Siemens SINUMERIK 808D User Manual page 199

Programming example 2: Milling around a closed contour externally
With this program, the same contour is milled as in example 1. The difference is that the contour programming is now in the
calling program.
N10 T3 D1
N20 S500 M3 F3000
N30 G17 G0 G90 X100 Y200 Z250 G94
N40 CYCLE72 ( "PIECE245:PIECE245E", 250, 200, 3, 175, 10,1,
1.5, 800, 400, 11, 41, 2, 20, 1000, 2, 20)
N50 X100 Y200
N60 M2
N70 PIECE245:
N80 G1 G90 X150 Y160
N90 X230 CHF=10
N100 Y80 CHF=10
N110 X125
N120 Y135
N130 G2 X150 Y160 CR=25
N140 PIECE245E:
N150 M2
Programming example 3
Proceed through the following steps:
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
1. Select the desired operating area.
2. Open the vertical softkey bar for available milling cycles.
3. Press this softkey to open the window for CYCLE72. Enter a name in the first input field.
4. Press one of the following two softkeys . The program automatically jumps to the program
editor screen form.
If you desire to edit and store the contour in a subroutine, press this softkey.
; T3: Milling cutter with radius 7
; Program feedrate and spindle speed
; Approach start position
; Cycle call
; Contour
; End of contour
199