Homing the machine can be carried out by using the G27, G28, or G30 Home Commands.  Homing can also be executed through a Homing Script defined through menu - Setup - Machine Setup - Home.  The Homing Script will execute any valid GCode Blocks when the Home Buttons are pressed.  The Homing Script can perform a Hard Home (to physical Home Switches) or Soft Home (move to position) functions.  Home Switches should be Normally Closed if used.

G27 - Verify Home:

G27 is used to verify table position and perform an Emergency Stop if table position tolerances are beyond specification. G27 will Home to a switch, record the switch location, and calculate the difference from this measured Home Location to the set Home Position.  G27 should only be used after the machine has been Homed using G30.  No Home Offset is performed during the G27 call.  

Syntax of G27 is...
G27 X0.001 Y0.002 Z0.003 F10

Where the axis values define the acceptable tolerance for table position error.  The example above will Home all 3 axes simultaneously to the Home Switches.  G27 is only available when doing a Hard Home to physical switches.  If an axis is not called out in the G27 command, then that axis is ignored during execution.  For example, G27 X0.001 Z0.005 will only home/verify the XZ axes.  The axis value defines the acceptable tolerance.  In the example, the X axis tolerance is set to 0.001.  If the table position is off be more than 0.001 then the G27 command will put the machine in E-Stop.  


G28 - Soft Home:
G28 is used to move to a known location.  The G28 position is set in the Work Coordinate Offset Table under menu Setup - Work Coordinate Offsets.  G28 will simply move to this location.


G30 - Hard Home:
G30 is used to Home to physical Home Switches.  G30 will Home to a switch, set the Home position, and then move to an Offset Location.  If an axis is not called out in the G30 command, then that axis is ignored during execution. For example.
G30 X.5 Z.25 F20
will Home the X and Z axes simultaneously at a feedrate of 20.  The position of the XZ coordinates will be set from values entered in menu Setup - Machine Setup - Axes Setup - Home Position.  The axis values set the Home Offset.  After the machine finds the Home Switches, the XZ axis will move to position 0.5 and 0.25 respectively.

Using the Homing Script:
Any valid GCode Block sequence can be executed when a Home Button is pressed.  The Homing sequence is defined for each axis separately as well as for the 'All' button.  Homing Scripts are defined in menu Setup - Machine Setup - Home.  One example of Homing using the All button follows...
M5                    (Turn Off Spindle)
G92.2 G54        (Zero Work Coordinate Offsets)
G30 X.5 F100  (Home the X Axis at a fast feedrate and offset by 0.5)
G30 X.5 F1      (Re-Home the X Axis at a slower feedrate and offset)
G30 Y.5 F100  (Home the Y Axis at a fast feedrate and offset by 0.5)
G30 Y.5 F1      (Re-Home the Y Axis at a slower feedrate and offset)
G30 Z.5 F100  (Home the Z Axis at a fast feedrate and offset by 0.5)
G30 Z.5 F1      (Re-Home the Z Axis at a slower feedrate and offset)