HEIDENHAIN ITNC 530 - CYCLE PROGRAMMING User Manual page 361

Please note while programming:
Danger of collision!
To prevent a collision between the touch probe and the
workpiece, enter a low estimate for the nominal diameter
of the pocket (or hole).
If the dimensions of the pocket and the safety clearance
do not permit pre-positioning in the proximity of the touch
points, the TNC always starts probing from the center of
the pocket. In this case the touch probe does not return to
the clearance height between the four measuring points.
The smaller the angle increment Q247, the less accurately
the TNC can calculate the datum. Minimum input value: 5°
Before a cycle definition you must have programmed a
tool call to define the touch probe axis.
Cycle parameters
U Center in 1st axis Q321 (absolute): Center of the
pocket in the reference axis of the working plane.
Input range -99999.9999 to 99999.9999
U Center in 2nd axis Q322 (absolute): Center of the
pocket in the minor axis of the working plane. If you
program Q322 = 0, the TNC aligns the hole center to
the positive Y axis. If you program Q322 not equal to
0, then the TNC aligns the hole center to the nominal
position. Input range -99999.9999 to 99999.9999
U Nominal diameter Q262: Approximate diameter of the
circular pocket (or hole). Enter a value that is more
likely to be too small than too large. Input range 0 to
99999.9999
U Starting angle Q325 (absolute): Angle between the
reference axis of the working plane and the first touch
point. Input range -360.0000 to 360.0000
U Stepping angle Q247 (incremental): Angle between
two measuring points. The algebraic sign of the
stepping angle determines the direction of rotation
(negative = clockwise) in which the touch probe
moves to the next measuring point. If you wish to
probe a circular arc instead of a complete circle, then
program the stepping angle to be less than 90°. Input
range -120.0000 to 120.0000
HEIDENHAIN iTNC 530 361