Datum, Single Point W/ C Axis G772 - HEIDENHAIN CNC PILOT 640 User Manual

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

Datum, single point w/ C axis G772

Cycle G772 measures with the C 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 element to be probed is
moved toward the touch probe by a rotation of the C axis. When
the workpiece touches the stylus, the measured value is saved and
the workpiece is returned.
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 G152 – activate datum shift and additionally save
in datum table (the datum shift also remains active after the
program run)
2: Activate datum shift with G152 for the further program run
(datum shift no longer active after program run)
C: Incr. meas path w/ Ri. (the algebraic sign determines the
probing direction) – measuring path of the C axis (in degrees)
starting from the current position
AC: Target pos. nominal value – absolute coordinate of touch
point in degrees
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
527