HEIDENHAIN TNC 410 ISO Programming - Manual (Page 208)

182 8 Programming: Cycles
8
.2 P
o
in
t T
a
b
les
Calling a cycle in connection with point tables
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 G79 PAT:
U U U U To program the cycle call, press the CYCL CALL key.
U U U U Press the CYCL CALL PAT soft key to call a point
table.
U U U 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).
U U U U If required, enter miscellaneous function M, then
confirm with the END key.
The TNC moves the tool back to the clearance height over each
successive starting point (clearance height = the spindle axis
coordinate for cycle call). To use this procedure also for the cycles
number 200 and greater, you must define the 2nd set-up clearance
(Q204) as 0.
If you want to move at reduced feed rate when pre-positioning in the
spindle axis, use the miscellaneous function M103 (see “Feed rate
factor for plunging movements: M103” on page 158).
Effect of the point tables with Cycles G83, G84 and G74 to G78
The TNC interprets the points of the working plane as coordinates of
the hole centers. The coordinate of the spindle axis defines the upper
surface of the workpiece, so the TNC can pre-position automatically
(first in the working plane, then in the spindle axis).
Effect of the point tables with SL Cycles and Cycle G39
The TNC interprets the points as an additional datum shift.
Effect of the point tables with Cycles G200 to G204
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.
With G79 PAT the TNC runs the point table that you last
defined (even if you have defined the point table in a
program that was nested with %).
The TNC uses the coordinate in the spindle axis as the
clearance height for the cycle call.