Selection Of Tool Reference Point And Center Of Rotation - HEIDENHAIN TNC 620 User Manual

Multiple-axis machining | Compensating the tool angle of inclination with FUNCTION TCPM (option 9)

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: the (theoretical) tool tip is the
reference point for positioning. The center of
rotation is also located at the tool tip
REFPNT TIP-CENTER: the tool tip is the reference
point for positioning. The center of rotation is
located at the center of the cutting-edge radius.
REFPNT CENTER-CENTER: the center of the
cutting-edge radius is the reference point 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). The use of this function only makes sense
for control in turning mode (Option 50). Currently, this software
option is only supported on the TNC 640.
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022
11
473