Siemens SINUMERIK 808D ADVANCED - Page 174

Programming and Operating Manual (Milling)
174 6FC5398-4DP10-0BA1, 01/2014
Programming example 1: Milling around a closed contour externally
This program is used to mill the contour shown in the diagram below.
Parameters for the cycle call:
Parameter
Description
Value
_RTP Retraction plane 250 mm
_RFP Reference plane 200 mm
_SDIS Safety clearance 3 mm
_DP Infeed depth 175 mm
_MID Maximum infeed depth 10 mm
_FAL Finishing allowance in the plane 1 mm
_FALD Finishing allowance in depth 1.5 mm
_FFP1 Feedrate in the plane 800 mm/min
_FFD Feedrate depth infeed 400 mm/min
_VARI Machining type 111 (Roughing up to finishing allowance;
intermediate paths with G1, for intermediate
paths retraction in Z to _RFP + _SDIS)
Parameters for approach:
_RL G41 - left of the contour, i.e. external machining 41
_LP1 Approach and retraction in a quadrant in the plane 20 mm radius
_FF3 Retraction feedrate 1000 mm/min
N10 T3 D1
; T3: Milling cutter with radius 7
N20 S500 M3 F3000
; Program feedrate and spindle speed
N30 G17 G0 G90 X100 Y200 Z250 G94
; Approach start position
N40 CYCLE72("EX72CONTOUR", 250, 200, 3, 175, 10,1, 1.5,
800, 400, 111, 41, 2, 20, 1000, 2, 20)
; Cycle call
N50 X100 Y200
N60 M2
; End of program
EX72CONTOUR.SPF ; Subroutine for contour milling (for
example)
N100 G1 G90 X150 Y160
; Starting point of contour
N110 X230 CHF=10
N120 Y80 CHF=10