Tool Length Compensation; Tool Radius Compensation - Mitsubishi Electric MELSEC iQ-R16MTCPU Programming Manual

Tool compensation No. (H/D)
"H" and "D" are used as addresses for specifying tool compensation Nos.
A maximum of 40 groups can be used between lines.
H is used for tool length compensation, and D is used for tool radius compensation.
Tool compensation

Tool length compensation

Tool radius compensation

■Points
• Tool compensation No. is modal data. Once specified, it remains in effect until a new "H" or "D" is commanded.
• A tool compensation No. can only be commanded once in a block. When commanded more than once in a block, the last
commanded tool compensation No. is valid.
• When the tool compensation No. is outside of range, a minor error (error code: 1FC3H (details code: 030DH)) occurs.
• When H0 or D0 is specified, tool length compensation or tool radius compensation is cancelled.
Tool length compensation
Controls movement so that the position of the end point of the movement command of each axis can be changed to a position
that considers the compensation amount set in tool compensation. By using the G43 command, G44 command, and G49
command, the difference between the position of the program coordinates and the tool tip position on the machine, which is
the tool length, is compensated.
Tool radius compensation
With tool radius compensation, the program path can be compensated for the compensation amount set in tool compensation
in a selected vector direction, using G-code commands or D commands.
There are two starting operations and ending operations for tool radius compensation: Type A and type B. Set the type of tool
radius compensation in [Motion Control Parameter][G-code Control Parameter][G-code Control Work Parameter]"Tool
Radius Compensation""Tool Radius Compensation Type".
Tool radius compensation start operation
With compensation cancelled, and all the conditions below satisfied, tool radius compensation starts. When starting
compensation, regardless of whether in single block operation or not, three blocks of movement command, or if there are not
three blocks of movement command, a maximum of five blocks are pre-read before execution. Also, during compensation, a
maximum of five blocks are pre-read.
• When compensation commands (G41, G42) are commanded.
• When the compensation No. for tool radius compensation is within the range.
• When the movement command is positioning (G00), or linear interpolation (G01).
When there is no movement command in the same block as a compensation command (G41, G42),
compensation operation is performed perpendicular to the direction of the next movement block.
Setting range
H01 to H40
D01 to D40
6 AUXILIARY AND APPLIED FUNCTIONS
6.4 Tool Compensation Function
6
183