HEIDENHAIN TNC 410 - Manual (Page 228)

215 HEIDENHAIN TNC 410
FN 18: SYS-DATUM READ
Reading system data
With the function FN18: SYS-DATUM READ you can read system
data and store them in Q parameters. You select the system data
through a group number (ID number),and additionally through a
number and an index.
1
0.7 A
dditional F
unctions
Group name, ID No. Number Index System data
Program information, 10 1 – MM/inch condition
2 – Overlap factor for pocket milling
3 – Number of active fixed cycle
Machine status, 20 1 – Active tool number
2 – Prepared tool number
3 – Active tool axis
0=X, 1=Y, 2=Z
4 – Programmed spindle rpm
5 – Active spindle status: 0=off, 1=on
6 – Active spindle orientation angle
7 – Active gear range
8 – Coolant status: 0=off, 1=on
9 – Active feed rate
10 – Active feed rate for transition arc
Data from the tool table, 50 1 – Tool length
2 – Tool radius
4 – Oversize for tool length DL
5 – Oversize for tool radius DR
7 – Tool inhibited (0 or 1)
8 – Number of replacement tool
9 – Maximum tool age TIME1
10 – Maximum tool age TIME2
11 – Current tool age CUR. TIME
12 – PLC status
13 – Maximum tooth length LCUTS
14 – Maximum plunge angle ANGLE
15 – TT: Number of teeth CUT
16 – TT: Wear tolerance for length LTOL
17 – TT: Wear tolerance for radius RTOL
18 – TT: Rotational direction DIRECT (3 or 4)
19 – TT: Offset for radius R-OFFS
20 – TT: Offset for length L-OFFS
21 – TT: Breakage tolerance in length LBREAK
22 – TT: Breakage tolerance in radius RBREAK