Re: [CAD_CAM_EDM_DRO] CNC Process

cadman@... wrote:

> I am new to using a CNC machine. I built a small (made of wood) 3
> axis mill so I could play and learn with. Later I will purchase a
> Drill/Mill and convert it. As of today I am using CNC-Pro
>
> I don't have any problems with the CAD/CAM software side of things.
> It is running the machine that has me stumped. The areas that I have
> questions are:
>
> 1. Home position.... When I press the Home button it moves my
> axis all the way to one side and sets the coordanants to 0,0,0 should
> this be left at 0,0,0 or should I touch my tool on top of the material
> and call that 0 in the z-axis?

In general, I can't comment on CNC-Pro specifically, you want
to home to MACHINE-specific points, which are repeatable over a
long time, and then keep the offsets from machine home to a fixture
location or part location.

> 2. When I need to change a tool I will loose the z-axis tool
> location. do I again touch the tool on the top of the part for z=0 or
> should I re-home?

If you use collets, then there is no way to repeatably insert a tool into
the spindle. Generally, you could touch the tip of the tool to the
top of the part, or the plane the part is seated on, and set Z=0
with the MDI command G92 Z0.

If you use tool holders which are repeatable (indexable end mills
with taper matching the spindle all in one piece, end mills or similar
tools in end mill holders, drills left in drill chucks on a tapered
arbor, etc. then you can repeatably position the tool in the spindle,
and an offset can be but in the tool table to supply the CNC with the
required length.

This is how I do it. I have made a tapered socket that matches the R-8
taper of my bridgeport mill. It sits flat on a surface plate. I use a
height gauge to mearure the height with the tool in the socket, and
record that measurement. I also have a "master tool" whose length
is known, and it often used first. It is, in my case, a center drill.
I put in the tool table the DIFFERENCE between the master tool and
all other tools. When I use the master tool first, I touch it to the
work, and set Z=0 with the G92 Z0 command. The length of this
tool is entered in the tool table as 0. (I could actually put the true length
of this tool in the table, and then load the tool table with actual lengths
of all tools, but I didn't think of that at the time.)
When I switch tools, my toolpath programs turn on tool length
compensation, and that activates the length offset from the tool table,
and all the tools will come down and touch the reference plane
(generally, for me, the top of the part) when Z is commanded to go
to 0.0)

> 3. If I rough the part and loose the top of the material (by cutting
> away all the material on top) How can I set the tool again?

If you are going to remove your reference points, then don't use those
for reference points. One method is to use the bed of the vise (or top
of the machine table) as your Z reference instead. But, by using the
length compensation method described above, you should be able
to reproduce the coordinate system from the machine home position
(assuming tool lengths are reproducible).

>
> I am so confused about setting the machine up for a job. I have the
> limit (home switches) set at the far positive position in all axis. Z
> moves up. X table moves to the left. Y table moves to me. So this
> means that the tool in relation to the table will move Z-up, X-right,
> Y-Away.

Yes. Forget table movement. Look at the part, think of it with
+Z up from the table, +X to the right, and +Y up, when looking down
onto the part.
As if you had a piece of graph paper with X right and Y up taped
to the top of the part. Then, the tool is moving over those coordinates
as you would expect.

> When I use the homing feature it sets 0,0,0 at the home position.
> This means that I always cut in the negative space. Is this correct?
> What is the best method?

Don't worry about machine coordinated. That is a reference system
for the machine, internally. You should be able to set a part
coordinate system that is offset from the machine's coordinates,
with the G92 command. If you jogged the machine so that the
tip of the tool was at the X=0, Y=0 and Z=0 coordinates, then
you enter G92 X0 Y0 Z0 to set the part coordinates to zero at
that location. (The CNC control keeps the offset between these
two systems, and generally, you can recall that offset when you
restart the CNC the next day.)

Jon