Siemens SINUMERIK 840D Programming Manual page 171

03.96
08.99
3
%_N_MYKONTUR_SPF
;$PATH=/_N_SPF_DIR
N100 G1 G90 X150 Y160
N110 X230 CHF=10
N120 Y80 CHF=10
N130 X125
N140 Y135
N150 G2 X150 Y160 CR=25
N160 M17
Programming example 2 (SW 5.2 and later)
Milling round the outside of a closed contour as
described in sample program 1, with the contour
defined in the calling program
$TC_DP1[20,1]=120 STC_DP6[20,11]=7
N10 T20 D1
N15 M6
N20 S500 M3 F3000
N25 G17 G0 G90 G94 X100 Y200 Z250 ->
CYCLE72 ( "START:END", 250, 200, ->
-> 3, 175, 10,1, 1.5, 800, 400, 11, ->
-> 41, 2, 20, 1000, 2, 20)
N30 G0 X100 Y200
N35 GOTOF END
START:
N100 G1 G90 X150 Y160
N110 X230 CHF=10
N120 Y80 CHF=10
N130 X125
N140 Y135
N150 G2 X150 Y160 CR=25
END:
N160 M02
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
3.12 Path milling - CYCLE72
Subroutine for contour milling (for example)
Start point of contour
T20: milling cutter with radius 7
Changing tool T20
Program feedrate and spindle speed
Approach starting position, cycle call
Milling Cycles
3
3-171