HEIDENHAIN iTNC 530 (340 422) ISO programming - Manual (Page 228)

228 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 a 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 for cycles above Cycle
199, you must define the 2nd set-up clearance (Q204) to equal 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 202).
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.
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, where the tool is located during cycle
call. A clearance height or 2nd set-up clearance that is
defined separately in a cycle must not be greater than the
clearance height defined in the global pattern.