Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 406)

Axis Motion
Chapter 14
14-30
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”.
When a G28 is executed in a part program (or through MDI) after the axes
have already been homed, it causes a return to machine home. In this case,
the axes specified in the G28 block simply go to their respective home
position in the machine coordinate system,after moving to a programmed
intermediate point. They do not repeat the homing routine of moving to
the limit switches and searching for the encoder marker. For example,
executing the block:
G28 X__ Y__ Z__ ;
In either absolute or incremental mode would return the axes automatically
to the machine home via an intermediate point. The control stores the
intermediate point specified by the axis words (X, Y, Z) in memory to be
used as the point of return for the automatic return from machine home
operation called out by G29.
The return operation generates two axis moves both executed at the rapid
feedrate. The first move travels to the intermediate point and the second
travels to the axis home position.
14.3.2
Automatic Return to
Machine Home (G28)