HEIDENHAIN iTNC 530 (340 49x-01) - Manual (Page 442)

442 8 Programming: Cycles
8.9
Coor
di
na
te
T
ra
n
s
for
m
a
ti
on Cy
cle
s
Procedure for working with Cycle 19 WORKING PLANE
1 Write the program
8 Define the tool (not required if TOOL.T is active), and enter the full
tool length.
8 Call the tool
8 Retract the tool in the tool axis to a position where there is no
danger of collision with the workpiece (clamping devices) during
tilting.
8 If required, position the rotary axis or axes with an L block to the
appropriate angular value(s) (depending on a machine parameter).
8 Activate datum shift if required.
8 Define Cycle 19 WORKING PLANE; enter the angular values for the
tilt axes.
8 Traverse all main axes (X, Y, Z) to activate compensation.
8 Write the program as if the machining process were to be executed
in a non-tilted plane.
8 If required, define Cycle 19 WORKING PLANE with other angular
values to execute machining in a different axis position. In this case,
it is not necessary to reset Cycle 19. You can define the new angular
values directly.
8 Reset Cycle 19 WORKING PLANE; program 0° for all tilt axes.
8 Disable the WORKING PLANE function; redefine Cycle 19 and
answer the dialog question with NO ENT.
8 Reset datum shift if required.
8 Position the rotary axes to the 0° position, if required.
2 Clamp the workpiece
3 Preparations in the operating mode
Positioning with Manual Data Input (MDI)
Pre-position the rotary axis/axes to the corresponding angular value(s)
for setting the datum. The angular value depends on the selected
reference plane on the workpiece.
4 Preparations in the operating mode
Manual Operation
Use the 3D-ROT soft key to set the function TILT WORKING PLANE
to ACTIVE in the Manual Operation mode. Enter the angular values for
the rotary axes into the menu if the axes are not controlled.
If the axes are not controlled, the angular values entered in the menu
must correspond to the actual position(s) of the rotary axis or axes,
respectively. The TNC will otherwise calculate a wrong datum.