HEIDENHAIN TNC 640, User Manual, Page: 625 / 948

Multiple-Axis Machining | FUNCTION TCPM (option 9)
13
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
625
13.5 FUNCTION TCPM (option 9)
Function
Refer to your machine manual.
The machine geometry must be specified by the
machine tool builder in the description of kinematics.
FUNCTION TCPM
is an improvement on the
M128
function, with
which you can define the behavior of the control when positioning
the rotary axes. In contrast to
M128
, with the
FUNCTION TCPM
you
can define the effect of various functions yourself:
Effect of the programmed feed rate:
F TCP
/
F CONT
Interpretation of the rotary axis coordinates programmed in the
NC program:
AXIS POS
/
AXIS SPAT
Type of interpolation between start and target position:
PATHCTRL AXIS
/
PATHCTRL VECTOR
Optional selection of a tool reference point and a center of
rotation:
REFPNT TIP-TIP
/
REFPNT TIP-CENTER
/
REFPNT
CENTER-CENTER
If
FUNCTION TCPM
is active, the control shows the
TCPM
symbol
in the position display.
NOTICE
Danger of collision!
Rotary axes with Hirth coupling must move out of the coupling
to enable tilting. There is a danger of collision while the axis
moves out of the coupling and during the tilting operation.
Tool retracted before the position of the tilting axis is changed
Programming notes:
Before positioning axes with
M91
or
M92
and before
a
TOOL CALL
block, cancel the
FUNCTION TCPM
function.
Only use spherical cutters for face milling operations
in order to avoid contour damage. In combination
with other tool shapes, you should use graphic
simulation to test the NC program for possible
contour damages.
Defining FUNCTION TCPM
Select the special functions
Select the programming aids
Select
FUNCTION TCPM