HEIDENHAIN TNC 640, User Manual, Page: 706 / 948

Turning | Turning program functions (option 50)
16
706
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
Procedure
To write a simultaneous program, proceed as follows:
Activate turning mode
Insert a turning tool.
Adjust the coordinate system with Cycle 800
Activate
FUNCTION TCPM
with
REFPNT TIP-CENTER
Activate radius compensation with RL / RR
Program simultaneous turning contour
Finish radius compensation with Departure block or R0
Reset
FUNCTION TCPM
Example
0 BEGIN PGM TURNSIMULTAN MM
...
12 FUNCTION MODE TURN
Activate turning mode
13 TOOL CALL "TURN_FINISH"
Insert a turning tool.
14 FUNCTION TURNDATA SPIN VCONST:OFF S500
15 M140 MB MAX
16 CYCL DEF 800 ADJUST XZ SYSTEM
Adapting the coordinate system
Q497=+90 ;PRECESSION ANGLE
Q498=+0 ;REVERSE TOOL
Q530=+0 ;INCLINED MACHINING
Q531=+0 ;ANGLE OF INCIDENCE
Q532= MAX ;FEED RATE
Q533=+0 ;PREFERRED DIRECTION
Q535=+3 ;ECCENTRIC TURNING
Q536=+0 ;ECCENTRIC W/O STOP
17 FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS
REFPNT TIP-CENTER
Activate FUNCTION TCPM
18 FUNCTION TURNDATA CORR-TCS:Z/X DRS:-0.1
19 L X+100 Y+0 Z+10 R0 FMAX M304
20 L X+45 RR FMAX
Activate radius compensation with RR
...
26 L Z-12.5 A-75
Program simultaneous turning contour
27 L Z-15
28 CC X+69 Z-20
29 CP PA-90 A-45 DR-
30 CP PA-180 A+0 DR-
...
47 L X+100 Z-45 R0 FMAX
Cancel radius compensation with R0
48 FUNCTION RESET TCPM
Reset FUNCTION TCPM
49 FUNCTION MODE MILL
...
71 END PGM TURNSIMULTAN MM