI
N90 EXTCALL "CAM_SEMIF_1"
N95 CYCLE832(0,_OFF,1)
N100 CYCLE832(0.001,_TOP_SURFACE_SMOOTH_ON+_ORI_FINISH,0.01)
N110 ; 5-axis program, tolerance value 0.001, [_TOP_SURFACE_SMOOTH_ON] = Top Surface active, smoothing on
N120 ; [_ORI_FINISH] = 5-axis finishing as plain text, [0.01]= ORI tolerance 0.01
N130 EXTCALL "CAM_FINISH_0"
N135 CYCLE832(0,_OFF,1)
N200 M30
Before the functions listed here can be used, the machine manufacturer must have
optimized the CNC machine correctly.
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
; Tool selection
; Select tool zero
; Clockwise spindle rotation and speed
; Call subprogram CAM_ROUGH_0
; Deselection CYCLE832
; Call subprogram CAM_SEMIF_1
; Deselection CYCLE832
; Call subprogram CAM_FINISH_0
; Deselection CYCLE832
; End of program
3.6
107