Re: would like to know...

WAnliker@... wrote:

> How are tool changes handled in the smaller equipment like the Sherline, and
> the modified manual machines?
> I realize that it has to be done by hand, but how is the programing handled,
> so that machine can be powered down, and restarted when tool is changed.

Well, an M02 is a temporary stop in the program, not the end. So, the
control waits for a manual command to 'un-pause'. There are also
commands to stop the spindle, coolant, etc. I don't have the spindle
control hooked up yet, so I manually stop the motor, but the program
has to retract the quill, and maybe move the table so there is sufficient
clearance to pull the tool holder out of the spindle. I have gotten a selection
of end mill holders to mount all the different sizes of tools at repeatable
Z offsets. I made a thing that looks like a cylindrical parallel, but has an
R-8 taper socket in it. I can measure the length of a tool, and reference
it to some 'master' tool. I use a center drill for my 'master' reference.
You can see some bad pictures of this at :
http://www.artsci.wustl.edu/~jmelson/preset.html
Most CNC controls have a tool length offset feature for this purpose.
You set the 'master' tool so that Z=0.0 when the tool is touching the
top of the work (or the surface the work will be placed on, if you
have Z=0.0 for the bottom of the part). You then enter the offsets
(the difference between the master length and that tool's length)
into the tool length offset table. When the program selects the new
tool, it will add the offset to the requested Z position, to compute
the position to move the tool to.

>
> Also in the programs I have looked at, commercial, the characteristic's of
> the tool are placed into the program.

It is not necessarily in the program, but for the sake of remembering what
tool to use, it should at least be a comment. RS-274D comments look like
N0100 (Insert .500" end mill)

> How is this done in the small programs for the Sherline's , etc.? Also how
> is the tool position and the program synchronized at the start of machining?

Using a .200" edge finder near the lower left corner of a part, you would
touch it to the left side, and then enter in MDI mode G92 X-.1
because the edge finder's center is .1" left of the part. Then, touching
the edge finder to the bottom edge, you'd enter G92 Y-.1.

Then, for setting height/depth, I often use either a center drill or an
end mill for the first operation. So, I lower the tool until it almost
touches the top of the part, then I slip a piece of paper I know is
.005" thick under the cutting edge, and jog the tool at an extremely
slow feed rate until the paper drags under the cutting edge. Then, I
enter G92 Z.005 (because the tool is about the thickness of the
paper above the top surface of the part).

> And after a tool change?

If the tool length is preset, and the program will call up the correct
tool length offset (by tool #) then you do nothing. Otherwise, you
need to do the 'touch off' thing above to reset the Z coord. The
X and Y will not be affected.

Jon