HEIDENHAIN iTNC 530 (340 49x-04) Touch Probe Cycles - Manual (Page 91)

HEIDENHAIN iTNC 530 91
3.2 Pr
eset
ting aut
o
matically
DATUM FROM INSIDE OF CORNER
(touch probe cycle 415, DIN/ISO: G415)
Touch probe cycle 415 finds the intersection of two lines and defines
it as the datum. If desired, the TNC can also enter the intersection into
a datum table or preset table.
1 Following the positioning logic (see “Running touch probe cycles”
on page 26), the TNC positions the touch probe at rapid traverse
(value from MP6150 or MP6361) to the first touch point
1 (see
figure at upper right) that you have defined in the cycle. The TNC
offsets the touch probe by the safety clearance in the direction
opposite the respective traverse direction.
2 Then the touch probe moves to the entered measuring height and
probes the first touch point at the probing feed rate (MP6120 or
MP6360). The probing direction is derived from the number by
which you identify the corner.
3 Then the touch probe moves to the next starting position 2 and
probes the second position.
4 The TNC positions the probe to starting point 3 and then to starting
point 4 to probe the third and fourth touch points.
5 Finally the TNC returns the touch probe to the clearance height and
processes the determined datum depending on the cycle
parameters Q303 and Q305 (see “Saving the calculated datum”
on page 69) and saves the coordinates of the determined corner in
the Q parameters listed below
6 If desired, the TNC subsequently measures the datum in the touch
probe axis in a separate probing.
X
Y
1 2
3
4
The TNC always measures the first line in the direction of
the minor axis of the working plane.
Parameter number Meaning
Q151 Actual value of corner in reference axis
Q152 Actual value of corner in minor axis
Before programming, note the following
Before a cycle definition you must have programmed a
tool call to define the touch probe axis.