G28 Return To Reference Point - Omron NY532-5400 Instruction & Reference Manual

2 G Code

G28 Return to Reference Point

This instruction returns the tool automatically to the reference point via the specified middle point.
Modal/Non-modal
Modal group
Instruction format
Relevant G codes
Parameters
Parameter
X
Y
Z
A
B
C
Function
The G28 command moves the tool to the optional middle point at rapid feed, then returns it to the refer-
ence point. If the middle point is not specified, the tool returns directly to the reference point.
• The tool is moved to the reference point (position 0) via the middle point.
• The middle point follows the specifications for the Absolute Dimension (G90) and Incremental Dimen-
sion (G91).
• The only axis that operates is the one for which the middle point is specified.
• Motion to each point follows the Rapid Positioning (G00) specifications.
• After the middle point is reached, this command releases Scaling (G50/G51), Mirroring
(G50.1/G51.1), and Coordinate System Rotation (G68/G69). During motion between the middle point
and reference point, this command also releases Zero Shift (G54 to G59) temporarily. It maintains the
current status of Inch Input (G20) and Metric Input (G21). Tool Offset (G43/G44/G49) and Cutter
Compensation (G40/G41/G42) must be released prior to execution of this command.
2 - 36
Non-modal
00 Non-modal
G28 X- Y- Z- A- B- C-
G90, G91, G50, G51, G50.1, G51.1, G68, G69, G54 to G59, G40, G41, G42, G43,
G44, G49
Name
X-axis middle point
Y-axis middle point
Z-axis middle point
A-axis middle point
B-axis middle point
C-axis middle point
Description
Specifies a middle point [command units] on the X-axis.
Specifies a middle point [command units] on the Y-axis.
Specifies a middle point [command units] on the Z-axis.
Specifies a middle point [command units] on the A-axis.
Specifies a middle point [command units] on the B-axis.
Specifies a middle point [command units] on the C-axis.
NJ/NY-series G code Instructions Reference Manual (O031)