HEIDENHAIN TNC 620 (73498x-02) - Manual (Page 212)

Programming: Programming contours
6.5 Path contours – Polar coordinates
6
212
TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013
Example: Helix
0 BEGIN PGM HELIX MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
Definition of workpiece blank
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S1400
Tool call
4 L Z+250 R0 FMAX Retract the tool
5 L X+50 Y+50 R0 FMAX Pre-position the tool
6 CC
Transfer the last programmed position as the pole
7 L Z-12,75 R0 F1000 M3 Move to working depth
8 APPR PCT PR+32 PA-182 CCA180 R+2 RL F100
Approach the contour on a circular arc with tangential
connection
9 CP IPA+3240 IZ+13.5 DR+ F200 Helical interpolation
10 DEP CT CCA180 R+2 Depart the contour on a circular arc with tangential
connection
11 L Z+250 R0 FMAX M2 Retract the tool, end program
12 END PGM HELIX MM