Re: [CAD_CAM_EDM_DRO] Newbie: Two halves of simple die not aligning properly - Long

kaptainkarst wrote:

>I then open Mach2, load the Gcode for the drill (indexing holes) and
>run the program (this is after indicating the workpiece in the vice
>and setting zeros on all three axises). After the 3 holes are
>drilled, it returns to zero, I remove the drill bit and replace with
>an end mill and reset the z axis zero (x and y are still the same).
>
>I then load the second half into the vise and indicate the corner to
>zero just like I did with the first half. I load the "Half B" drill
>gcode, let it run, it returns to zero and I change the drill bit out
>for an end mill and reset the Z axis zero. I then run the mill
>process for half B.
>
>When I put the two halves together, the index holes line up properly
>but the two milled slots are slightly skewed from each other (approx.
>1/8" over 4" of travel).
>
>

Skewed? Do you mean they are parallel, but offset by 1/8"? Or, do you
mean there is an angle between them?

If there is an offset, but they are parallel, you may have tool deflection.
it is not uncommon for a heavily loaded, small diameter end mill to deflect
up to 1/2 its diameter when side milling. You might make the cut
several times
and see if the cutter removes metal each time. If so, the tool is being
deflected by the work, and taking off a little more material each time.
That would indicate your feedrate is too high, or more likely, your length
of cut is too much. Generally, when plowing at full cutter diameter into
work, you step the cutter down 1/2 of cutter diameter each pass, and repeat
until you are at the full slot depth. Then, you make a final pass,
removing a
little bit more material. So, if the cut was along the X axis, you'd
move the
Y axis in by .005 to .020 or so, to clean up the face of the cut.

If the slots are actually at an angle to each other, then you have something
wierd in the DXF to milling step. I never use DXF for this, but use a
CAD?CAM
package that goes directly from the CAD's native drawing info to G-code.
If something is wrong, I can READ the G-code to see where the trouble is.

Also, for work like this, I generally do not use CAD, unless there are arcs
and angles which make the G-code more complex. I have some programs
that write G-code directly from menu entries. See
http://jelinux.pico-systems.com/gcode.html for some of these programs
that you can download. For milling slots, there is the treprect program
(trepan rectangle - it cuts around the edges of the hole all the way
through a panel) or rectpocket (it mills out the entire interior of the
pocket). I use these all the time to make slots. I would select a tool
just a bit smaller than the slot width if I don't need mostly squared-off
corners. If the final allowance is .010" (per side), and the slot is to
be 1/2" wide, then use a tool that is less than .470" diameter. But,
1/4 or 3/8" would work fine. Rectpocket would make one full-diameter
plowing cut down the middle, then go around the sides to within .010"
of the desired slot width, then repeat at greater depth until the full depth
is reached, then finish it to full width.

Jon