HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 53)

Working with fixed cycles 2.1
2
TNC 640 | User's Manual Cycle Programming | 5/2013
53
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 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