HEIDENHAIN TNC 320 (34055x-06) Cycle programming - Manual (Page 304)

Touch Probe Cycles: Automatic Datum Setting
15.7 DATUM FROM OUTSIDE OF CIRCLE (Cycle 413, DIN/ISO: G413)
15
304
TNC 320 | User's Manual Cycle Programming | 5/2013
15.7 DATUM FROM OUTSIDE OF CIRCLE
(Cycle 413, DIN/ISO: G413)
Cycle run
Touch Probe Cycle 413 finds the center of a circular stud and
defines it as datum. If desired, the TNC can also enter the
coordinates into a datum table or the preset table.
1 The TNC positions the touch probe at rapid traverse (value from
FMAX column) following the positioning logic (See "Executing
touch probe cycles", page 259) to the starting point
1 . The TNC
calculates the touch points from the data in the cycle and the
safety clearance from the
SET_UP column of the touch probe
table.
2 Then the touch probe moves to the entered measuring height
and runs the first probing process at the probing feed rate
(column
F). The TNC derives the probing direction automatically
from the programmed starting angle.
3 Then the touch probe moves in a circular arc either at measuring
height or at clearance height to the next starting point 2 and
probes the second touch point.
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 "Characteristics common to all
touch probe cycles for datum setting", page 284) and saves the
actual values in the Q parameters listed below.
6 If desired, the TNC subsequently measures the datum in the
touch probe axis in a separate probing.
Parameter number Meaning
Q151 Actual value of center in reference
axis
Q152 Actual value of center in minor axis
Q153 Actual value of diameter
Please note while programming:
Danger of collision!
To prevent a collision between touch probe and
workpiece, enter a
high estimate for the nominal
diameter of the stud.
Before a cycle definition you must have programmed
a tool call to define the touch probe axis.
The smaller the angle increment Q247, the less
accurately the TNC can calculate the datum.
Minimum input value: 5°.
If you set a datum (Q303 = 0) with the touch probe
cycle and also use probe in TS axis (Q381 = 1), then
no coordinate transformation must be active.