Adapt Rotary Coordinate System (Cycle 800, Din/Iso: G800); Application - HEIDENHAIN TNC 640 User Manual

12
12.2 ADAPT ROTARY COORDINATE SYSTEM
(Cycle 800, DIN/ISO: G800)

Application

This function must be adapted by your machine
manufacturer.
You need to position the tool appropriately with respect to the
turning spindle, in order to be able to perform a turning operation.
You can use Cycle 800 ADAPT ROTARY COORDINATE SYSTEM for
this.
With turning operations the angle of incidence between the tool
and rotary spindle is important, in order to e.g. machine contours
with back cuts. Cycle 800 provides various possibilities for aligning
the coordinate system for an inclined machining operation:
If you have positioned the tilting axis for inclined machining,
you can use Cycle 800 to orient the coordinate system to the
positions of the tilting axes (Q530=0)
Cycle 800 uses the angle of incidence Q531 to calculate the
required tilting axis angle. Depending on the strategy selected in
parameter INCLINED MACHINING Q530, the TNC positions the
tilting axis with (Q530=1) or without compensating movement
(Q530=2).
Cycle 800 uses the angle of incidence Q531 to calculate the
required tilting axis angle, but does not perform any movements
for positioning the tilting axis (Q530=3). You need to position the
tilting axis to the calculated values Q120 (A axis), Q121 (B axis)
and Q122 (C axis) after the cycle.
If you change the position of a tilting axis, you need to
run Cycle 800 again to align the coordinate system.
If the milling spindle axis and rotary spindle axis are aligned in
parallel, you can define any rotation of the coordinate system
around the spindle axis (Z axis) with the precession angle Q497.
This may be necessary if you have to bring the tool into a specific
position due to space restrictions or if you want to improve your
ability to observe a machining process. If the axes of the rotary
spindle and milling spindle are not aligned in parallel, only two
precession angles for machining are meaningful. The TNC selects
the angle that is closest to the input value Q497
Cycle 800 positions the milling spindle such that the cutting edge is
aligned relative to the turning contour. You can also use the tool in
mirrored state (REVERSE TOOL Q498), whereby the milling spindle
is positioned offset by 180°. In this way you can use tools both
for inside and outside machining. Position the cutting edge at the
center of the turning spindle using a positioning block, such as L Y
+0 R0 FMAX.
366
Cycles: Turning | ADAPT ROTARY COORDINATE SYSTEM
HEIDENHAIN | User's manual for cycle programming | 10/2017
(Cycle 800, DIN/ISO: G800)