Fanuc Power Mate i-D/H Operator Manual

PROGRAMMING
(Common to Power Mate i–D and –H)
12. COMPENSATION FUNCTION
B–63174EN/03
98
Select tool length offset A, B or C, by setting bits 0 (TLC) and 1 (TLB)
of parameter No.5001.
When G43 is specified, the tool length offset value (stored in offset
memory) specified with the H code is added to the coordinates of the end
position specified by a command in the program. When G44 is specified,
the same value is subtracted from the coordinates of the end position. The
resulting coordinates indicate the end position after compensation,
regardless of whether the absolute or incremental mode is selected.
If movement along an axis is not specified, the system assumes that a
move command that causes no movement is specified. When a positive
value is specified for tool length offset with G43, the tool is moved
accordingly in the positive direction. When a positive value is specified
with G44, the tool is moved accordingly in the negative direction. When
a negative value is specified, the tool is moved in the opposite direction.
G43 and G44 are modal G codes. They are valid until another G code
belonging to the same group is used.
The tool length offset value assigned to the number (offset number)
specified in the H code is selected from offset memory and added to or
subtracted from the coordinates specified by a command in the program.
The tool length offset value may be set in the offset memory through the
CRT/MDI panel.
The range of values that can be set as the tool length offset value is as
follows.
Metric input Inch input
Tool length offset value 0 to ±999.999mm 0 to ±99.9999inch
WARNING
When the tool length offset value is changed due to a
change of the offset number, the offset value changes to the
new tool length offset value, the new tool length offset value
is not added to the old tool length offset value.
H1 : tool length offset value 20.0
H2 : tool length offset value 30.0
G90 G43 Z100.0 H1 ; Z will move to 120.0
G90 G43 Z100.0 H2 ; Z will move to 130.0
NOTE
The tool length offset value corresponding to offset No.0,
that is, H0 always means 0. It is impossible to set any other
tool length offset value to H0.
Explanations
Selection of tool length
offset
Direction of the offset
Specification of the tool
length offset value

Leave a Reply

Your email address will not be published. Required fields are marked *