G43: Tool Length Compensation (+) - Mitsubishi Electric MELSEC iQ-R16MTCPU Programming Manual

G43: Tool length compensation (+)

Adds the set compensation amount to the movement command. By setting actual difference from the tool length as the
compensation amount, programs can be created without having to remember the tool length.
Code
G43
Processing details
• When G43 command is executed, the compensation amount set in [Motion Control Parameter][G-code Control
Parameter][G-code Control Work Parameter]"Tool Compensation Data""Tool Length Compensation Amount" is
added to the end position of the movement command.
• The G43 command is modal. Compensation continues until tool length compensation cancel (G49) is commanded.
• When "0" is specified as the tool No., the tool length compensation command is cancelled. However, when an axis address
is specified in the same block, tool length compensation is only performed for that specified axis address.
G43 H0 (With tool No. as 0, tool length compensation is cancelled)
• The G43 command calculates the movement amount by the following calculation.
Program
G43 Z10. H01
• When G43 is commanded again during tool length compensation, only the difference between the compensation amounts
of the compensation Nos. is compensated.
Program
G43 Z10. H01
:
G43 Z10. H02
• For movement commands to the machine coordinate system (G53 command), movement to the machine position is made
with tool compensation amount cancelled. When returning to work coordinate system (G54 to G59), the tool compensation
amount is added to the position again.
• When transitioning to G-code control, or after resetting, the mode changes to G49 (tool length compensation cancel).
• Tool length compensation is valid for the axis addresses commanded in the same block as G43. The valid axis addresses
are those set in [Motion Control Parameter][G-code Control Parameter][G-code Control System Parameter]"Plane
Composition""Base Axis I to K" only. (The details below are based on the following address settings: Base axis I="X",
base axis J="Y", and base axis K="Z".)
• When there is no axis address specified in the same block as G43, tool length compensation is valid for the Z-axis.
However, when base axis K has not been set tool length compensation is not performed.
• Tool length compensation is a command only valid for one axis. When two or more axes are commanded at the same time,
the order of priority is "Z > Y > X".
Ex.
The following shows the valid axis for compensation for the following programs
Program
G43 X10. H01
G43 X10. Y10. Z10. H01
G43 H01
5 G-CODE CONTROL PROGRAMS
132
5.6 G-Code
Format
G43 Z z H h
Tool No.
Coordinate command
Z-axis movement amount
10+(Tool length compensation amount of tool No. 01)
Z-axis movement amount
10+(Tool length compensation amount of tool No. 01)
:
10-(Tool length compensation amount of tool No. 02-Tool length compensation amount of tool No. 01)
Axis for compensation
X-axis is valid
Z-axis is valid
Z-axis is valid
Operation
Compensation in the + direction for the tool
compensation amount only