30
Cutter Compensation
G40, G41 and G42
Format
Description
The movement of the tool specified by the program is the path taken by the center of the tool. Because the tool has a certain thickness
(i.e., a certain diameter), it will over-cut by an amount equal to its radius if the coordinates on the drawing are input just as they are.
To cut a shape as specified by the drawing, the tool must be made to move at a place which shifted away by a distance equal to the tool
radius. This is called the “tool-diameter offset.”
Using this function makes it possible to input the values from the drawing as coordinate values (or amounts of movement) with no need
for modification, thus facilitating programming. Also, if cutting is to be performed with a tool that has a different tool diameter, it is
only necessary to change the amount of offset.
The words for cutter compensation are “
G40
,” “
G41
,” and “
G42
.”
G40
: Cancel cutter compensation
G41
: Cutter compensation -- left
G42
: Cutter compensation -- right
G17
{
G00
G01
}
[X
x
][Y
y
]
{
G41
G42
}
{
G00
G01
}
G40[X
x
][Y
y
]
D
number
Parameter
Function
Acceptable range
Effective range
x
Coordinate or movement distance (X axis)
Range 1
Maximum cutting range
y
Coordinate or movement distance (Y axis)
Range 1
Maximum cutting range
number
Offset number
0—10
0—10
Restrictions on Cutter Compensation
Cutter compensation is subject to the following restrictions.
1.
Cutter compensation can be performed only in the XY plane.
2.
Do not position two or more blocks without X- and Y-axis motion commands next to each other during tool diameter compensation.
It may cause excessive or insufficient cutting depth.
3.
No interference check for cutter compensation is performed. However, an error is generated if an attempt is made to machine the
inner side of a circle or arc with an amount of offset that is larger than the radius for circular interpolation.
45
15
25
15
15
25
15
45
R15
R15
R
R15+
R
R15
R15
R15-
R
Workpiece
Tool
: Tool path
