HEIDENHAIN TNC 620 User Manual page 464

12
Multiple axismachining
12.4 Miscellaneous functions for rotary axes
M128 on tilting tables
If you program a tilting table movement while M128 is active, the
TNC rotates the coordinate system accordingly. If, for example,
you rotate the C axis by 90° (through a positioning command or
datum shift) and then program a movement in the X axis, the TNC
executes the movement in the machine axis Y.
The TNC also transforms the set datum, which has been shifted by
the movement of the rotary table.
M128 with 3-D tool compensation
If you carry out a three-dimensional tool compensation with
active M128 and active radius compensation /G41/G42, the TNC
will automatically position the rotary axes for certain machine
geometrical configurations (peripheral milling).
Further Information:
(option 9)", page
Effect
M128 becomes effective at the start of the block, M129 at the end
of the block. M128 is also effective in the manual operating modes
and remains active even after a change of mode. The feed rate for
the compensation movement will be effective until you program a
new feed rate or until you cancel M128 with M129.
Enter M129 to cancel M128. The TNC also cancels M128 if you
select a new program in a program run operating mode.
Example NC blocks
Feed rate of 1000 mm/min for compensation movements:
N50 G01 G41 X+0 Y+38.5 IB-15 F125 M128 F1000*
464
"Three-dimensional tool compensation
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016