Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 679)

Skip, Gauge, and Probing Cycles
Chapter 27
27-5
Format for any G37 skip blocks is as follows:
G37 Z__ F__;
Where : Is :
G37 Corresponds to any of the G-codes in the G37 series. Use the one that is
configured to respond to the current skip signal device that is being used.
X, Y, Z The axis on which the offset measurement is to be taken is specified here as
either X, Y, or Z. Only one axis may be specified in a G37 block. The numeric
value following the axis name corresponds to the exact coordinate at which the
skip signal is expected to occur. This value is a signed value (+ or --) and
determines the initial direction of travel. If modifying the tool length offset, then
the tool length axis should be programmed. If modifying the tool diameter, then
any axis that is not a tool length axis may be programmed.
F The tool gauging external skip function feedrate. If no value is entered here, the
external skip function will execute at either the currently active feedrate, or the
feedrate defined for it in AMP (based on whether the AMP parameter Use AMP
Skip Feedrate is set to ”NO”or ”YES”). A value entered here replaces the
currently active feedrate and supersedes the AMP defined feedrate.
The system installer determines (in AMP) a position tolerance for the G37
functions. This tolerance defines a legal range before and after the
coordinate position programmed with the axis word in the G37 block.
If the skip signal is received before the tool enters or after the tool exits the
position tolerance range, a PROBE ERROR will occur. This error appears
on the screen as a warning but does not place the control in E-STOP.
Instead the G37 block is aborted, and program execution proceeds to the
next block. No modification of the tool offset table is performed.
The target offset value for these gauging operations is determined by the
currently active offset number (active D word for tool diameter offset,
active H word for tool length offset). Note that for length offset
measurement, not only must the correct H word be active but the correct
offset must be on (G43, or G44). If the tool diameter offset value is to be
modified, then the following conditions must be true:
a tool diameter offset (D word) must be active though diameter
compensation (G41, G42) does not need to be on.
for most tools to get an accurate measurement for tool diameter, the tool
must be oriented so that the measured diameter is the outside edge of the
tool (not a flute or other geometric feature that would affect the tool
diameter).