HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 468)

468 8 Programming: Cycles
8.9 Coor
dinat
e
T
ransf
or
mation Cy
cles
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 performs the tilt 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.
Example NC blocks:
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.
N50 G00 G40 Z+100 *
N60 X+25 Y+10 *
N70 G01 A+15 F1000 * Position the axis of rotation
N80 G80 A+15 * Define the angle for calculation of the compensation
N90 G00 GG40 Z+80 * Activate compensation for the tool axis
N100 X-7.5 Y-10 * Activate compensation for the working plane