Re: [CAD_CAM_EDM_DRO] Re: Need G Code help

Ed, I don't know if you ever got the help you were after, but, I'll see if
I can chime in here. First, it appears you're making the outline for a 2.5"
x 2.5" pocket, with 0.75" R corners. Assuming the first line is going to be
a goto a starting position, say, N010 G0 X0 Y0 Z1 (assuming you want 1" of
clearance from the workpiece), the next line should include N020 M06 T01.
Then, set your cutter rotation & speed for the 1/2" e.m.; N030 M03 S800
(maybe 1800 for Aluminum). Next, a rapid to the pilot hole; assuming your
G0 is modal, you'll say, N040 X10 Y2. So, now you're centered over the
hole, 1" off the part, so you need to rapid down to a clearance plane, say,
N050 Z0.1. Now, I'd NEVER rapid into a pilot hole, so the next line would
be N060 G01 Z-.75 F6 (or whatever depth & feed you need, I allow a
chip-load of less than .002 per tooth on a 4-flute e.m. [I have 3KW spindle
power]).The next line should include the offset; N070 G41 T1 D1 (assuming
you'd entered the tool dia/rad & length offset parameters beforehand).
Assuming your F & G01 is modal, your next line would normally be N080 X8.9
Y3.25, but it shouldn't be! Since the offset takes place over the entire
first linear move after it's invoked, it's wanting to end up with the
tool-center at X8.7965 Y2.9892, (Your tool is being offset 1/4" to the
left, perpendicular, and with-respect-to the theoretical tool path, but, it
must *begin* it's radius at the tool-center co-ordinates of X8.65 Y3, and
your system is bound to 'fault-out', or wander around in la-la land). The
rest of the corners are okay, because the radius starts at the correct
tool-center. This is why I ALWAYS invoke my lead-in offset cut away from
corners, especially radius-ed corners. The best way is to generate your
lead-in in an orthagonal (pure X or Y) move, (that way you'll *know* where
the tool center will be) then lead-in to the workpiece with a tangent arc,
or shallow angle (it won't take you a millisecond or so more time). I
actually did a layout dwg in CAD of each successive move, and it verifies
what I suspected. Hope this helps somewhat.

RayHex
----------

> From: EdFanta <atex57@...>
>
> Ok Guys, I'm completely lost. I will ask if someone can write a bit of
> code to get me started. The pocket in question has been programmed and
> works EXCEPT for the first corner. If I put a negative radius for the
> first R word it gives a funny loopy corner, comes back to the end point
> of the radius and completes the rest of the pocket just fine. I am
> starting from x0y0to a pre drilled hole at x10y2, the z goes down and
> mills to x8.9y3.25 then a .75 radius to x8.15y2.5, a straight cut to
> x8.15y1.5 then a .75 radius to x8.9y.75 then simular to the other two
> corners to return to x8.9y3.25 All co ordinants are to the outside of
> the pocket.I am using a 1/2 endmill which is called out as T1 in the
> tool file, am using G3 and G41 to climb mill in the corners. If some
> helpful soul can write a little code to get the first corner done and I
> can see my mistakes I would be grateful. After it is all figured out I
> can post with the postmortem. Ain't lernin fun??? Thanks. Ed.