HEIDENHAIN TNC 620 User Manual page 414

12
Programming: Multiple Axis Machining
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 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 RL/RR/, the TNC will automatically
position the rotary axes for certain machine geometrical
configurations (Peripheral milling, See "Three-dimensional tool
compensation (software option 2)", page 423).
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:
L X+0 Y+38.5 IB-15 RL F125 M128 F1000
TNC 620 | User's Manual
414
HEIDENHAIN Conversational Programming | 3/2014