Key functions for 5-axis machining
3.6
© Siemens AG All rights reserved. SINUMERIK, Manual, 5-axis machining
66
Notes 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.
Programming example
for CYCLE832
Before the functions listed here can be used, the machine manufacturer must have opti-
mized the CNC machine correctly.
CYCLE832(0.01,112103) Programming of the cycle with a tolerance
such as 0.01 and transformation parameters.
CYCLE832() Abbreviated program call. Corresponds to
selecting the "Machining" "Deselection" input
screen.
CYCLE832(0.01) Abbreviated program call. Entry of the toler-
ance value. The active G commands are not
changed in the cycle.
N10 T1 D1 ; Activate TRAFO
N20 G54 ; Select tool zero
N30 M3 S1200 ; Clockwise spindle rotation and speed
N40 CYCLE832(0.05,112103) ; 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
N50 EXTCALL "CAM_ROUGH" ; Call subprogram CAM_ROUGH
N60 CYCLE832(0.005,112101) ; 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
N70 EXTCALL "CAM_FINISH" ; Call subprogram CAM_FINISH
N80 M03
NOTE
To Next Page
Loading...
Need help?
General
