Siemens SINUMERIK 840D Programming Manual page 302

4
Turning Cycles
4.5 Stock removal cycle – CYCLE95
Programming example 1
Stock removal cycle
The contour illustrated in the figure explaining the
assignment parameters must be machined
completely (longitudinal, outside). Axis-specific final
machining allowances have been defined. No
interruption between cuts has been programmed.
The maximum infeed is 5mm.
The contour is stored in a separate program.
DEF STRING[8] UPNAME
N10 T1 D1 G0 G18 G95 S500 M3 Z125 X81
UPNAME="CONTOUR_1"
N20 CYCLE95 (UPNAME, 5, 1.2, 0.6, , ->
-> 0 .2, 0.1, 0.2, 9, , , 0.5)
N30 G0 G90 X81
N40 Z125
N50 M30
PROC CONTOUR_1
N100 G1 Z120 X37
N110 Z117 X40
N120 Z112
N130 G1 Z95 X65 RND=5
N140 Z87
N150 Z77 X29
N160 Z62
N170 Z58 X44
N180 Z52
N190 Z41 X37
N200 Z35
N210 G1 X76
N220 M17
-> Must be programmed in a single block
4-302
X
P6 (35,76)
P4 (52,44)
P5 (41,37)
Definition of a variable for the contour name
Approach position before cycle call
Assignment of subroutine name
Cycle call
Reapproach to starting position
Traverse in each axis separately
End of program
Beginning of contour subroutine
Traverse in each axis separately
Rounding with radius 5
Traverse in each axis separately
End of subroutine
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
4
03.96
12.98
P2 (87,65)
P1 (120,37)
P3 (77,29)
Z
© Siemens AG, 2002. All rights reserved