HEIDENHAIN TNC 640 User Manual page 655

Turning | Turning program functions (option 50)
M144
Inclining a swivel axis creates an offset from tool to tool. The
function M144 considers the position of the inclined axes and
compensates this offset. In addition the function M144 aligns the
Z direction of the workpiece coordinate system to the direction of
the centerline of the workpiece. If an inclined axis is a tilting table,
meaning that the workpiece itself is inclined, the control performs
traverse movements in the rotated workpiece coordinate system. If
the inclined axis is a swivel head (meaning that the tool is inclined),
the workpiece coordinate system is not rotated.
After inclining the swivel axis you may have to again pre-position
the tool in the Y coordinate and orient the position of the tool tip
with Cycle 800.
...
N10 M144*
N20 G00 A-25 G40*
N30 800 ADJUST XZ SYSTEM
Q497=+90 ;PRECESSION ANGLE
Q498=+0 ;REVERSE TOOL
Q530=+2 ;INCLINED MACHINING
Q531=-25 ;ANGLE OF INCIDENCE
Q532=750 ;FEED RATE
Q533=+1 ;PREFERRED DIRECTION
Q535=3 ;ECCENTRIC TURNING
Q536=0 ;ECCENTRIC W/O STOP
N40 G00 X+165 Y+0 G40*
N50 G00 Z+2 G40*
...
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 G41/G42, is not possible. If you
activate inclined machining via M144 then this limitation does not
apply.
HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017
Activate inclined machining
Position swivel axis
Workpiece coordinate system and align tool
Pre-positioning the tool
Tool at starting position
Machining with inclined axis
16
655