HEIDENHAIN TNC 640 (34059x-05) ISO programming - Manual (Page 440)

Programming: Multiple Axis Machining
12.4 Miscellaneous functions for rotary axes
12
440
TNC 640 | User's ManualDIN/ISO Programming | 1/2015
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 defined datum, which has been
shifted by the movement of the rotary table.
M128 with 3-D tool compensation
If you carry out a 3-D 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 millingsee "Three-dimensional tool
compensation (Option #9)").
Effect
M128 becomes effective at the start of block, M129 at the end of
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 *