EDM for a Taig?

[teilhardo]

Hi everyone,
I have been having a real good time in the last 5 months with my CNC Taig mill but I have run into several problems cutting metal. I am currently working on an aluminum diffuser for a turbine that is about 1" thick (See:
http://www.teilhardo.com/Projects/microturbine.html
for more info)
Anyways, I am real new to all this CAD/CAM/CNC stuff but so far the diffuser has been relatively difficult to machine. Because I am cutting it out of square stock, and I don't have any fancy-shmancy CAM software, I have to cut each pass at .04" (I have to create separtate g-codes for the vanes and the circles). machining was going well until I started to get below .5". The accuracy of the taig started to suffer and the top of the flute (on the long endmill) started to hit the top of the work, causing a large area to cut and eventually breaking the endmill or stalling the steppers.
The real problem comes next though. The diffuser has a similiar shape to the "Nozzle Guide vane", the difference is in the material. The NGV is subjected to the heat of combustion and needs to be made out of 316 Stainless to survive even the first couple of firings. Now, if the diffuser can barely be machined, how is the NGV even within the scope of reality?
So I was just wondering, would it be feasible to make some EDM setup to do? What about ElectroChemical machining, does anybody know a thing or two about that?
I would appreciate any help/advice/comments

Thanks a lot,
Tei

Similar Threads:

• Taig 3 Jaw Chuck on Taig Mill?
• Taig or X2?
• About to get a new Taig, need help!
• Soon, i will buy a taig!
• X2 VS Taig

[Klox]

Hi! Tei,
I took a peek at the link in your post. Do you mean to edm the vanes?
I have read somewhere about a spark erosion "kit" that can be set up on a conventional mill.....I haven't met someone using such a device but i know it could possibly work for you.
I don't know anything about electro chemical machining, LOL!
If you needed something wire edm you can send me a PM, the only obstacle is that i'm down under in Africa.

Klox

[teilhardo]

I am pretty ignorant when it comes to the workings of the EDM. All I know is what a 30 year old machining book said in one paragraph. What caught my eye was that it didn't use any physical contact (which is a plus when you are using a small machine to cut stainless steel). What I was wondering is if the whole thing could be cut using EDM. I suppose that I could cut out a cylinder that is the heighth of the diffuser and then just edm the vanes to their proper depth but I think the real problem is that I don't know understand the constraints of the edm. How deep can it "cut"?
Thanks,
Tei

[TAB]

teilhardo,

I know a thing or two about EDM and jet engine (commercial and military hardware).

First EDM is a noncontact process. ECM is used to produce very accurate but small parts. ECM is a process mostly used in semiconductor or siimilar industries as I understand.

Ram EDM units can be retrofitted to brideport frames. Also hardinge bench top units can be bought for cheap.

As for the stainless, I would suggest that you use a 15-5 or 17-4 PH at a minimum. This is available but will be very miserable to machine. I don't know what type of mill you have but if it is a commercially available millling unit it should be rigid enough to mill stainless if you use carbide and go slow.

The only caution I have about an older EDM unit would be premature failure of the features due to thermal corrosion.

An alternate option may be to make the components out of aluminum and send them to seltzer metco and have them thermally sprayed to protect against attack. This is used in gas turbine applications to protect the base metal in real high temperature locations of the engine. I don't know what it will cost.

Back to the EDM. EDM can cut up to 12" deep if you need. The only drawback is speed and cost. Also you need to produce electrodes and if form is an issue, it may take 10 electrodes to produce a square 5"x5"x12" deep. also this could take days.

Most of the flow features you are inquiring about are formed using 5 or 6 axis machines.

Cool project.

Good luck.

[HuFlungDung]

teilhardo

One trick you could use would be to undercut the flutes of your tool to give it clearance so that the whole depth is not engaged.

If your cuts are only .04 deep, then that is really the entire useful length of your tool flute anyways.

Or, you could carefully create some offsets at each new Z level, that would give more clearance to the tool, in effect cutting a tapered wall. The amount could be only .0005 per level or so, I suppose.

Also, make sure to go around at least twice at each Z level, to ensure that all the material has been removed that is supposed to be removed, but because the cutter deflected, it left a bit. This would eliminate the tendency of the tool to "bite in" anywhere.

Climb mill also, to keep the tool from wanting to pull into the workpiece.

Use a tool radius that is smaller than any internal corner radius of your part. You want the tool to never nest perfectly in any corner, rather, you want it to interpolate the corner by swinging through a small arc.

[teilhardo]

Hi,
Again, thanks a lot for all the helpful posts. My mill is not to fancy. It is a taig desktop mill that runs stepper motors (not servos) and I can usually get a maximum of 16ipm. From what I hear, this is not nearly fast enough to do anything worthwhile EDM wise.
Tab,
Do you have any more info on that temperature coating process? Sounds real interesting
HuFlung,
What do you mean by creating some offsets at each z-wall. I have only been machining for ~6months and the terminology is just a little bit new to me. What is "climb mill"? Can that be done with a simple CAM program?
Thanks a lot for all the generous help,
Tei

[TAB]

This is the company I was talking about

http://www.sulzermetco.com/eprise/Su...Sites/main.htm

additionally here is the address for the listing of all the materials available and their properties

http://www.sulzermetco.com/eprise/Su.../overview.html

Hope this helps.

