HEIDENHAIN TNC 620 (81760x-02) Cycle programming - Manual (Page 265)

WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) 10.9
10
TNC 620 | User's Manual Cycle Programming | 2/2015
265
Resetting
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 once again and respond to
the dialog question with the
NO ENT key to disable the function.
Positioning the axes of rotation
The machine tool builder determines whether Cycle
19 positions the axes of rotation automatically or
whether they must be positioned manually in the
program. Refer to your machine manual.
Manual positioning of rotary axes
If the rotary axes are not positioned automatically in Cycle 19, you
must position them in a separate L block after the cycle definition.
If you use axis angles, you can define the axis values right in the L
block. If you use spatial angles, then use the Q parameters
Q120
(A-axis value), Q121 (B-axis value) and Q122 (C-axis value), which
are described by Cycle 19.
For manual positioning, always use the rotary axis
positions stored in Q parameters Q120 to Q122.
Avoid using functions, such as M94 (modulo rotary
axes), in order to avoid discrepancies between
the actual and nominal positions of rotary axes in
multiple definitions.
Example NC blocks:
10 L Z+100 R0 FMAX
11 L X+25 Y+10 R0 FMAX
12 CYCL DEF 19.0 WORKING PLANE
Define the spatial angle for calculation of the compensation
13 CYCL DEF 19.1 A+0 B+45 C+0
14 L A+Q120 C+Q122 R0 F1000
Position the rotary axes by using values calculated by Cycle
19
15 L Z+80 R0 FMAX
Activate compensation for the spindle axis
16 L X-8.5 Y-10 R0 FMAX Activate compensation for the working plane