HEIDENHAIN TNC 410 ISO Programming - Manual (Page 291)

HEIDENHAIN TNC 410, TNC 426, TNC 430 265
8.7 SL Cy
cles Gr
ou
p II (no
t T
N
C
4
1
0)
8.7 SL Cycles Group II (not TNC 410)
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
n 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.
n
The TNC ignores feed rates F and miscellaneous functions M.
n
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.
n
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.
n
The subprograms must not contain tool axis coordinates.
n The working plane is defined in the first coordinate block of the
subprogram. The secondary axes U,V,W are permitted.
Characteristics of the fixed cycles
n
The TNC automatically positions the tool to set-up clearance before
a cycle.
n
Each level of infeed depth is milled without interruptions since the
cutter traverses around islands instead of over them.
n The radius of “inside corners” can be programmed—the tool keeps
moving to prevent surface blemishes at inside corners (this applies
for the outermost pass in the Rough-out and Side-Finishing cycles).
n The contour is approached in a tangential arc for side finishing.
n For floor finishing, the tool again approaches the workpiece in a
tangential arc (for tool axis Z, for example, the arc may be in the Z/X
plane).
n The contour is machined throughout in either climb or up-cut milling.
The machining data (such as milling depth, finishing allowance and
set-up clearance) are entered as CONTOUR DATA in Cycle G120.
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 *
...
N99999 %SL2 G71 *
The memory capacity for programming an SL cycle (all
contour subprograms) is limited to 48 kilobytes. 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. 256 line blocks.
With MP7420 you can determine where the tool is
positioned at the end of Cycles G121 to G124.