Siemens SINUMERIK 828D Manual page 106

3.6
CYCLE832(tolerance, technology, ORI tolerance)
CYCLE832(0.05,12,0.5)
CYCLE832(0.01,_TOP_SURFACE_SMOOTH_OFF+_ORI_FINISH,0.1)
N10 T1 D1
N20 G54
N30 M3 S1200
N40 CYCLE832(0.1,3,1)
N50
N60 EXTCALL "CAM_ROUGH_0"
N65 CYCLE832(0,_OFF,1)
N70 CYCLE832(0.1,_ROUGH,1)
N80
N90 EXTCALL "CAM_ROUGH_1"
N95 CYCLE832(0,_OFF,1)
N100 CYCLE832(0.01,11,0.1)
N110
N120 ORISON
N130 EXTCALL "CAM_FINISH_0"
N135 CYCLE832(0,_OFF,1)
N140 CYCLE832(0.005,_ORI_FINISH,0.05)
N150
N160 ORISON
N170 EXTCALL "CAM_FINISH_1"
N180 CYCLE832(0,_OFF,1)
N200 M30
106
Important functions for 3- to 5-axis machining
Programming the cycle:
CYCLE832 for semi-finishing with tolerance 0.05 with orientation
smoothing and ORI tolerance 0.5.
CYCLE832 for finishing with 0.01 tolerance, Top Surface activated,
smoothing off and orientation smoothing with ORI tolerance 0.1
CYCLE832 Advanced Surface programming example
; Tool selection
; Select tool zero
; Clockwise spindle rotation and speed
; 3-axis program, tolerance value 0.1
; [3] = Roughing, [1] = Standard without ORI
; Call subprogram CAM_ROUGH_0
; Deselection CYCLE832
; 3-axis program, tolerance value 0.1
; [_ROUGH] = Roughing as plain text, [1] = Standard without ORI
; Call subprogram CAM_ROUGH_1
; Deselection CYCLE832
; 5-axis program (with orientation), tolerance value 0.01
; [11] = finishing, [0.1]= ORI tolerance 0.1
; Activation of the orientation smoothing
; call subprogram CAM_FINISH_0
; Deselection CYCLE832
; 5-axis program (with orientation), tolerance value 0.005
; [_ORI_FINISH] = finishing as plain text, [0.05]= ORI tolerance 0.05
; Activation of the orientation smoothing
; call subprogram CAM_FINISH_1
; Deselection CYCLE832
; End of program
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
Tolerance (chord tolerance)
Technology
0 = Deselection
1 = Finishing (_FINISH)
2 = Semi-finishing (_SEMIFIN)
3 = Roughing (_ROUGH)
11 = Finishing multi-axis program (_ORI_FINISH)
12 = Semi-finishing multi-axis program (_ORI_SEMIFIN)
13 = Roughing multi-axis program (_ORI_ROUGH)
1000000 = Top Surface without smoothing
2000000 = Top Surface with smoothing
ORI tolerance
Orientation tolerance or version identifier CYCLE832. Is required
when executing an HSC program on machines with dynamic
orientation transformation (e.g. 5-axis machining). Parameter
S_OTOL must be programmed. This also applies for applications
on 3-axis machines for programs without orientation of the tool
(S_OTOL = 1).