Calling A Cycle In Connection With Point Tables - HEIDENHAIN TNC 620 User Manual

Using Fixed Cycles | Point tables

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:
To program the cycle call, press the CYCL CALL
key
Press the CYCL CALL PAT soft key to call a point
table
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 is not valid)
If required, enter a miscellaneous function M,
then confirm with the END key
The TNC retracts the tool to the clearance height 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 clearance height.
Before CYCL CALL PAT you can use the function GLOBAL DEF 125
(located in SPEC FCT/program defaults) with Q352=1. Then the
TNC always retracts the tool between the holes to the 2nd set-up
clearance that was defined in the cycle.
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 table with SL cycles and Cycle 12
The TNC interprets the points as an additional datum shift.
Effect of the point table 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 table 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 | TNC 620 | User's manual for cycle programming | 10/2017
2
67