Calling A Cycle In Connection With Point Tables - HEIDENHAIN ITNC 530 - CYCLE PROGRAMMING User Manual

Calling a cycle in connection with point tables

With CYCL CALL PAT the TNC runs the point table that you
last defined (even if you defined the point table in a
program that was nested with CALL PGM).
If you want the TNC to call the last defined fixed cycle at the points
defined in a point table, then program the cycle call with CYCLE CALL
PAT:
U To program the cycle call, press the CYCL CALL key
U Press the CYCL CALL PAT soft key to call a point table
U Enter the feed rate at which the TNC is to move from
point to point (if you make no entry the TNC will move
at the last programmed feed rate; FMAX not valid)
U If required, enter a miscellaneous function M, then
confirm with the END key
The TNC retracts the tool to the safety clearance between the starting
points. Depending on which is greater, the TNC uses either the spindle
axis coordinate from the cycle call or the value from cycle parameter
Q204 as the safety clearance.
If you want to move at reduced feed rate when pre-positioning in the
spindle axis, use the miscellaneous function M103.
Effect of the point tables with SL cycles and Cycle 12
The TNC interprets the points as an additional datum shift.
Effect of the point tables with Cycles 200 to 208 and 262 to 267
The TNC interprets the points of the working plane as coordinates of
the hole centers. If you want to use the coordinate defined in the point
table for the spindle axis as the starting point coordinate, you must
define the workpiece surface coordinate (Q203) as 0.
Effect of the point tables with Cycles 210 to 215
The TNC interprets the points as an additional datum shift. If you want
to use the points defined in the point table as starting-point
coordinates, you must define the starting points and the workpiece
surface coordinate (Q203) in the respective milling cycle as 0.
Effect of the point tables with Cycles 251 to 254
The TNC interprets the points of the working plane as coordinates of
the cycle starting point. If you want to use the coordinate defined in
the point table for the spindle axis as the starting point coordinate, you
must define the workpiece surface coordinate (Q203) as 0.
HEIDENHAIN iTNC 530 69