Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 694)

Skip, Gauge, and Probing Cycles
Chapter 27
27-20
The control will perform its normal axis deceleration as it approaches the
final depth. When the final depth is reached the axis stops and the part
program continues on from that point. Since the actual location of the
endpoint of the move is not known until the probe is depressed, the control
must re-setup any part program blocks that it previously read into block
look ahead. If you program an adaptive depth probe distance (with the
integrand word) that is very close to the AMPed probe trigger tolerance,
axis speed as the control searches for a probe input may be reduced to
allow enough time for the axis to decelerate once the probe has fired. For
example if .2 inches of deflection is the probe trigger tolerance and you
program an integrand of .21 inches, the control may need to limit the
feedrate since only .01 inches are available for deceleration of the axis
once the probe has fired.
You must program the G26 block in G01 mode. Programming G26 in
other cutting modes (such as G00, G02, or G03) will generate an error.
The G26 command is not modal and must be programmed in all blocks
that use the adaptive depth feature. Using the G61 (inposition mode)
during G26 blocks means that the G26 block will wait for the depth probe
to reach the AMP’ed inposition.
Example 27.1
Adaptive Depth Drilling 7.5 mm Into Part Surface
Spindle
Motor
Adaptive Depth Probe
Drilling Surface
Z Axis
Z
20
15
10
5
0
Hole Depth K
Point Past hole bottom (Z)
G90G01F100;
G26 Z1 K7.5;