Siemens SINUMERIK 840D Programming Manual page 340

4
Turning Cycles
4.10 Extended stock removal cycle – CYCLE950 (SW 5.3 and higher)
Programming example 2
A simple inside contour is to be machined on the same
part as in sample program 1.
A center bore is made first using a diameter-10 drill.
Then, the inside contour is roughed parallel to the
contour, since the hole roughly corresponds to the end
contour.
This is done by defining a blank contour again for
inside machining.
The stock removal contour is located in the same
program as the cycle call in the blocks N400 to N420,
the blank contour in blocks N430 to N490.
Machining program:
%_N_EXAMPLE_2_MPF
;$PATH=/_N_WKS_DIR/_N_STOCK_REMOVAL_NEW_WPD
; Example 1: inside stock removal,
parallel to contour
; Sca, 01.04.99
;
; Tool offset data for turning tool,
inside
N100 $TC_DP1[2,1]=500 $TC_DP2[2,1]=6
$TC_DP6[2,1]=0.5 $TC_DP24[2,1]=60
N105 $TC_DP1[1,1]=200 $TC_DP3[1,1]=100
$TC_DP6[1,1]=5
N110 G18 G0 G90 DIAMON
N120 X300
N130 Z150
N140 T1 D1 M6
N150 X0
N160 Z100
N170 F500 S400 M3
N175 G1 Z75
N180 Z76
N190 Z60
N200 Z61
N210 Z45
N220 G0 Z100
N230 X300
N240 Z150
N250 T2 D1 M6
4-340
X
Change drill with diameter 10
Center drilling in three steps
Approach tool change point
Insert turning tool for inside machining
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
4
03.96
04.00
NP5
_NP6, _NP7
_NP2, _NP3
Z
© Siemens AG, 2002. All rights reserved