Siemens SINUMERIK 840D Manual page 66

3.6
Notes
Programming example
for CYCLE832
66
Key functions for 5-axis machining
CYCLE832 is based on the use of G1 blocks.
In the event of changes, you should use the tolerance value specified in the CAM program as
a guide. Tolerances that are lower than the one specified there are not practical.
CYCLE832 programming
Ideally, you should program CYCLE832 in the higher-level NC master program that then calls the
geometry program. This means that you can apply the cycle to the complete geometry or -
depending on the transparency of the CAM program - to individual program sections or free-form
surfaces.
CYCLE832(0.01,112103)
CYCLE832()
CYCLE832(0.01)
N10 T1 D1
N20 G54
N30 M3 S1200
N40 CYCLE832(0.05,112103)
N50 EXTCALL "CAM_ROUGH"
N60 CYCLE832(0.005,112101)
N70 EXTCALL "CAM_FINISH"
N80 M03
Before the functions listed here can be used, the machine manufacturer must have opti-
mized the CNC machine correctly.
© Siemens AG All rights reserved. SINUMERIK, Manual, 5-axis machining
Programming of the cycle with a tolerance
such as 0.01 and transformation parameters.
Abbreviated program call. Corresponds to
selecting the "Machining" "Deselection" input
screen.
Abbreviated program call. Entry of the toler-
ance value. The active G commands are not
changed in the cycle.
; Activate TRAFO
; Select tool zero
; Clockwise spindle rotation and speed
; Tolerance value 0.05
; From right to left
; (Tol,decimal places 76543210)
; 0 [3] = roughing, 1 [0]= no function
; 2 [1] = TRAORI, 3 [2] = G642
; 4 [1] = FFWON SOFT, 5 [1] = COMPCAD
, 6 and 7 not used
; Call subprogram CAM_ROUGH
; Tolerance value 0.005
; From right to left
; (Tol,decimal places 76543210)
; 0 [1] = finishing, 1 [0]= no function
; 2 [1] = TRAORI, 3 [2] = G642
; 4 [1] = FFWON SOFT, 5 [1] = COMPCAD
, 6 and 7 not used
; Call subprogram CAM_FINISH