[TAB]

I don't want to impose but I will try to clarify HuFlungDung's comments about offset and climb milling. Climb milling is where the cutter rotation evacuates the cups opposite the direction of the cut. If you imagine a rack and pinion gear, the way the gear moves in relation to the rack is how the cutter would move in relation to the workpiece. FYI if the direction of the cut were the other way it woul dbe called conventional milling.


As for the offset if you were to imagine cutting a square 1"x1"x1" deep and taking cuts at .100" deep z moves and offsetting the cutter by .001" each pass as you moved down it woul dbe as follows. This examle assumes you are cutting a pocket where Z0.0 is the top, X0.0 and Y0.0 are the pocket center.

1st pass cut Z-.1 X-.5 Y-.5
cut Z-.1 X.5 Y-.5
cut Z-.1 X.5 Y.5
cut Z-.1 X-.5 Y.5
cut Z-.1 X-.5 Y-.5

2nd pass cut Z-.2 X-.499 Y-.499
cut Z-.1 X.499 Y-.499
cut Z-.1 X.499 Y.499
cut Z-.1 X-.499 Y.499
cut Z-.1 X-.499 Y-.499

3rd same as 2nd but Z-.3 and X-.498 Y-.498
Etc.

The wall would look like a stair case which moves the cuter away from the wall reducing vibration and creating clearance.

[HuFlungDung]

In case Tab's explanation of climb milling is not clear, in layman's terms, climb milling is like sawing from the side of your table saw that says "Do not rip from this end"

I think of climb milling as this: when taking a cut at only half the width of the tool, the tool edge enters the work at maximum chip thickness and leaves the work at minimum chip thickness.

There are only two ways to mill: climb or conventional. If you have ever used a manual mill, you can feel the cutter "assisting you" when you climb mill, because it wants to pull the work into the cutter. If things aren't tight and the screws at minimum backlash, it will indeed "climb" onto your work or fixture and and make a real mess of things

Most machines with high backlash cannot climb mill successfully if cutting heavily.

During conventional mill, the cutter wants to push away the work, and it takes extra feed power to force the work into the cutter.

During all these cutting motions, your endmill does deflect from the forces of the cut. In climb mill, the cutter tends to deflect away from the work, which means it leaves a little surplus to finish. During conventional milling, the cutter tends to deflect into the wall created by your previous passes. This causes the somewhat "predicatably unpredictable" behaviour of gouging the wall at the most inopportune moments, just when things get dicey near the finish

[teilhardo]

Ok, i think that I finally understand the concept. Now my next question is:

How do I do that to make my diffuser

http://www.teilhardo.com/Pics%20Dec....1-18%20005.jpg

with a cheap CAM program and without having to change the 1500 lines of G-code?

If you go here:

http://www.teilhardo.com/Projects/Cn...January04.html

and you look at the 3rd picture from the top, you'll see what the endmill does. At the very top, left hand corner and bottom left hand corner of the diffuser, you'll see the dark areas that the endmill took a bite out of... I can only wait until I have to cut out a piece similiar with stainless steel

Thanks for all the help,
Tei

[HuFlungDung]

Steps to take:

Step 1, you find a girl you love....no, no, that's something else

Step1, make sure your "cheap cam toolpath" is taking your tool around the part in the climb milling attitude.

Step 2, make 2 passes at each level (or more) to make sure the cutter has removed all the material it was supposed to.

Step 3, if the tool wants to hog in when it enters a corner where the tool tends to dwell as it changes direction, this is the dreaded nested corner I wrote about. Solution: use a smaller diameter cutter, or increase the radius of the corner so it is slightly larger than your chosen cutter radius.

Step 4, if you still have trouble, then grind away the flutes (undercut, we call it) behind the first .1" of the cutter, to create clearance for the total length of the cutter when it is at full depth. In essence, you will be creating a T shaped cutter out of your endmill. It might not be pretty, but it will definitely clear after that.

[Klox]

[QUOTE]Originally posted by HuFlungDung
[B]Steps to take:

Step 1, you find a girl you love....no, no, that's something else

Hu, thanks you have just brigthen up my day LOL!!

Klox

[TAB]

Did you think about an extended endmill to get down further? Are you making a mold to cast the part in or is that the final part?

I looked in MSC to see about longer LOC (length of cut) endmills they have a 1/4" single end end mill with a 1.25 LOC which looks like it would be better than what you have in the pics you posted.

[teilhardo]

I have several of those long endmills. The problem is that the CAM software doesn't compensate very well for it, the spindle is not very powerful and the endmill usually takes generous bites and in the process digs itself into the work.

Tab,
You've worked with jet engines before, what ways do they use to make axial turbine blades, diffusers and combustion chambers?
I would appreciate it if you could educate me a little bit in that type of manufacturing. It is very interesting to me

Thanks,
Tei

I wish that I new how to cast... That would sure make the job much simpler

[teilhardo]

By the way,
What is EDM used to make that High Speed machining can't do?