HEIDENHAIN TNC 320 User Manual page 258

6
Programming contours
6.5 Path contours – Polar coordinates
Example: Helix
0 BEGIN PGM HELIX MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S1400
4 L Z+250 R0 FMAX
5 L X+50 Y+50 R0 FMAX
6 CC
7 L Z-12.75 R0 F1000 M3
8 APPR PCT PR+32 PA-182 CCA180 R+2 RL F100
9 CP IPA+3240 IZ+13.5 DR+ F200
10 DEP CT CCA180 R+2
11 L Z+250 R0 FMAX M2
12 END PGM HELIX MM
258
Definition of workpiece blank
Tool call
Retract the tool
Pre-position the tool
Transfer the last programmed position as the pole
Move to working depth
Approach the contour on a circular arc with tangential
connection
Helical interpolation
Depart the contour on a circular arc with tangential
connection
Retract the tool, end program
HEIDENHAIN | TNC 320 | Conversational Programming User's Manual | 9/2016