Single-Point Measurmnt., Datum G771 - HEIDENHAIN CNC PILOT 640 User Manual

Touch probe cycles | Touch probe cycles for single-point measurement

Single-point measurmnt., datum G771

Cycle G771 measures with the programmed measuring axis in the
specified direction. If the tolerance value defined in the cycle is
exceeded, the cycle saves the measured deviation as datum shift.
The result of the measurement is saved additionally in the variable
#i99.
Further information: "Touch probe cycles for automatic mode",
Page 521
Cycle run: From the current position the touch probe moves along
the defined measuring axis toward the measuring point. When the
stylus touches the workpiece, the measured value is saved and the
touch probe is positioned back to the starting point.
The control outputs an error message if the touch probe does
not reach any touch point within the defined measuring path.
If a Max. deviation WE was programmed, the measuring point
is approached twice and the mean value is saved as result. If
the difference of the measurements is greater than the Max.
deviation WE, the program run is interrupted and an error message
is displayed.
Parameters:
R: Type of datum shift
1: Table and G59 – activate datum shift and additionally save
in datum table (the datum shift also remains active after the
program run)
2: Activate datum shift with G59 for the further program run
(zdatum shift no longer active after program run)
D: Measuring axis – axis in which the measurement is to be
made
K: Incr. meas path w/ Ri. (the algebraic sign determines the
probing direction) – maximum measuring path for probing
AC: Target pos. nominal value – touch point coordinate
BD: Tolerance position +/ – measurement result range in which
no compensation is applied
WE: Max. deviation – probe twice and monitor the dispersion
of the measured values
F: Measuring feed – feed rate for probing (if nothing is entered,
the measuring feed rate from the touch probe table is used)
If the entered measuring feed rate F is higher than the one in
the touch probe table, the feed rate is reduced to the value from
the touch probe table.
Q: Tool orientation (machine-dependent)
Orient the touch probe in the programmed probing direction
before each probing operation.
P: PRINT outputs
0: OFF – do not display measuring results
1: ON – display measuring results on the screen
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
5
525