Brother TC-32B - Tool Length Offset (G43, G44, G49); Tool Length Fine Offset

TC-32B Chapter4 Preparation function (Tool offset function)
2004/01/22 4 - 31 eTCOMNCPR4.doc
4
4.2 Tool Length Offset (G43, G44, G49)
This function corrects the tool position so that the tool nose comes to the programmed position.
In either the absolute command or the incremental command, the end point in the
programmed Z-axis move command is offset as specified by H code to become the actual end
point.
(1) Tool length offset (+)
Command format G43 Hn
Hn: Tool length offset No. (n=0~99)
(Note)
The offset amount of H0 is always zero.
The offset amount is set on the tool data setting screen.
The tool length offset is done in the Z-axis direction.
(2) Tool length offset (-)
Command format G44 Hn ;
Hn: Tool length offset No. (n=0~99)
(3) Tool length offset cancel
Command format G49
(Note 1)
The tool length offset can be cancelled by commanding G49 or specifying zero for
the tool length offset number.
(Note 2)
The tool length offset is cancelled by M06 (tool change) or
G100 (non-stop ATC).
(Note 3)
If the Z-axis command is not given to the block of "G43H_;" or "G44H_;", it
isregarded that the Z-axis command is given to the current position and Z
axismoves by the offset amount specified by the H code.
In the same way, if the Z-axis command is not given to the block of "G49;", it is
regarded that the Z-axis command is given to the current position and Z axis moves
by the offset amount specified by the final H code.
(Note 4)
If the Z-axis command of the reference point return (G28) or the 2nd, 3rd,4th
reference point return (G30) is given, the tool moves while the tool length offset is
applied to the intermediate point and the tool returns to the reference point by
cancelling the tool length offset tentatively.
The Z-axis movement afterwards is executed with the tool length offset.
If the incremental mode is selected at this time, the tool movement is regarded to
start from the reference point.
(Note 5)
When G53Z_; is commanded during tool length offset, tool length offset is canceled
temporarily and the Z axis moves to a certain point.
4.2.1 Tool length fine offset
When G43 and G44 are commanded in the program, the tool length fine offset value
corresponding to the commanded tool No. is added to the tool length offset value.
Offset value to be reflected = Tool length offset value + Tool length fine offset value.
The tool length fine offset value is placed on the tool list screen.