HEIDENHAIN TNC 310 (286 140) - Manual (Page 188)

10 Programming: Q Parameters 176
1
0.9 Pr
eassigned Q P
ar
a
met
ers
10.9 Preassigned Q Parameters
The Q parameters Q100 to Q122 are assigned values by the TNC.
These values include:
■ Values from the PLC
■ Tool and spindle data
■ Data on operating status, etc.
Values from the PLC: Q100 to Q107
The TNC uses the parameters Q100 to Q107 to transfer values from
the PLC to an NC program.
Tool radius: Q108
The current value of the tool radius is assigned to Q108.
Tool axis: Q109
The value of Q109 depends on the current tool axis:
Tool axis Parameter value
No tool axis defined Q109 = –1
Z axis Q109 = 2
Y axis Q109 = 1
X axis Q109 = 0
Spindle status: Q110
The value of Q110 depends on which M function was last
programmed for the spindle:
M function Parameter value
No spindle status defined Q110 = –1
M03: Spindle ON, clockwise Q110 = 0
M04: Spindle ON, counterclockwise Q110 = 1
M05 after M03 Q110 = 2
M05 after M04 Q110 = 3
Coolant on/off: Q111
M function Parameter value
M08: Coolant ON Q111 = 1
M09: Coolant OFF Q111 = 0
Overlap factor: Q112
The overlap factor for pocket milling (MP7430) is assigned to Q112.