HEIDENHAIN TNC 620 (340 56x-02) ISO programming - Manual (Page 310)

310 Programming: Multiple Axis Machining
1
1
.4 Miscellaneous F
unctions f
or Rotary Ax
es
Behavior with M128 (TCPM: Tool Center Point Management)
If the position of a controlled tilted axis changes in the program, the
position of the tool tip to the workpiece remains the same.
After M128 you can program another feed rate, at which the TNC will
carry out the compensation movements in the linear axes. If you do
not enter a feed rate, the TNC uses the maximum feed rate.
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 .
The machine geometry must be specified by the machine
tool builder in the description of kinematics.
X
Z
B
Z
X
For tilted axes with Hirth coupling: Do not change the
position of the tilted axis until after retracting the tool.
Otherwise you might damage the contour when
disengaging from the coupling.
Before positioning with M91 or M92 and before a T block,
reset M128.
To avoid contour gouging you must use only spherical
cutters with M128.
The tool length must refer to the spherical center of the
tool tip.
If M128 is active, the TNC shows the symbolTCPM in the
status display.