Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 400)

Axis Motion
Chapter 12
12-28
Automatic homing is accomplished through the use of a G28 code. When
programmed as the first motion block in a part program, (or through MDI)
a G28 automatically homes any axes programmed in the G28 block that
have not yet been homed. Only axes that have their axis words
programmed in the G28 block are homed.
Homing follows the sequence of homing events described in chapter 3.
The coordinate values which are programmed with the axis words in a G28
block are stored by the control as intermediate point values (described in
the next section).
If all the axes programmed in the G28 block have already been homed
when the G28 code is executed, then the control considers it an “Automatic
Return to Machine Home” as described in the next section.
Important: When a homing request is made the feedback device for the
axis (typically an encoder) must encounter at least one marker before
tripping the homing limit switch. If the axis is close to the home limit
switch you should jog the axis away from this switch before attempting a
homing operation.
Automatic Machine Homing (G28) with Distance Coded Markers
The following outlines automatic machine homing (G28) for an axis with
DCM feedback if the axis has not already been homed:
1. The axis moves at a speed and direction defined in AMP by G28
Home Speed and G28 Direction to Home, respectively.
The axis will come to a stop once the axis crosses three consecutive
markers on the DCM scale.
Important: To determine an absolute position using DCMs, you must
encounter at least three consecutive markers. Thus, if the axis position will
not accommodate this assumption, the axis must be moved to another
position before attempting a homing operation.
2. When the output command equals 0 (i.e., the axis stops), the control
will determine the absolute position. Refer to your AMP manual for
more information about DCM Homing for Absolute Position.
If your axis is already homed, refer to the Automatic Return to
Home (G28) section later in this chapter.
Important: DCM axis homing must be performed manually or by
programming a G28. Attempting to program any motion command other
than a G28 will result in the decode error “MUST HOME AXIS”.
12.4.1
Automatic Machine Homing
(G28)