Siemens SINUMERIK 808D User Manual page 198

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:
Pa rameter D e scription
_RTP Retraction plane
_RFP Reference plane
_SDIS Safety clearance
_DP Infeed depth
_MID Maximum infeed depth
_FAL Finishing allowance in the plane
_FALD Finishing allowance in depth
_FFP1 Feedrate in the plane
_FFD Feedrate depth infeed
_VARI Machining type
Parameters for approach:
_RL G41 - left of the contour, i.e. external machining
_LP1 Approach and retraction in a quadrant in the plane
_FF3 Retraction feedrate
N10 T3 D1
N20 S500 M3 F3000
N30 G17 G0 G90 X100 Y200 Z250 G94
N40 CYCLE72("EX72CONTOUR", 250, 200, 3, 175, 10,1, 1.5,
800, 400, 111, 41, 2, 20, 1000, 2, 20)
N50 X100 Y200
N60 M2
EX72CONTOUR.SPF
N100 G1 G90 X150 Y160
N110 X230 CHF=10
N120 Y80 CHF=10
N130 X125
N140 Y135
N150 G2 X150 Y160 CR=25
N160 M2
198
Va lue
250 mm
200 mm
3 mm
175 mm
10 mm
1 mm
1.5 mm
800 mm/min
400 mm/min
111 (Roughing up to finishing allowance;
intermediate paths with G1, for intermediate
paths retraction in Z to _RFP + _SDIS)
41
20 mm radius
1000 mm/min
; T3: Milling cutter with radius 7
; Program feedrate and spindle speed
; Approach start position
; Cycle call
; End of program
; Subroutine for contour milling (for
example)
; Starting point of contour
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017