HEIDENHAIN TNC 620 User Manual page 463

Maintaining the position of the tool tip when
positioning with tilted axes (TCPM): M128 (option 9)
Standard behavior
If the inclination angle of the tool changes this results in an offset
of the tool tip compared to the nominal position. The control does
not compensate this offset. If the operator does not take this
deviation into account in the NC program, offset machining is
executed.
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 in relation to the workpiece remains the
same during the tilting process.
Caution: Danger to the workpiece!
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.
After M128 you can program another feed rate, at which the TNC
will carry out the compensation movements in the linear axes.
If you want to change the position of the tilting axis with the
handwheel during the program run, use M128 along with M118.
Superimposing handwheel positioning is implemented with active
M128, depending on the setting in the 3D-ROT menu of the Manual
operation operating mode, in the active coordinate system or in
the untilted coordinate system.
The functions TCPM or M128 in conjunction with the
dynamic collision monitoring M118 are not available.
Before positioning with M91 or M92 and before a T
BLOCK, RESET M128.
To avoid contour gouging you must use only radius
cutters with M128.
The tool length must refer to the spherical center of
the tool tip.
If M128 is active, the TNC shows the TCPM symbol
in the status display.
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
Miscellaneous functions for rotary axes 12.4
12
463