HEIDENHAIN TNC 320 (340 55x-04) Cycle programming - Manual (Page 264)

264 Cycles: Coordinate Transformations
1
1
.9 W
O
RKING PLANE (Cy
c
le 1
9
, DIN/ISO: G80, Sof
tw
a
re
Option 1)
Procedure for working with Cycle 19 WORKING
PLANE
1 Write the program
U Define the tool (not required if TOOL.T is active), and enter the full
tool length.
U Call the tool
U Retract the tool in the tool axis to a position where there is no
danger of collision with the workpiece (clamping devices) during
tilting.
U If required, position the rotary axis or axes with an L block to the
appropriate angular value(s) (depending on a machine parameter).
U Activate datum shift if required.
U Define Cycle 19 WORKING PLANE; enter the angular values for the
tilt axes.
U Traverse all principal axes (X, Y, Z) to activate compensation.
U Write the program as if the machining process were to be executed
in a non-tilted plane.
U 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.
U Reset Cycle 19 WORKING PLANE; program 0° for all rotary axes.
U Disable the WORKING PLANE function; redefine Cycle 19 and
answer the dialog question with NO ENT.
U Reset datum shift if required.
U Position the rotary axes to the 0° position, if required.
2 Clamp the workpiece
3 Datum setting
„ Manually by touch-off
„ Controlled with a HEIDENHAIN 3-D touch probe (see the Touch
Probe Cycles User's Manual, chapter 2).
„ Automatically with a HEIDENHAIN 3-D touch probe (see the Touch
Probe Cycles User's Manual, chapter 3).
4 Start the part program in the operating mode Program Run, Full
Sequence
5 Manual Operation mode
Use the 3-D ROT soft key to set the TILT WORKING PLANE function
to INACTIVE. Enter an angular value of 0° for each rotary axis in the
menu.