Siemens SINUMERIK 840D sl Programming Manual page 330

Path action
11.2 Continuous-path mode (G64, G641, G642, G643, G644, G645, ADIS, ADISPOS)
NOTICE
If a rounding movement initiated by G641, G642, G643, G644 or G645 is interrupted, the
starting or end point of the original traversing block (as appropriate for REPOS mode) will be
used for subsequent repositioning (REPOS), rather than the interruption point.
Example
The two outside corners on the groove are to be approached exactly. Otherwise machining
should be performed in continuous-path mode.
Program code
N05DIAMOF
N10 G17 T1 G41 G0 X10 Y10 Z2 S300 M3
N20 G1 Z-7 F8000
N30 G641 ADIS=0.5
N40 Y40
N50 X60 Y70 G60 G601
N60 Y50
N70 X80
N80 Y70
N90 G641 ADIS=0.5 X100 Y40
N100 X80 Y10
N110 X10
N120 G40 G0 X-20
N130 Z10 M30
330
Comment
; Radius as dimension.
; Approach starting position, activate
spindle, path compensation.
; Tool infeed.
; Contour transitions are smoothed.
; Approach position exactly with exact
stop fine.
; Contour transitions are smoothed.
; Deactivate path compensation.
; Retract tool, end of program.
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Fundamentals