8 Basic CNC Programming
8.4 NC Codes
105
8.4.6.6.1.
G28 and G29: Homing Commands
The Homing feature in the control software sends the machine to the predefined Home position (0,0,0).
This is used as a reference for other motion.
The homing commands (G28, G29) allow you to return to and check this established position. The milling
center uses this point as a reference for all machine coordinate movements. This allows you to use the
Soft Limits and Coordinate Systems commands (under the Setup Menu) to move the milling center
consistently to the same location.
Before you can use any homing commands, or the Soft Limits and Coordinate Systems commands, you
must use the Set/Check Home command to establish an initial reference point. See
for information on using the Set/Check Home command.
Using G28 Code
G28 homes the machine, zeroing the machine coordinates. Optionally, the machine can be instructed to
pass through specified coordinates on its way to the home position. For example, G28 X1 Y1 Z2
commands the machine to pass through X1 Y1 Z2 and then move to home position.
Using G29 Code
The G29 code moves the tool at a rapid traverse rate to a coordinate specified by XYZ. If you have set an
intermediate point on one or more axes, the machine first rapids from the current position to the
intermediate point then continues to the specified destination. If you command a G29 code in
incremental mode, your specified XYZ point is relative to the intermediate point. If you have not
specified an intermediate point, your specified XYZ point is relative to the current position. Use the G29
code after a G28 code to return the tool to a position closer to the part. The example below shows the
use of a G28 code and a G29 code.
N1G28X2Z-1; INTERMEDIATE POINT THEN HOME N2G29X4Z1; GO TO G29 POINT
8.4.6.6.2.
G92: Preset Position
The G92 code is used to initialize the current tool position. In other words, the G92 code can be used to
redefine the X, Y and Z values of the tool’s current position. The X, Y, and Z coordinates following a G92
code define the new current position of the tool.
The tool position can also be redefined through the control software, by clicking Setup | Set Position in
the Main Menu.
8.4.6.7.
The Coordinate System Group
Use the Coordinate System codes to establish multiple coordinate systems on one or more workpieces
to create multiple parts.
For instance, you can run a part program using a typical coordinate system (with the point of origin on
the left side of the workpiece next to the chuck, along the centerline of the workpiece), and then select
another coordinate system which has its origin at a different point on the surface of the workpiece.
