Re: (unknown)

--- In CAD_CAM_EDM_DRO@y..., "Tim Goldstein" <timg@k...> wrote:

> G43 is tool length offset. Not sure on G44
>
> Tim
> [Denver CO]

Tool Length Compensation Syntax -

G43 Hnn* ; tool length comp. away from the part

G44 Hnn* ; tool length comp. toward the part

G49* ; cancel tool length compensation

The parameter nn for the H code is the identification number of the
associated tool. This value is the tool number displayed on the left
side
of the screen in the Tool Size window.


G43 - Tool Length Compensation Away From The Part
G43 assumes zero length tools, meaning the G-code tool, or z-axis,
coordinates will specify the length from the quill face to the desired
destination position. The offset associated with the tool will then
be
added to the tool axis destination position. The tool offset data
for this command will be the actual length of the tools.

Example:
If the distance from the quill to the destination position is 10
inches
towards the part for the rapid move and 10.5 inches for the feedrate
move,
and you want to apply tool length compensation away from the part for
tool
number 0, the G-code commands will be:

G43 H0* ; enable tool length compensation for tool number 0
G00 Z-10.0 G90* ; lower the tool at the rapid rate in G90 absolute
mode
G01 Z-10.5 F10.0* ; lower the tool to the cutting position at 10 ipm

If the z axis starting position was at 0 and the offset length
assigned in
the Tool Size window for tool number 0 was 7.5 inches, the actual
length of
the G00 move in this case will be 10.0 - 7.5 = 2.5 inches. The offset
length is always subtracted when G43 compensation is active. The next
command will move the tool down an additional .5 inches, at a
feedrate of 10
inches per minute.

If a tool change was required at some later point it would only be
necessary to cancel the current tool length compensation, retract the
tool
to the tool change position, and re-enable the compensation while
specifying
the tool to use for the operation, using the 'Hnn' parameter.
However, the
offset length must have been previously assigned for this tool before
the
file is executed. These additional commands might be:

G49* ; cancel tool length compensation
G00 Z0 G90* ; retract to tool change position
M01* ; program pause for the tool change
G43 H01* ; re-enable compensation for tool number 1
G00 X2.0 Y1.0* ; position the tool
G00 Z-10.0 G90* ; lower the tool at the rapid rate
G01 Z-10.5 F10.0* ; lower the tool to the cutting position at
10 ipm

The last 2 commands simply continue the sequence of tool axis moves
in a
similar way as before. Even though the lengths of the two tools may
be
different, the G-code commands to move the tool to the same
destination
position remain the same as long as the offset length for each tool is
specified properly. Remember that the offset length specified in the
Tool
Size window, must be the actual length of the tool when using the G43
command.

It can be seen from these examples the danger in using the G43
compensation
command. Because this command compensates the tool away from the
part and
assumes a zero length tool, the coordinates in the tool axis moves
are all
longer than actually desired. The compensation actually reduces the
length
of travel by the amount assigned in the Tool Size window for the
offset
length for the specified tool. If this value is assigned a zero the
tool
move will travel too far, possibly resulting in a collision with the
part
or table.

Please make sure you dry run the program from the Main Screen before
execution, if you use the G43 command, to check the proper display
position
of the z-axis coordinate. Never assume the Tool Size data still
exists or
have the same data the was previously assigned. This data is stored
in DOS
files which can easily be deleted, overwritten or otherwise
corrupted. At
the very least you should check to make sure the Tool Size data is
still
valid before you run G-code files containing tool length compensation
commands.


G44 - Tool Length Compensation Toward The Part
G44 assumes that when creating G-code commands, the tool axis
coordinates
are assigned based on a standard length, for an imaginary tool, which
is longer than any of the tools in the system. The tool offset length
data
in this case will be the difference in length between each tool and
the
standard tool length chosen by the programmer. The offset for this
command
will be subtracted from the tool axis destination position.

An extra calculation is required when using the G44 command, since
after the
tool length is measured it must be subtracted from the chosen standard
length, to obtain the desired offset. It is this difference that is
stored
as the offset length in the Tool Size window for each tool which will
be
used in a G44 tool length compensation operation.

This method of tool length compensation is actually safer than using
the
G43 method, since the coordinates for tool move commands will be
programmed
with a shorter value than is desired. If an offset has not been
assigned
for the selected tool the resulting move will be shorter than desired
and a
collision with the part or table should not occur.

Example:
If the distance from the tip of the standard length tool and the
destination
position is 2.0 inches towards the part for the rapid move, and 2.5
inches
for the feedrate move, and you want to apply tool length compensation
toward the part to tool number 0, the G-code commands will be:

G44 H0* ; enable tool length compensation for tool number 0
G00 Z-2.0 G90* ; lower the tool at the rapid rate in G90 absolute
mode
G01 Z-2.5 F10.0* ; lower the tool to the cutting position at 10 ipm

If the z axis starting position was at 0 and the offset length
assigned in
the Tool Size window for tool number 0 was .5 inches, the actual
length of
the G00 move in this case will be 2.0 + .5 = 2.5 inches. The offset
length
is always added when G44 compensation is active. The next command
will
move the tool down an additional .5 inches at a feedrate of 10 inches
per
minute.

As with the G43 command, additional tools could be used at later
points in
the G-code program. As long as the tool length offsets were properly
assigned, the tool axis coordinates would simply reflect the length
of the
standard tool, and the program would compute the actual destination
positions for the specified tool.


Since the tool length compensation commands allow the programmer to
create
G-code programs that are not dependent on the lengths of the various
tools
that will be used, the programs will be easier to write and
maintain. With
this greater flexibility and freedom comes additional danger and risk
if the
commands are not used properly. This is especially true with the G43,
compensate tool away from the part, command. If you decide to use
these
commands please take extra precautions to verify the correctness of
the
program before actually driving an expensive power tool.


G49 - Cancel Tool Length Compensation

The G49 command is used to cancel any active tool length compensation
operation. If you want to perform a tool change you will almost
certainly
want to include a G49 command before the retract move is made. If
this is
not done the retract operation may not be moved to a point that
provides
adequate clearance for the tool change operation. After the
specified tool
change or pause command, the previous tool compensation command
should be
included, to re-enable this operation for the new tool, if so desired.

> > -----Original Message-----
> >
> > hi all
> >
> > what is g43/44 for?
> >
> > JS
> >
> >
> > Addresses:
> > FAQ: http://www.ktmarketing.com/faq.html
> > FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/
> > Post Messages: CAD_CAM_EDM_DRO@y...
> > OFF Topic POSTS: General Machining
> > If you wish to post on unlimited OT subjects goto:
> > aol://5863:126/rec.crafts.metalworking or go thru Google.com
> > to reach it if you have trouble.
> > http://www.metalworking.com/news_servers.html
> >
> http://groups.yahoo.com/group/jobshophomeshop I consider this to

be a

> sister site to the CCED group, as many of the same members are

there,

> for OT subjects, that are not allowed on the CCED list.
>
> NOTICE: ALL POSTINGS TO THIS GROUP BECOME PUBLIC DOMAIN BY POSTING

THEM.

> DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........ bill
> List Mom List Owner