G44: Tool Length Compensation - Mitsubishi Electric MELSEC iQ-R16MTCPU Programming Manual

G44: Tool length compensation (-)

Subtracts the set compensation amount from the movement command. By setting the actual difference from the tool length as
the compensation amount, programs can be created without having to remember the tool length.
Code
G44
Processing details
• When G44 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
subtracted from the end position of the movement command.
• The G44 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.
G44 H0 (With tool No. as 0, tool length compensation is cancelled)
• The G44 command calculates the movement amount by the following calculation.
Program
G44 Z10. H01
• When G44 is commanded again during tool length compensation, only the difference between the compensation amounts
of the compensation Nos. is compensated.
Program
G44 Z10. H01
:
G44 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 subtracted from 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 G44. 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 G44, 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
G44 X10. H01
G44 X10. Y10. Z10. H01
G44 H01
5 G-CODE CONTROL PROGRAMS
134
5.6 G-Code
Format
G44 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