G41: Tool Radius Compensation - Left - Mitsubishi Electric MELSEC iQ-R16MTCPU Programming Manual

G41: Tool radius compensation - Left

The actual path of the tool center for the programmed path is compensated by an amount of the tool radius. The path is
calculated by intersection operation method therefore the overcutting of inside corners can be prevented.
Code Format
G41
G41 X x
Processing details
• When G41 command is executed, the tool radius compensation amount set in [Motion Control Parameter][G-code
Control Parameter][G-code Control Work Parameter]"Tool Compensation Data""Tool Compensation Data" is added
to the end position of the movement command, and outside or inside compensation is performed for movement.
• The G41 command is modal. The compensation amount is kept until tool radius compensation cancel (G40) is
commanded.
• In tool radius compensation, H commands are ignored and only D commands are valid.
• When "0" is specified as the tool No., the tool radius compensation command is cancelled.
G41 D0 (With tool No. as 0, tool radius compensation is cancelled)
• Tool radius compensation is performed on the plane selected in [Motion Control Parameter][G-code Control
Parameter][G-code Control System Parameter]"Modal Initial Setting""Plane Selection". Compensation is not
performed on axes that are not included in the specified plane.
• The operation for when compensation amount is set as a positive value (+), and negative value (-) is shown below.
<When compensation amount is (+)>
• Refer to tool radius compensation for details of tool radius compensation. (Page 183 Tool radius compensation)
Program example
■Program that starts tool radius compensation (left) and performs positioning
Tool radius compensation amount is "compensation No.: 10", "compensation amount: 10[mm]"
Operation Program
(1) G90 X0. Y0.
(2) G91 G01 G41 X40. Y40. D10 F500.
(3) G01 X30.
*1 Describes the tool center position.
Y
70
60
(3)
50
40
30
(2)
20
10
(1) 10 20 30 40 50 60 70
Y y D d
Tool No.
Coordinate command
<When compensation amount is (-)>
: Program path
: Tool center path
X
[Unit: mm]
: Program path
: Tool center path
*1
Remarks
Move to "X0,Y0" by absolute position command
Move to "X40,Y50" by tool radius compensation start operation
Move to "X70" by straight line
5 G-CODE CONTROL PROGRAMS
5
127
5.6 G-Code