PDA

View Full Version : Would like info about machining electrode



jeffrey001
09-25-2010, 11:50 PM
Hi,

Would like to start a small business for machining EDM electrode.

I do not have a lot of experience with EDM machining but I've been a CNC machinist for the last 25 years.

I work with SolidWorks and Mastercam.

I know that SolidWorks have an Add-on for electrode but not a lot of info or tutorial on how to use it.

Is Graphite is complex to machine.

Is there any chart for the spark gap and how to design shape for the electrode.

Thanks for any info, will be appreciated.

Jeff

jeffrey001
09-27-2010, 03:28 AM
Any tutorials on the internet.

Jeff

mc_n_g
09-27-2010, 01:50 PM
Never did it myself but I know you need a sealed machine with vacuum to contain the dust. You also need a very high spindle speed and balanced toolholders. Hurco, Haas and other manufacturers make CNC machines specifically for the graphite market. You will have some hefty investment in equipment and carbide. Graphite tends to be a wearing/abrasive type cut so endmill coatings are desired. Also advise look ahead code reading for the cnc machine.

jeffrey001
09-27-2010, 02:45 PM
Thanks for the comment.

So should stay with copper electrode.

Jeff

mc_n_g
09-27-2010, 03:16 PM
I have no idea.
Money or your health?

gyro_john
10-06-2010, 10:25 PM
Graphite is a piece of cake to machine. Cut it dry. I use 4000 rpm for a lot of things - partly because I don't like to run my spindle much faster than that. Since the graphite is fairly abrasive I like TiAln coated cutters for the long-winded toolpaths. For drills etc, HSS is just fine, but if you had to do a lot of holes, you might have to sharpen the drill occasionally.

Drilling feedrates similar to steel, and maybe 1500 to 2000 rpm. A fountain of dust comes out of the hole. When the hole gets deep you start to peck with cleanouts and the dust doesn't cause a problem.

I wire up the hose from a shop vac right close to the cutter and most of the dust is removed then and there. The rest goes into the coolant tank the next time I use coolant and doesn't cause a problem there either.

I like a stepover of maybe 25% to 50% of cutter width, about a .002" chip per tooth, and depth of cut maybe 25% to 50% of cutter diameter, although since the material is quite forgiving just about anything will get you started.

Where the material is a bit tricky is that it is not very tough or very flexible. A drilled hole breaking through the back side of the part will chip out unless you slow the feed to maybe 25% for breaking through. Similarly the edge of a block may chip a bit if you are conventional milling on the first pass. If it's chipping, you're trying too hard. Take smaller or slower cuts. Try climb milling first. You will be very gratified at the delicate, precise shapes you can make, and fast!

You can make a long skinny pipe with a thin wall (nice for burning out broken taps), or you can make a tall, skinny fin. But you can't make them IN ONE PASS! If you try a big cut, the delicate part will snap off at the base. Make them in many short steps so that the base material supports the part, and when you're done, the part will still be standing there, looking fine.

Barely any heat is generated in machining (unless you use a drill to destruction).

Good surface finish on machined graphite. If you left tool marks, a very light sanding with very fine sandpaper will take them right out.

It's easy to drill coolant passages and plumb your electrode to shoot flushing oil to evacuate the metal as it's burned off.

Graphite electrodes are a bit sensitive to frequency (duty cycle) in the EDM machine. Roughing and semi-finishing frequencies work fine, but as soon as I try to go to the finer surface finishes, it starts to consume the graphite, and a black plume is discharged from the cavity. When the cycle ends I will then see significant electrode wear. When that happens I have to re-cut with another electrode, at the end, to sharpen up the EDM'd cavity.

At least this is how it works for me. YMMV.

Regards,

gyro_john

gyro_john
10-06-2010, 10:41 PM
As for spark gap, two things to report:

1. My first EDM was an antique Elox sinker, and it had a chart showing that the spark gap might be as much as .005" per side.

2. Now I have a Sure First, I think it is, an oriental machine and it's four times as good, and several times as fast to set up. This one, those big spark gaps don't exist. I find if I budget for a gap of .002 - .003" per side, that'll be right in there. A little experimentation will show you.

Another word on graphite electrode consumption: Minimum electrode wear is about in the middle of the frequency range. Lower frequency for bigger craters and fast metal removal eats the electrode quicker, and Higher frequency to get a good finish eats it Real fast.

As for CAM software, anything I can't program by hand or with macros, the CAM software (Visual Mill) works just fine. It's all about intelligent choices of rpm, feedrate, stepover, step down ... Just like any other machining. Start with big cuts with big cutters, re-cut with small cuts using small cutters only where necessary, suddenly hey presto, you've got a part.

Try it. In no time you'll be a Graphite Master (TM) and turning out electrodes like crazy. I actually like graphite better than copper (maybe because I've used it more).

And anudder ting! If the electrode had been cutting just great, then it stops cutting and just starts to bounce up and down and act weird, then I stop, retract, and I'll find a bunch of carbon residue plastered to the bottom of the cavity.

Have at it with a brass bristle wire brush and some EDM fluid, it comes right off, and you go back to cutting. Insufficient flushing (sometimes you can't get the fluid in there to flush good) is the culprit.

jeffrey001
10-06-2010, 11:01 PM
Hey, thanks a lot for your help gyro_john, it is really appreciated.

I have some mold companies in my region and maybe they could be interested to sub contract these king of jobs.

Again, thanks for your precious time.


Jeff

Cmailco
10-12-2010, 09:06 PM
I'd suggest PVD (diamond) coated tooling for graphite. Depending on the brand, you could spend 3-4x as much per cutter... but see 20-30x the tool life, so it's really a no brainer as graphite is quite abrasive.

Run as much rpm as you've got and keep an eye on speeds... mainly due to the fact that many older machines don't have the look-ahead capabilities. Mill a square at 300 inch/minute and what you end up with is 4 flat edges with large sweeping radii leading into each corner, IF you don't have the loo-ahead capabilities and/or lots of slop in the machine.

Good luck,
Chuck

rusty abe
11-02-2010, 12:06 AM
If you want fast removal (ie. large amperage as well as long on time) then I would opt for graphite, but if the model require a very fine finish as well as delicate form then I would go for copper electrode. Since graphite will take a very high current and does not bend as a result of heat from the current, but it's quite fragile and create quite a mess to machine. On the other hand, copper can't stand taking high current but it will give a very fine finish on the workpiece, providing you give a "breathing hole" (ie. drill a hole at the highest point on the electrode) so the dielectric fluid will flow and remove the debris.
From my experience, I mix 4 part of diesel feul to 1 part of kerosine for my dielectric fluid. Kerosine will give a better surface finish, cleaner to use as well as been able to get the debris away from the impression better at the cost of obnoxious fume and lower flashing point. Lastly, do a lot of exprimenting, it is fun to see a soft metal can bite a very hard steel.