HEIDENHAIN TNC 640, User Manual, Page: 705 / 948

Turning | Turning program functions (option 50)
16
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
705
15 L X+165 Y+0 R0 FMAX
Pre-positioning the tool
16 L Z+2 R0 FMAX
Tool at starting position
...
Machining with inclined axis
M128
Alternately, you can use the
M128
function The effect is the same,
but the following limitation applies here: if you activate inclined
machining with M128 then tool-tip radius compensation without
a cycle, i.e. in traversing blocks with
RL
/
RR
, is not possible. If you
activate inclined machining via
M144
or
FUNCTION TCPM
with
REFPNT TIP-CENTER
then this limitation does not apply.
FUNCTION TCPM with REFPNT TIP-CENTER
Use
FUNCTION TCPM
with the selection
REFPNT TIP-CENTER
to
activate the virtual tool tip. If you activate inclined machining via
FUNCTION TCPM
with
REFPNT TIP-CENTER
then tool-tip radius
compensation without a cycle, i.e. in traversing blocks with
RL
/
RR
,
is possible.
Inclined turning is also possible in the
Manual operation
operating
mode if you activate
FUNCTION TCPM
with the selection
REFPNT
TIP-CENTER
in, for example, the
Positioning w/ Manual Data Input
operating mode.
Simultaneous turning
You can combine the turning operation with function
M128
or
FUNCTION TCPM
and
REFPNT TIP-CENTER
. This enables you to
manufacture contours in one cut, for which you have to change the
inclination angle (simultaneous machining).
The simultaneous turning contour is a turning contour for which a
rotary axis whose inclination does not violate the contour can be
programmed on polar circles
CP
and linear blocks
L
. Collisions with
lateral cutting edges or holders are not prevented. This makes it
possible to finish contours with one tool in a continuous movement
although different parts of the contour are only accessible with
different tool inclinations.
In the NC program you define how the rotary axis has to be
inclined to reach the different contour parts without collisions.
Use the cutter radius oversize
DRS
to leave an equidistant oversize
on the contour.
Use
FUNCTION TCPM
and
REFPNT TIP-CENTER
to measure the
theoretical tool tip of the turning tools being used for this.