HEIDENHAIN iTNC 530 (340 49x-03) ISO programming - Manual (Page 383)

HEIDENHAIN iTNC 530 383
8.6 SL Cy
cles
8.6 SL Cycles
Fundamentals
SL cycles enable you to form complex contours by combining up to 12
subcontours (pockets or islands). You define the individual
subcontours in subprograms. The TNC calculates the total contour
from the subcontours (subprogram numbers) that you enter in Cycle
G37
CONTOUR GEOMETRY.
Characteristics of the subprograms
„ Coordinate transformations are allowed. If they are programmed
within the subcontour they are also effective in the following
subprograms, but they need not be reset after the cycle call.
„ The TNC ignores feed rates F and miscellaneous functions M.
„ The TNC recognizes a pocket if the tool path lies inside the contour,
for example if you machine the contour clockwise with radius
compensation G42.
„
The TNC recognizes an island if the tool path lies outside the
contour, for example if you machine the contour clockwise with
radius compensation G41.
„
The subprograms must not contain tool axis coordinates.
„ The working plane is defined in the first coordinate block of the
subprogram. The secondary axes U,V,W are permitted in useful
combinations. Always define both axes of the machining plane in
the first block.
„ If you use Q parameters, then only perform the calculations and
assignments within the affected contour subprograms.
Example: Program structure: Machining with SL
cycles
%SL2 G71 *
...
N120 G37 ... *
N130 G120 ... *
...
N160 G121 ... *
N170 G79 *
...
N180 G122 ... *
N190 G79 *
...
N220 G123 ... *
N230 G79 *
...
N260 G124 ... *
N270 G79 *
...
N500 G00 G40 Z+250 M2 *
N510 G98 L1 *
...
N550 G98 L0 *
N560 G98 L2 *
...
N600 G98 L0 *
...
N99999999 %SL2 G71 *
The memory capacity for programming an SL cycle (all
contour subprograms) is limited. The number of possible
contour elements depends on the type of contour (inside or
outside contour) and the number of subcontours. For
example, you can program up to approx. 8192 line blocks.
SL cycles conduct comprehensive and complex internal
calculations as well as the resulting machining operations.
For safety reasons, always run a graphical program test
before machining! This is a simple way of finding out
whether the TNC-calculated program will provide the
desired results.