21
Each block (line) in the program must start with a G- or M-code. None of the data entered before a G-
or M-code will be interpreted.
Incorrect parameters for a given G-code will not be interpreted.
If a parameter appears twice in a given block (e.g. G00 X2.0 X3.00), it will have the value of the last
entry (in this case,
“
X
”
will have the value of X=3.0).
It is not possible to add comments to the file that contains a stored program.
3.5.1
G-codes (preparatory functions)
Table 3.2. A list of the available G-codes
–
Preparatory functions
G00
linear interpolation at fast feed (under construction)
G01
linear interpolation at slow feed
G02
circular interpolation clockwise
G03
circular interpolation counter-clockwise
G50/G59
selection of a base co-ordinate system
3.5.1.1
G00/G01 Linear interpolation at slow feed
X
- movement command for the X-axis (endpoint X coordinates)
Y
- movement command for the Y-axis (endpoint Y coordinates)
Z
- movement command for the Z-axis (endpoint Z coordinates)
A
- movement command for the A-axis (endpoint A coordinates)
A program that carries out drilling to the depth of 2mm:
Absolute:
Incremental:
%
G56
G90
G00 X0 Y0 Z0 A0
G01 Z-2.0
G01 Z0.0
%
%
G56
G00 X0 Y0 Z0 A0
G01 Z-2.0
G01 Z+2.0
%
3.5.1.2
G02 Circular interpolation clockwise
X
- movement command for the X-axis (endpoint X coordinates)
Y
- movement command for the Y-axis (endpoint Y coordinates)
Z
- movement command for the Z-axis (endpoint Z coordinates)
I
- distance along the X-axis toward the centre of wheel
J
- distance along the Y-axis toward the centre of wheel
Presented below is a program that carries out an arc at the inclination angle of 130˚ and 5mm radius:
Absolute:
%
G56
G90
G00 X0 Y0 Z0 A0
G00 X1.79 Y3.83 Z0 A0
G02 X10.0 Y0.0 I3.21 J-3.83
%
Incremental:
%
G56
G00 X0 Y0 Z0 A0
G00 X1.79 Y3.83 Z0 A0
G02 X8.21 Y-3.83 I3.21 J-3.83
%
