HEIDENHAIN TNC 640 (34059x-05) - Manual (Page 320)

Programming: Q Parameters
9.8 Additional functions
9
320
TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 1/2015
FN 18: SYSREAD: Reading system data
With the
FN 18: SYSREAD function you can read system data and
store them in Q parameters. You select the system data through a
group name (ID number), and additionally through a number and an
index.
Group name, ID no. Number Index Meaning
Program information, 10 3 - Number of the active fixed cycle
103 Q parameter
number Relevant within NC cycles; for inquiry as
to whether the Q parameter given under
IDX was explicitly stated in the associated
CYCLE DEF.
System jump addresses, 13 1 - Label jumped to during M2/M30 instead
of ending the current program. Value = 0:
M2/M30 has the normal effect
2 - Label jumped to if FN14: ERROR after
the NC CANCEL reaction instead of
aborting the program with an error. The
error number programmed in the FN14
command can be read under ID992 NR14.
Value = 0: FN14 has the normal effect.
3 - Label jumped to in the event of an internal
server error (SQL, PLC, CFG) instead
of aborting the program with an error
message. Value = 0: Server error has the
normal effect.
Machine status, 20 1 - Active tool number
2 - Prepared tool number
3 - Active tool axis
0=X, 1=Y, 2=Z, 6=U, 7=V, 8=W
4 - Programmed spindle speed
5 - Active spindle condition: -1=not defined,
0=M3 active,
1=M4 active, 2=M5 after M3, 3=M5 after
M4
7 - Gear range
8 - Coolant status: 0=off, 1=on
9 - Active feed rate
10 - Index of prepared tool
11 - Index of active tool
Channel data, 25 1 - Channel number