G40/G41/G42: Tool radius compensation
It is used to compensate for the radius of the cutting tool. A new path is created either inside or outside the programmed tool path, and movement is performed along this new path.
|
Format: |
G41/G42 D_ |
|
Format: |
G40 |
G41: Tool radius compensation left
G42: Tool radius compensation right
D: The offset number where the radius compensation value to be applied is written
G40: Tool radius compensation Off
When tool radius compensation is applied, the consecutive movements within the program are pre-read, interpreted, and a new vector path is generated. The tool is then moved along this new path. To achieve correct results while using this function, the number of lines between two movements should be no less than 10. During the creation of the new path, if the target coordinates of the next line cannot be found, the tool is positioned 90 degrees to the left or right of the target of the processed line. If the angle between two consecutive movements is less than 180 degrees, trimming is performed at the end of the processed movement and the beginning of the next movement. If the angle between two consecutive movements is greater than 180 degrees, an arc is added connecting the starting points of both movements.
When the tool radius compensation command is given, the following first movement must be linear. Tool radius compensation should not be initiated with an arc movement.
Example:
G00 G53 Z0. (Z REFERENCE)
M3 S1000 (SPINDLE CW ROTATION)
G41 D1 (RADIUS COMPENSATION LEFT)
G90 G00 X100. Y100. (RAPID MOVEMENT TO X100 Y100 POINT)
G90 G00 Z10. (MOVE TO THE SAFE Z POSITION)
G01 Z-1. F500 (ENTER THE WORKPIECE AT F500)
Y550. F1000. (PERFORM CUTTING AT F1000 UNTIL Y550.)
X350. (PERFORM CUTTING AT F1000 UNTIL X350.)
Y100. (PERFORM CUTTING AT F1000 UNTIL Y100.)
X100. (PERFORM CUTTING AT F1000 UNTIL X100.)
G40 (RADIUS COMPENSATION OFF)
G00 G53 Z0. (Z REFERENCE)
G00 X0. Y0. (MOVE THE TOOL AWAY FROM THE CUTTING AREA)
M5 (SPINDLE STOP)
M30
%