Re: Intro and Beginners

--- In CAD_CAM_EDM_DRO@yahoogroups.com, "Tony Mori" <tonym@c...>
wrote:

> Still some things I need to understand in the computerized and CNC
> world of machining.
>
> I understand how the CNC works, and the principles. I just have
> a hard time understanding how you start, ie, tell the software that
> the slide is here, the tool is angled this way, etc... you know: the
> EXACT position of the tool in relation to the material, so it knows
> how/where to move it.

The CNC coordinate system on a mill locates the spindle center.
The part is located with respect to the CNC coordinate system.

You may use an edgefinder to locate the X and Y edges of a
rectangular piece of material which has been clamped parallel to the
X and Y axes. This corner is where your zeros are set. Any time you
command movement to X0 Y0 the machine will return to that corner.

When you cut, you program the tool center movement with respect to
this zero corner. With a flat bottomed end mill, the programmed cuts
will be offset from the final size by one radius of the tool.

For a simple example

Set your zero point at the front(Y) left(X) corner of your stock. If
you wanted to cut a 4 inch square with a 1/4 cutter, you would
program a move to Y=-.125 and the first side from X-.125 to X4.125
Next side Y4.125
Next Side X-.125
Last side Y-.125 (return to the beginning)

Here is the whole program (Z depth is left off for simplicity):

G0 X-.125 Y-.125 (G0 rapid movement)
G1 X4.125 F10.0 (G1 feed controlled movement 10 inches per minute)
Y4.125
X-.125
Y-.125
M2

Z zero is usually set by touching the tool to the top of the
material, or to a piece of paper between the cutter and the top of
the material (gently, oh so gently, with .001 incremental jogs).
There are much more sophisticated methods, but for a beginner this is
the way to start.

Adding Z movement to the above program will actually cut the part,
instead of just tracing the outline.

G0 X-.125 Y-.125
G1 Z-.125 F2.0 (plunge to depth usually slower that cut along feed
rate)
G1 X4.125 F10.0
Y4.125
X-.125
Y-.125
Z1.5 (Retract tool to 1.5 inches above the part)
M2



Lathe is similar, but the part crossection is programmed, instead of
the sidewall as in milling. The tool path is not offset but is
compensated by the turning tool, nose radius.

Fred Smith - IMService