HEIDENHAIN iTNC 530 (340 49x-05) Cycle programming - Manual (Page 229)

HEIDENHAIN iTNC 530 229
9.1 SL Cy
cles with Complex Cont
our F
o
rm
ula
Properties of the subcontours
„ By default, the TNC assumes that the contour is a pocket. Do not
program a radius compensation. In the contour formula you can
convert a pocket to an island by making it negative.
„ The TNC ignores feed rates F and miscellaneous functions M.
„ 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.
„ Although the subprograms can contain coordinates in the spindle
axis, such coordinates are ignored.
„ The working plane is defined in the first coordinate block of the
subprogram. The secondary axes U,V,W are permitted.
Characteristics of the canned cycles
„ The TNC automatically positions the tool to the setup clearance
before a cycle.
„ Each level of infeed depth is milled without interruptions since the
cutter traverses around islands instead of over them.
„ 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).
„ The contour is approached on a tangential arc for side finishing.
„ For floor finishing, the tool again approaches the workpiece on a
tangential arc (for tool axis Z, for example, the arc may be in the Z/X
plane).
„ The contour is machined throughout in either climb or up-cut milling.
The machining data (such as milling depth, finishing allowance and
setup clearance) are entered as CONTOUR DATA in Cycle 20.
Example: Program structure: Calculation of the
subcontours with contour formula
0 BEGIN PGM MODEL MM
1 DECLARE CONTOUR QC1 = “CIRCLE1“
2 DECLARE CONTOUR QC2 = “CIRCLE31XY“
3 DECLARE CONTOUR QC3 = “TRIANGLE“
4 DECLARE CONTOUR QC4 = “SQUARE“
5 QC10 = ( QC1 | QC3 | QC4 ) \ QC2
6 END PGM MODEL MM
0 BEGIN PGM CIRCLE1 MM
1 CC X+75 Y+50
2 LP PR+45 PA+0
3 CP IPA+360 DR+
4 END PGM CIRCLE1 MM
0 BEGIN PGM CIRCLE31XY MM
...
...
With Machine Parameter 7420 you can determine where
the tool is positioned at the end of Cycles 21 to 24.