HEIDENHAIN TNC 320 User Manual page 45

Calling a cycle with CYCL CALL POS
The CYCL CALL POS function calls the most recently defined fixed cycle
once. The starting point of the cycle is the position that you defined in
the CYCL CALL POS block.
Using positioning logic the TNC moves to the position defined in the
CYCL CALL POS block.
If the tool's current position in the tool axis is greater than the top
surface of the workpiece (Q203), the TNC moves the tool to the
programmed position first in the machining plane and then in the
tool axis.
If the tool's current position in the tool axis is below the top surface
of the workpiece (Q203), the TNC moves the tool to the
programmed position first in the tool axis to the clearance height and
then in the working plane to the programmed position.
Three coordinate axes must always be programmed in the
CYCL CALL POS block. With the coordinate in the tool axis
you can easily change the starting position. It serves as an
additional datum shift.
The feed rate most recently defined in the CYCL CALL POS
block applies only to traverse to the start position
programmed in this block.
As a rule, the TNC moves without radius compensation
(R0) to the position defined in the CYCL CALL POS block.
If you use CYCL CALL POS to call a cycle in which a start
position is defined (for example Cycle 212), then the
position defined in the cycle serves as an additional shift
of the position defined in the CYCL CALL POS block. You
should therefore always define the start position to be set
in the cycle as 0.
Calling a cycle with M99/89
The M99 function, which is active only in the block in which it is
programmed, calls the last defined fixed cycle once. You can program
M99 at the end of a positioning block. The TNC moves to this position
and then calls the last defined fixed cycle.
If the TNC is to execute the cycle automatically after every positioning
block, program the cycle call with M89.
To cancel the effect of M89, program:
M99 in the positioning block in which you move to the last starting
point, or
Use CYCL DEF to define a new fixed cycle.
HEIDENHAIN TNC 320 45