HEIDENHAIN TNC 620 User Manual page 347

D18 – Reading system data
With the D18 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.
Values read from the function D18 are always output
in metric units.
Group name, ID no.
Program information, 10
System jump addresses, 13
Machine status, 20
Channel data, 25
Cycle parameter, 30
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
Number Index
3 -
103 Q parameter-
number
1 -
2 -
3 -
1 -
2 -
3 -
4 -
5 -
7 -
8 -
9 -
10 -
11 -
1 -
1 -
2 -
3 -
Additional functions
Meaning
Number of the active fixed cycle
Relevant within NC cycles; for inquiry as
to whether the Q parameter given under
IDX was explicitly stated in the associated
CYCLE DEF .
Label jumped to during M2/M30 instead of
ending the current program
Value = 0: M2/M30 functions normally
Label jumped to in the event of FN14:
ERROR with the NC CANCEL reaction
instead of aborting the program with an error
message. The error number programmed in
the FN14 command can be read under ID992
NR14.
Value = 0: FN14 has the normal effect.
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.
Active tool number (without index)
Prepared tool number (without index)
Active tool axis
0=X, 1=Y, 2=Z, 6=U, 7=V, 8=W
Programmed spindle speed
Active spindle condition: -1=not defined,
0=M3 active,
1=M4 active, 2=M5 after M3, 3=M5 after
M4
Gear range
Coolant status: 0=off, 1=on
Active feed rate
Index of prepared tool
Index of active tool
Channel number
Set-up clearance of active fixed cycle
Drilling depth or milling depth in active fixed
cycle
Plunging depth of active machining cycle
9
9.8
347