HEIDENHAIN TNC 620 (81760x-02) ISO programming - Manual (Page 247)

Path contours – FK free contour programming (option 19) 6.6
6
TNC 620 | User's ManualDIN/ISO Programming | 2/2015
247
Example: FK programming 1
%FK1 G71*
N10 G30 G17 X+0 Y+0 Z-20*
Definition of workpiece blank
N20 G31 X+100 Y+100 Z+0*
N30 T 1 G17 S500*
Tool call
N40 G00 G90 Z+250 G40 M3* Retract the tool
N50 G00 X-20 Y+30 G40* Pre-positioning the tool
N60 G01 Z-10 G40 F1000* Move to working depth
N70 APPR CT X+2 Y+30 CCA90 R+5 G41 F250* Approach the contour on a circular arc with tangential
connection
N80 FC DR- R18 CLSD+ CCX+20 CCY+30* FK contour section:
N90 FLT* Program all known data for each contour element
N100 FCT DR- R15 CCX+50 CCY+75*
N110 FLT*
N120 FCT DR- R15 CCX+75 CCY+20*
N130 FLT*
N140 FCT DR- R18 CLSD- CCX+20 CCY+30*
N150 DEP CT CCA90 R+5 F2000*
Depart the contour on a circular arc with tangential
connection
N160 G00 X-30 Y+0*
N170 G00 Z+250 M2*
Retract the tool, end program
N99999999 %FK1 G71*