Re: Setting Coordinate Systems

Matt Shaver wrote:

> From: "Matt Shaver" <mshaver@...>
>
> > From: D.F.S. <dfs@...>
> > How could the system intelligenty do a "Tool Change" without simply
> > making me do absolute positioning of the entire table based on
> presumed
> > tool location.
> >
> > I'd like to be able to go back to an old G code file and make a new
> part
> > months later.
> > I REALLY like to be able to set the tooling up in about the same
> locations,
>
> > and recalibrate the system on a tool-by-tool basis, rather than
> trying to
> > bold every single tool back in an exact location down to the
> ten-thousanths
> > or have a new part that is out of whack.
> >
> > Is this something the system can do with tool offsets? or is this
> more
> > complicated than that?
>
> Some controls (this includes the EMC) have "work coordinate systems"
> or
> "fixture offsets" that can be independently adjusted and called up as
> required in your program. The G-codes in the EMC are G54 (default),
> G55, G56,
> G57, G58, G59, G59.1, and G59.2 for a total of 8 plus the G53
> coordinate
> system which is non-adjustable and refers to the machine's basic
> position. In
> other words, no problem for 8 tools or less.

Also, there is a tool length offset (G43 and G44, I think) command that
uses the tool length
specified in the tool table to correct for variations in tool length.
See my little description
of a cheap tool presetter
http://www.artsci.wustl.edu/~jmelson/preset.html for the
physical part of how I do it. Once I have the tools measured, I just
enter the difference
between the 'master' tool, and the other tools. The 'master' tool has
an assumed length
of 0, and all other tools have a length based on the difference from the
master.
You usually set up so the master tool is the first one used. You lower
this tool until
a piece of paper cannot be moved under the tool. Assuming the paper is
.005" thick,
you do a G92 Z.005 to set the coordinate system for Z. You also enter
the difference
between the master tool's length and the other tools that will be needed
into the tool table,
so that if a 1/2" enc mill is 1.567" longer than the master, its entry
in the tool table would
be 1.567. When the 1/2" end mill is called for in the program, and it
is tool #4, you
have a line of G-code in the program that says G43 L4 to correct the Z
axis
to account for the tool length difference. Use G49 to reset to the
original
coordinate system.

See http://206.19.206.56/rs274.htm for some more details on this.
I have used this method with excellent results, and get parts within
.001 to .002"
of the desired height, which is about the best my machine can do for
overall
accuracy, anyway.

There is no need to worry about X and Y coordinates on a tool change,
they
are not affected. If you have an accurate fixture, changing parts will
not
affect these coordiantes, either. To align to an edge of the part for
your
first part, you use an edge finder. For instance, to set the lower left

corner to be coordinate (0,0), you would first bring the 'bottom' of the

part against the edge finder until it deflects, and enter G92 Y-.1
(compensating
for the edge finder's .2" diameter sensing end) then move the left
edge of the part against the edge finder, and enter G92 X-.1 to
set the X coordinate. Raise the edge finder and center the end
of it with respect to its body, and then enter X0 Y0 to bring the
table to (0,0). If the edge finder appears well centered over the
corner of the part, you got the minus signs, etc. correct in the above
MDI entries. When setting various corners as the reference edge,
it is common to enter a -.1 when a +.1 was the correct thing to
do, this will cause a .2" error in one axis, so I always check the
(0,0) to make sure I didn't goof.

Jon