Datum In One Axis (Cycle 419, Din/Iso: G419, Software Option 17); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 620 User Manual

14
Touch Probe Cycles: Automatic Datum Setting
14.13 DATUM IN ONE AXIS (Cycle 419, DIN/ISO: G419)
14.13 DATUM IN ONE AXIS (Cycle 419,
DIN/ISO: G419, software option 17)

Cycle run

Touch Probe Cycle 419 measures any coordinate in any axis
and defines it as datum. If desired, the TNC can also enter the
measured coordinate in a datum table or preset table.
1 Following the positioning logic, the TNC positions the touch
probe at rapid traverse (value from FMAX column) (see
"Executing touch probe cycles", page 304) to the programmed
touch point 1. The TNC offsets the touch probe by the safety
clearance in the direction opposite the programmed probing
direction.
2 Then the touch probe moves to the programmed measuring
height and measures the actual position with a simple probing
movement.
3 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 332).

Please note while programming:

Before a cycle definition you must have programmed
a tool call to define the touch probe axis.
If you want to save the datum of several axes in the
preset table, you can use Cycle 419 several times
in a row. However, you also have to reactivate the
preset number after every run of Cycle 419. If you
work with preset 0 as active preset, this process is
not required.
376
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 9/2015