HEIDENHAIN TNC 620 User Manual page 53

Using Fixed Cycles | Working with fixed cycles
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 for traverse to the start position
programmed in this block.
Using positioning logic the TNC moves 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.
Cycle call with M99/M89
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 run the cycle automatically after every positioning
block, program the first 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 620 | User's manual for cycle programming | 10/2017
2
53