re: EMC coordinate systems

John,

orig. snipped and answers below

>I'm working on setting up a benchtop mill with EMC. Can anybody
>suggest resources for dxf to NC tool generation?

Check the back msgs on the list. this comes up repeatedly.

>Also, I'm interested in determining coordinate systems for standard
>NC (EMC). (i.e. I'm trying to figure out how I need to set up +x,
>+y, and +z to work with standard NC output? Is z=0 essentially the
>endmill at it's lowest setting, and z=3 three inches off of the
>surface? I'm still figuring this out, but was hoping for some
>insight.

First re: XY, most mills and machining centers home to the most
positive (physical) position in all axes, and then call this zero.
The net effect is that you work(by default,see below)in quadrant III
(-x,-y)of the cartesian co ordinate plane.

Most routers/engravers home to the most negative (physical) point and
call it zero. This has the effect of allowing you to work(again, by
default) in quad. I (+x,+y).

Most CAD/CAM pkgs. default to lower left corner as 0,0. (origin)This
means (until and unless you reset it) you are drawing in QUAD I.
(Some CAD/CAM does put the origin 0,0 in the center of the screen.)

If your system allows offsets(most currently do); then this is
academic, since you will place/set the co ordinate origin where ever
"it makes the most sense" for what you are doing. (however, some
systems REQUIRE working in +,+ or -,- space.)

Now to Z: The Z axis is "homed" as above with XY. However, it is
nearly always "reset" to one of two positions:

1.Material surface becomes zero. Which means any negative z
coordinate will be cutting into the material. And positive coords
mean we're at/or above the surface of the stock. (flat stock assumed)

or...

2.Zero is assigned to a "release" or "clearance" plane. Historically
this is .100 above the stock surface; as machines get better and the
push for faster part cycle times increase, it is getting closer and
closer to the material! Sometimes this plane is set well off the part
(to clear clamps, or casting protrusions, for example).

Of the 2 methods, I recommend using the first. (you can still set a
"release" plane in most software which will be used for canned
cycles,etc. to prevent crashing the tool!)

>I'm guessing I should match up 0,0 (x,y) in my drawing with
>a matching 0,0 position for the mill.<snip>

Yes. And treat z as described above.

<snip> or is there a G code I can send to set the diameter
of the cutting tool? Will EMC move the tool exactly on the coordinates
in my NC file (implying that I need to generate NC with a tool
diameter offset), or can I tell it the installed tool and have it
account for it. (I'm guessing that I need to give it the exact path
the tools should travel, and I (or my NC software) needs to account
for the tool travel.)

Any control with G40,41,42 properly implemented will account for tool
diameter when cutting on the XY plane. G43/49 is typical for tool
length compensation.

Again, you are asking a question which is handled one of two ways:

1.Program part OUTLINE, and use the control cutter compensation
features to account for tool diameter/length.

or...

2.Program TOOL CENTERLINE, and let the control use its compensation
features(if available) to account for variations between "programmed"
tool diameter/length, and "actual" tool dia./ length.

>Each time I do a run, would I "locate" 0,0,0 for the mill, or can I
>use home switches (are magnetic switches accurate enough, do I need
>to use IR?).

Only YOUR part requirements and the accuracy/ repeatability of your
machine can answer this!

Expensive magnetic sensors are used in the "big boys", usually
combined with an encoder "index" pulse. (Again, see past posts on
this list). There are a LOT of ways to sense "home".

Hope this helps.

Ballendo