Programming Chapter Three Commands and Functions
92
3.1.7 G26
—
Reference Point Return
Command format
：
G26 ;
The tool returns to the reference point( machining starting point) with G26, and the mode of the
reference point return with G26 is the same that of G00. See Fig. 13:
Reference point return
：
After executing G commands, X, Z moves to the point defined by G50. Without G50 in the
program, move to the reference point defined in
“Manual”
mode with G26. Define the point with
G50 as the reference point if the user does not define the reference point in
“Manual”
mode. The
system defaults X=150
，
Z=150 as the reference point if it has never defined the reference point.
If the system executes the first motion after G26 in the program without G50, it must firstly
position with the command in X, Z absolute programming mode, otherwise the following
command after G26 cannot be executed rightly. X, Z move from A to the reference point B
simultaneously and respectively at max. rapid traverse speed and the speed defined by the rapid
traverse override.
When the system uses G50 in the program to define the reference point, the tool retracts to the
point defined by G50 after executing G26, and the following program is needed to execute the
programming. Without G50 in the program, G26 is executed according to the position of
reference point defined by user in
“Manual”
mode. Take the previous position defined by G50 as
the reference point which is not defined by user. The system will default X=250
，
Z=250 as the
reference point if the system has never defined it. When the system uses G26 without G50, must
position again with G0 before executing the traverse command behind G26, otherwise the
following command cannot be executed rightly.
Note 1:
After the tool returns to the reference point with G26, it must position simultaneously X, Z
absolute coordinates with G00 to continuously
traverse
, which is contributed to the right
motion.
Note 2:
The tool returns to the reference point with G26 at the speed defined (rapid traverse
speed) by G00 and controlled by the rapid traverse override.
Note 3:
After the tool returns to the reference point with G26, the offsets of tool and system are
cancelled.
3.1.8 G27
—
X Reference Point Return
Command format
：
G27 ;
After X returns to the reference point with G27 at the rapidest traverse speed controlled by the
rapid traverse override, X offsets of tool and system are cancelled. When Z offset value is also 0,
the tool offset number is displayed to 0.
Fig. 13 G26 reference point return
