HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 161)

145 HEIDENHAIN TNC 410, TNC 426, TNC 430
Calling a cycle in connection with point tables
Before programming, note the following:
With G79 PAT the TNC runs the points 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.
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:
ú To program the cycle call, press the CYCL CALL key.
ú Press the CYCL CALL PAT soft key to call a point table.
ú 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).
ú If required, enter miscellaneous function M, then
confirm with the END key.
The TNC moves the tool back to the safe height over each
successive starting point (safe 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 section
”7.4 Miscellaneous Functions for Contouring Behavior”).
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 (see the example in section ”8.3 Drilling
Cycles”).
Effect of the point tables with Cycles G210 to
G215
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 (see the example in section ”8.4 Cycles
for Milling Pockets, Studs and Slots”).
8.2 P
oint T
ables (only in
TNC
41
0)
Kkap8.pm6 29.06.2006, 08:06 145