WEIHONG ELECTRONIC Ncstudio, Programming Manual

Page: 14 / 74

上海维宏电子科技股份有限公司
Weihong Electronic Technology Co., Ltd.
Specialized, Concentrated, Focused 11
G28 Auto Back to Reference Position
Command Format: G28 X_Y_Z_
Description:
X_Y_Z_: coordinates of the middle position (Workpiece Coordinates)
A machine tool returns to REFER point (machine origin) through the middle point, as shown in
Fig. 4-3.
A (0, 0, 10), target position, X and Y
back to origin, Z-axis keeps still.
Instruction: G28 X100 Y50
The machine Tool moves from
point C (current position) to
point A (machine origin) via
point B (middle point). Since Z
axis does not appear, Z axis
keeps still without returning to
zero.
C (40, 90, 10)
current position
B (100, 50, 10)
middle point
Fig. 4-3 Back to Reference Position
G992 Temporarily Set WCS according to Tool Position
Command Format : G992 X_Y_Z_ /I_J_K_
Description:
The function of this command is similar to G92 command. Their difference is: G92 command
alters the WCS permanently and takes the same standard to the whole system, while G992 command
alters the WCS temporarily and only influences the coordinate parsing of processing instruction,
which will be restored automatically at the end of machining.
The command can be used for implementing array function. The steps are as shown below.
Method one:
G992 X_Y_Z_
1. Delete M30 command in the processing file.
2. Adding the following contents at the beginning of the processing file:
#1=30
’X offset value
#2=40
’Y offset value
#3=30
’machining quantity along X axis
#4=30
’machining quantity along Y axis
G65 P3455 L=#4
G00 G90 X=-#1*#3 Y=-#2*#4
G992 X0 Y0
M30
O3455
G65 P3456 L=#3
G00 G90 X=-#1*#3 Y=#2
G906