HEIDENHAIN iTNC 530 (340 49x-03) ISO programming - Manual (Page 263)

HEIDENHAIN iTNC 530 263
7.
4 Miscellaneous F
u
nctions f
o
r Cont
our
ing Beha
vior
Behavior with M120
The TNC checks radius-compensated paths for contour undercuts and
tool path intersections, and calculates the tool path in advance from
the current block. Areas of the contour that might be damaged by the
tool are not machined (dark areas in figure at right). You can also use
M120 to calculate the radius compensation for digitized data or data
created on an external programming system. This means that
deviations from the theoretical tool radius can be compensated.
Use LA (look-ahead) after M120 to define the number of blocks
(maximum: 99) that you want the TNC to calculate in advance. Note
that the larger the number of blocks you choose, the higher the block
processing time will be.
Input
If you enter M120 in a positioning block, the TNC continues the dialog
for this block by asking you the number of blocks LA that are to be
calculated in advance.
Effect
M120 must be located in an NC block that also contains radius
compensation RL or RR. M120 is then effective from this block until
„ radius compensation is canceled, or
„ M120 LA0 is programmed, or
„
M120 is programmed without LA, or
„ another program is called with PGM CALL, or
„ the working plane is tilted with Cycle G80 or the PLANE function.
M120 becomes effective at the start of block.
Limitations
„ After an external or internal stop, you can re-enter the contour with
M120 only with the RESTORE POS. AT N function.
„ If you are using the path functions G25 and G24, the blocks before
and after G25 or G26 must contain only coordinates of the working
plane.
„
Before using the functions listed below, you have to cancel M120
and the radius compensation:
„
Cycle G60 Tolerance
„ Cycle G80 Working Plane
„ M114
„ M128
„ M138
„
M144
„ PLANE function
„ TCPM FUNCTION (only conversational)
„ WRITE TO KINEMATIC (only conversational format)