Search Cycles; Find Hole In C Face G780 - HEIDENHAIN CNC PILOT 640 User Manual

5
5.6

Search cycles

Find hole in C face G780

Cycle G780 probes the workpiece face several times with the Z
axis. Prior to each probing, the touch probe is shifted by a distance
defined in the cycle until a hole is found. Optionally, the cycle
determines the mean value by two probing operations in the hole.
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.
Result #i99
Meaning
< 999997 Result of first measurement
999999 Deviation of probing operations was higher than
programmed in parameter Max. deviation WE
–999999 Hole was not found
Cycle run: From the current position the touch probe moves
along the measuring axis Z 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. Then
the cycle rotates the C axis by the angle defined in the parameter
Search grid Ci RC and probes again with the Z axis. This process
is repeated until a hole is found. In the hole the cycle performs two
probing operations with the C axis, calculates the center of the
hole and places the datum in the C axis.
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(datum shift no longer active after program run)
D: Result:
1: Position—set datum without determining the hole center.
No probing operation in the hole.
2: Object center—before the datum is set, determine hole
center in two probing operations with the C axis.
K: Incr. meas path Z with Ri. (the algebraic sign determines the
probing direction) – maximum measuring path for probing
C: Starting position C – position of the C axis for the first
probing operation
RC: Search grid Ci – stepping angle of the C axis for the
subsequent probing operations
A: Number of points – maximum number of probing operations
548
Touch probe cycles | Search cycles
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017