Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 682)

Skip, Gauge, and Probing Cycles
Chapter 27
27-8
The purpose of this cycle is to provide a means to measure the actual
radius and/or locate the center of a hole in a part or gauge using a touch
probe.
To use the G38 cycle, the currently active plane when the G38 is
programmed must be the same plane that the hole to be measured is in (see
chapter 13 for information on plane selection). For example, to measure a
hole that is cut in the XY plane, the G38 code must be programmed with
the XY plane active.
Format for the G38 code is as follows:
G38 H__ R__ D__ E__ F__;
Where : Is :
H The estimated or expected diameter of the hole. This parameter is optional. If H is
not programmed, the control will generate an H value that is equal to 2(R+D),
where R is the approach distance and D is the tolerance band. Note that if R+D
is greater than one half H, the control will ignore the programmed H value and use
2(R+D) as the new expected diameter.
R The incremental unsigned approach distance. Enter the distance from the
start--point of the probing cycle to a point that it is desirable for the feedrate to be
slowed. At this point, the feedrate will slow from the approach feedrate (E) to the
probing feedrate (F). This parameter is optional. If not entered, the control will
default to the value entered in the probing cycle parameter table discussed in
section 27.5.
D The tolerance band distance. The value entered for D defines a band on each side
of the expected diameter entered with the H parameter. Enter a value defining a
tolerance distance on either side of the expected probe triggering point. This
parameter is optional. If not entered, the control will default to the value entered in
the probing cycle parameter table discussed in section 27.5.
E The approach feedrate. Enter a value for this parameter that defines the feedrate
at which the probe is to approach the position specified by the R parameter. This
parameter is optional. If not entered, the control will default to the value entered in
the probing cycle parameter table discussed in section 27.5.
F The probe feedrate. Enter a value for this parameter that defines the feedrate at
which the probe is to move after passing the point defined by the R parameter.
The probe continues on at this feedrate until contact has been made with the
diameter of the hole or until the tolerance band is exceeded. This parameter is
optional. If not entered, the control will default to the value entered in the probing
cycle parameter table discussed in section 27.5.
Parameters R, D, E, and F can be entered in three ways:
The system installer may have entered them in AMP, in which case they
will always be available and need not be programmed in the G38 block.
Refer to the documentation provided by your system installer.
They may be entered or changed through the probing parameters table
described in section 27.5. If entered in the table, they need not be
programmed in the G38 block. The table value will supersede any
values entered in AMP.
27.4
Hole Probing (G38)