20
3.
Before the reference point does not returning and the machine coordinate system is established, rapid
moving speed can be manually set parameters 0960-0962, manual rapid traverse rate F0 set by parameters
0966-0968.
4.
Machine homing operation by G28 is generally not in G90 absolute manner, If performing "G90 G28
X_Y_Z0;" statement would be in danger of a serious accident, it is generally requires the machine operating in
G91 homing mode, namely: G91 G28 X0 Y0 Z0;Back to the machine origin with intermediate point as current
point.
8 Coordinate System
8.1 Machine Coordinate System
The point that is specific to a machine and serves as the reference of the machine is referred to as the
machine zero point. A machine tool builder sets a machine zero point for each machine. A coordinate system with
a machine zero point set as its origin is referred to as a machine coordinate system. A machine coordinate system
is set by performing manual reference position return after power–on. A machine coordinate system, once set,
remains unchanged until the power is turned off.
Format:
G90
（
G53
）
X_Y_Z_
；
X_Y_Z_
；
Absolute dimension word
1.
Selecting a machine coordinate system (G53)
When a position has been specified as a set of machine coordinates, the tool moves to that position by means
of rapid traverse. G53, used for selecting the machine coordinate system, is a one–shot G code. Any commands
based on the selected machine coordinate system are thus effective only in the block containing G53. The G53
command must be specified using absolute values
（
G90
）
. If incremental values
（
G91
）
are specified, the G53
command is ignored. When the tool is to be moved to a machine–specific position such as a tool change position,
program the movement in a machine coordinate system based on G53.
Explanation:
1.
When the G53 command is specified, cancel the tool nose radius compensation and tool offset.
2.
Since the machine coordinate system must be set before the G53 command is specified, at least one
manual reference position return or automatic reference position return by the G28 command must be performed
after the power is turned on. This is not necessary when an absolute–position detector is attached.
8.2 Workpiece Coordinate System
A coordinate system used for machining a workpiece is referred to as a workpiece coordinate system. A
workpiece coordinate system is to be set with the NC beforehand (setting a workpiece coordinate system). A
machining program sets a workpiece coordinate system (selecting a workpiece coordinate system). A set
workpiece coordinate system can be changed by shifting its origin (changing a workpiece coordinate system).
8.2.1 Setting a Workpiece Coordinate System
A workpiece coordinate system can be set using one of three methods:
1.
Method using G92 :A workpiece coordinate system is set by specifying a value after G92 in the
program.
Format:
（
G90
）
G92 X_Y_Z_
;
2.
Automatic setting :The parameter is set to 1 in advance, a workpiece coordinate system is automatically
set when manual reference position return is erformed. This function is, however, disabled when the workpiece
coordinate system option is being used.
