Measure Coordinate (Cycle 427, Din/Iso: G427); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Touch Probe Cycles: Automatic Workpiece Inspection | MEASURE COORDINATE (Cycle 427, DIN/ISO: G427)
16.11 MEASURE COORDINATE (Cycle 427,
DIN/ISO: G427)

Cycle run

Touch Probe Cycle 427 finds a coordinate in a selectable axis
and saves the value in a system parameter. If you define the
corresponding tolerance values in the cycle, the TNC makes a
nominal-to-actual value comparison and saves the deviation value in
system parameters.
1 Following the positioning logic, the TNC positions the touch
probe at rapid traverse (value from FMAX column) (See
"Executing touch probe cycles", page 497) to touch point 1.
The TNC offsets the touch probe by the safety clearance in the
direction opposite to the defined traverse direction.
2 Then the TNC positions the touch probe to the entered touch
point 1 in the working plane and measures the actual value in
the selected axis.
3 Finally the TNC returns the touch probe to the clearance
height and saves the measured coordinate in the following Q
parameter.
Parameter number
Q160

Please note while programming:

Before a cycle definition you must have programmed a
tool call to define the touch probe axis.
If an axis of the active working plane is defined as
measuring axis (Q272 = 1 or 2), the TNC compensates
the tool radius. From the defined traversing direction
(Q267) the TNC determines the direction of
compensation.
If the touch probe axis is defined as measuring axis
(Q272 = 3), the TNC compensates the tool length.
If you reference parameter Q330 to a turning tool, the
following applies:
– Parameters Q498 and Q531 have to be described
– The information of the parameters Q498, Q531,
for example from Cycle 800, has to match this
information
– If the TNC compensates the turning tool, the
appropriate values in line DZL and DXL, respectively,
are compensated.
– The TNC monitors the breakage tolerance which is
defined in column LBREAK
If you reference parameter Q330 to a milling tool, the
information of the parameters Q498 and Q531 has no
effect.
HEIDENHAIN | User's manual for cycle programming | 10/2017
Meaning
Measured coordinate
16
617