HEIDENHAIN TNC 320 User Manual page 376

9
Programming Q parameters
9.12 Preassigned Q parameters
9.12 Preassigned Q parameters
The Q parameters Q100 to Q199 are assigned values by the TNC.
The following types of information are assigned to Q parameters:
Values from the PLC
Tool and spindle data
Data on operating status
Results of measurements from touch probe cycles etc.
The TNC saves the values for the preassigned Q parameters Q108,
Q114 and Q115 to Q117 in the unit of measure used by the active
program.
Preassigned Q parameters (QS parameters) between
Q100 and Q199 (QS100 and QS199) must not be
used in NC programs as calculation parameters.
Otherwise you might receive undesired results.
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.
Active tool radius: Q108
The active value of the tool radius is assigned to Q108. Q108 is
calculated from:
Tool radius R (tool table or TOOL DEF block)
Delta value DR from the tool table
Delta value DR from the TOOL CALL block
The TNC remembers the current tool radius even if
the power is interrupted.
Tool axis: Q109
The value of Q109 depends on the current tool axis:
Tool axis
No tool axis defined
X axis
Y axis
Z axis
U axis
V axis
W axis
376
Parameter value
Q109 = –1
Q109 = 0
Q109 = 1
Q109 = 2
Q109 = 6
Q109 = 7
Q109 = 8
HEIDENHAIN | TNC 320 | Conversational Programming User's Manual | 9/2016