HEIDENHAIN TNC 640, User Manual, Page: 629 / 948

Multiple-Axis Machining | FUNCTION TCPM (option 9)
13
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
629
Selection of tool reference point and center of rotation
The control provides the following functions for defining the tool
reference point and center of rotation:
REFPNT TIP-TIP
references the (theoretical) tool
tip for positioning. The center of rotation is also
located at the tool tip
REFPNT TIP-CENTER
references the tool tip for
positioning. With a milling cutter, the control
references the theoretical tool tip for positioning,
with a turning tool, it references the virtual tool
tip. The center of rotation is located at the center
of the cutting-edge radius.
REFPNT CENTER-CENTER
references the center
of the cutting-edge radius for positioning. The
center of rotation is also located at the center of
the cutting-edge radius.
The reference point is optional. If you do not enter anything, the
control uses
REFPNT TIP-TIP
.
REFPNT TIP-TIP
The
REFPNT TIP-TIP
variant corresponds to the default behavior
of
FUNCTION TCPM
. You can use all previously allowed cycles and
functions.
REFPNT TIP-CENTER
The
REFPNT TIP-CENTER
variant is mainly intended for the use
with turning tools. In this case the center of rotation and the
positioning point are not coincident. In an NC block, the center of
rotation (center of the cutting-edge radius) is kept in position, but
at the end of the block, the tool tip will no longer be in its initial
position.
The main goal of selecting this reference point is to enable
machining of complex contours in turning mode with active
radius compensation and simultaneously inclined tilting axes
(simultaneous turning).
Further information: "Simultaneous turning", page 705