Table of Contents
Advertisement
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 o the position defined in the
CYCL CALL POS block.
If the 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 current tool 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.
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 cycles serves as an additional shift
on 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 first cycle call with M89 (depending on MP 7440).
To cancel the effect of M89, program:
M99 in the positioning block in which you move to the last starting
point, or
A CYCL CALL POS block or
A new fixed cycle with CYCL DEF
HEIDENHAIN iTNC 530
51
Hide quick links:
Advertisement
Table of Contents
Need help?
Do you have a question about the ITNC 530 - CYCLE PROGRAMMING and is the answer not in the manual?
Questions and answers
Can I change the approach direction when cycle def a stud to avoid obstruction to the right
The provided context does not explicitly mention changing the approach direction to avoid obstruction. However, it describes selecting different axis configurations using the MOD function in the Programming and Editing mode. If modifying the axis configuration allows for adjusting the approach direction, it may be possible. Otherwise, specific cycle parameters should be checked in the programming manual.
This answer is automatically generated