HEIDENHAIN TNC 640, User Manual, Page: 467 / 948

Programming Q Parameters | Preassigned Q parameters
10
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
467
10.12 Preassigned Q parameters
The Q parameters Q100 to Q199 are assigned values by the
control. The following types of information are assigned to the Q
parameters:
Values from the PLC
Tool and spindle data
Data on operating status
Results of measurements from touch probe cycles etc.
The control saves the preassigned Q parameters Q108, Q114 and
Q115 - Q117 in the unit of measure used by the active program.
NOTICE
Danger of collision!
Q parameters are used in the HEIDENHAIN cycles, in machine
tool builder cycles, and in supplier functions. You can also
program Q parameters within the NC program. If, when using Q
parameters, the recommended Q parameter ranges are not used
exclusively, then this can lead to overlapping (reciprocal effects)
and thus cause undesired behavior. Danger of collision during
machining!
Only use Q parameter ranges recommended by
HEIDENHAIN.
Comply with the documentation from HEIDENHAIN, the
machine tool builder, and suppliers.
Check the machining sequence using a graphic simulation
You must not use preassigned Q parameters (QS
parameters) between
Q100
and
Q199
(
QS100
and
QS199
) as calculation parameters in the NC programs.
Values from the PLC: Q100 to Q107
The control assigns values from the PLC to parameters Q100 to
Q107 in 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 control remembers the current tool radius even if
the power is interrupted.