HEIDENHAIN TNC 320 User Manual page 51

Enter Retract the tool: Press the orange axis key Z
in order to get clear in the tool axis, and enter the
value for the position to be approached, e.g. 250.
Confirm with the ENT key
Confirm Radius comp.: RL/RR/no comp? by
pressing the ENT key: Do not activate the radius
compensation
Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)
Miscellaneous function M? Enter M2 to end the
program and confirm with the END key: The TNC
saves the entered positioning block
Example NC blocks
0 BEGIN PGM C200 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 5 Z S4500
4 L Z+250 R0 FMAX
5 PATTERN DEF
POS1 (X+10 Y+10 Z+0)
POS2 (X+10 Y+90 Z+0)
POS3 (X+90 Y+90 Z+0)
POS4 (X+90 Y+10 Z+0)
6 CYCL DEF 200 DRILLING
Q200=2 ;SET-UP CLEARANCE
Q201=-20 ;DEPTH
Q206=250 ;FEED RATE FOR PLNGNG
Q202=5 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=-10 ;SURFACE COORDINATE
Q204=20 ;2ND SET-UP CLEARANCE
Q211=0.2 ;DWELL TIME AT BOTTOM
7 CYCL CALL PAT FMAX M13
8 L Z+250 R0 FMAX M2
9 END PGM C200 MM
Further information on this topic
Creating a new program: See "Opening programs and entering",
page 85
Cycle programming: See User's Manual for Cycles
TNC 320 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
Programming the first part
Definition of workpiece blank
Tool call
Retract the tool
Define the machining positions
Define the cycle
Spindle and coolant on, call the cycle
Retract the tool, end program
1
1.3
51