HEIDENHAIN iTNC 530 (340 49x-01) ISO programming - Manual (Page 404)

404 8 Programming: Cycles
8.9
Coor
di
na
te
T
ra
n
s
for
m
a
ti
on Cy
cle
s
If you set the function TILTING program run to ACTIVE in the Manual
Operation mode (see “Tilting the Working Plane (Software Option 1)”
on page 70), the angular value entered in this menu is overwritten by
Cycle G80 WORKING PLANE.
8 Tilt axis and tilt angle?: Enter the axes of rotation
together with the associated tilt angles. The rotary
axes A, B and C are programmed using soft keys.
If the TNC automatically positions the rotary axes, you can enter the
following parameters:
8 Feed rate ? F=: Traverse speed of the rotary axis
during automatic positioning.
8 Set-up clearance? (incremental value): The TNC
positions the tilting head so that the position that
results from the extension of the tool by the set-up
clearance does not change relative to the workpiece.
Cancellation
To cancel the tilt angle, redefine the WORKING PLANE cycle and enter
an angular value of 0° for all axes of rotation. You must then program
the WORKING PLANE cycle again, without defining an axis, to disable
the function.
Position the axis of rotation
If the axes are positioned automatically in Cycle G80:
„ The TNC can position only controlled axes.
„ In order for the tilted axes to be positioned, you must enter a feed
rate and a set-up clearance in addition to the tilting angles, during
cycle definition.
„ You can use only preset tools (with the full tool length defined in the
G99
block or in the tool table).
„ The position of the tool tip as referenced to the workpiece surface
remains nearly unchanged after tilting.
„ The TNC tilts the working plane at the last programmed feed rate.
The maximum feed rate that can be reached depends on the
complexity of the swivel head or tilting table.
If the axes are not positioned automatically in Cycle G80, position them
before defining the cycle, for example with a G01 block.
The machine tool builder determines whether Cycle G80
positions the axes of rotation automatically or whether
they must be pre-positioned in the program. Refer to your
machine manual.