[Cartierusm]

OK so I just got a plasma cutter and never did anything but hand cutting until now and need a little guidance.

I'm using the 4th Axis on my CNC mill with a holder for my plasma torch to do some tube coping on some 3/8" Wall 4" Stainless tube. I cover the mill with welding blankets to protect it from the sparks. I'm using an Everlast Power Plasma 50, 50 AMP NON-High Frequency Start Plasma Cutter. The manual is useless and doesn't mention speeds and amps for cutting, I mean it doesn't mention anything to at least give me an idea of where to start. One person told me on an Everlast forum that the stand off should be 1/8" for CNC and my friends who have a CNC plasma run at 20 IPM for 3/8" thick material, but almost everyone else in the plasma world pierces at that height and then cuts at 1/16". So I set my PSI at 60, cut height at 1/16" [didn't need to pierce], 50 amps and 20 IPM on my CNC.

It cut like butter and seemed to come out pretty good. So my questions are I got a ton of splatter slag inside the tube. Is this much, refer to the pictures, or do I have it cutting with too much power (50 amps). What can I do to not have all that splatter slag as the parts are machined ahead of time? I figure I can do two things, spray the inside with MIG splatter shield spray and I could also make a circular aluminum insert that is held stationary while the part rotates in the 4th axis, with a notch in the shield at the top for the plasma to go through but not spray the tube itself?

Also the tube miter came out good but since the plasma cutter is stationary it, obviously, didn't bevel the sides of the tube miter. Think of mitering a tube with a hole saw. The saw goes straight down and cut the right and left side of the tube as it goes down, but when mitering on the 4th axis the cutter remains perpendicular to the workpiece as the workpiece rotataes so the sides don't bevel in. So when setting the tube miter on the corresponding tube is sits proud. I could just grind and hand fit it, but it would be nice to do all one operation and have it come out perfect.

Any help would be appreciated. Thanks.

[307startup]

I told you the welding blanket would work

Simplest solutions are always best...copiously coat the inside with anti-spatter. After a few cuts with an internal sleeve, it will be covered with spatter and be a pain to remove and insert.

You're going to have to mount your torch with the amount of bevel you are seeking. The nose of the torch will be between 30-45* above horizontal for what you want to achieve.

I would suggest some kind of backing plate between your workpiece and the front of your 4th axis chuck, as this bevel cut will blow slag towards it...don't want that crap on the jaw screws!

[Cartierusm]

Thanks for the suggestions. I did use a plate inside to protect the 4th axis chuck. If I manually bevel the torch then the top and bottom of the cope will be angeled as well and if I can help it I'd like to have the part sit on the mating tube will all sides touching so I can braze it on. But maybe the bevel is better all around then having to manually grind it later on.

Question, do you think, from looking at my pictures, that my torch height was good, had enough air pressure, good speed and power were correct? I think I might have used too much power? Thanks.

[307startup]

Unless you have one of those tilting 4th axis rotabs, you're gonna have to manually bevel your torch while it's entering & exiting the cut to only have beveled top & bottoms mouths...

I think your parts look good. Too much air is never enough with plas. The cut edge looks a little dark, but I think it is not a bad setup you were working with.

If you really want the skinny on plasma setups, you need to get ahold of Jim Colt (?) on the Hypertherm forum...that man knows his stuff!

[Cartierusm]

Thanks, again. Now you said the edges look a little dark and I was thinking the same thing, but what is that a symptom of?

[307startup]

The dark edge is a result of oxidation from cutting with air or CO2 as a shield gas.

You can get a better cut (smaller HAZ) with more amps and more speed. You can get a better edge with a different shield gas like nitrogen, H35 (argon/hydrogen 35%), or methane/natural gas.

The alternative shield gases react with the oxygen in the kerf, preventing oxidation.

That being said...you're still going to need to grind the HAZ off down to clean metal if you want to minimize risk of hydrogen embrittlement or weld failure. (As it stands with the dark edge you currently have)

If you switch to a different shield gas you would only need a light dressing using the grinder to be ready to weld.

I'm assuming this is a 300 series stainless, not a 400 series? The same rules apply, but 400 series reacts more like mild steel due to the higher iron content (leading to nitriding of the face of the HAZ).

[307startup]

I just thought of this...

If you leave your workpiece in place on the rotary table and have a 2nd program (modified slightly from the first), you can reset your torch at the angle you want and cut your bevel on the top and bottom lips, turning the torch off as the 4th rotates out of the section of lip that needs beveled, through the straight cut of the saddle, and back on as it enters into the next lip...

It seems only the top and bottom 1/3rd needs beveled to seat properly.

[Cartierusm]

Yes it's 304 stainless. I have welding gases such as straight Argon, Tri Mix and Argon CO2, but I don't mind a little grinding. I think I'm going to weld these from the inside and not braze so I can bevel the whole thing and just use filler metal on the rest. Thanks again.

[Cartierusm]

This morning when I woke up I came up with this idea. Look at the pic. I took the jig I made to hold the Plasma Torch in my Mill Spindle and added a pivot point to the front. So now what I can do is have the Z axis raise and lower to change the angle of the torch to make the bevel cuts automatically as it's cutting the tube cope.

The only mistake I made was that I just added a random pivot point to the front of the jig and then I realized that I had to have the pivot point a little below, but on the same vertical plane as the Plasma Torch Tip. As of now when it pivots the tip of the torch moves to the left an inch or so.

So all I need to do now, once I fix the pivot point, is take the distance from Z0 to 30 degrees, which is what the tube miter angle is, which is 2.6364" and divide that by the number of lines in my Gcode from 0 degrees to 45 degrees and input those numbers as Z coodrinates and it should track.

Does this sound like it should work?

[307startup]

The pivot is brilliant

I'm not sure why you are wanting to take the total Z axis travel of 2.6364" and divide it by the number of lines in your program...

If you want the total Z axis of travel to occur during a 45* revolution, issue a Z axis feed rate per degree...

For 2.6364" in Z over 45*, you would need a feed rate of 0.0585866666666667" per degree...call it 0.05859" or 0.06"

As you want the bevel to then decrease in the next 45* of A axis travel, your feedrate for an opposite Z move would be the same.

You would have -Z axis feed from 0-45*, +Z axis feed from 45-90*, flat and level from 90-180*, -Z axis feed from 180-225*, +Z axis feed from 225-270*, flat and level from 270-360*...

Does this correlate with what you're attempting to do?

[Cartierusm]

Yes, but i realized it's not 45 duh, but 90 degrees x4. I just got done hand coding the whole thing and tested it out and it seems to work perfect.

ALTHOUGH, I'm going to redo the code to make it better and for next time...so how would I write the G-Code like you are talking about to do a feed per degree with the Z axis? Thanks, that would help a lot!!

[307startup]

I don't know how you're writing your code to rotate your 4th axis...

You should be able to do a simultaneous feed movement in Z as your 4th axis rotates. Just like you would do a simultaneous X,Y movement or X,Z movement or Y,Z movement....

[Cartierusm]

Your funny, I'm not writing my 4th axis code RhinoCAM is! Well hand coding is a pain in the ass but it's not too bad. Thanks anyway.

[307startup]

You should be able to tell RhinoCAM to issue a Z feed rate at the appropriate points of rotation...

it's effectively the same thing as engraving on a 4th axis...

neither RhinoCAM, your mill or the controller knows that you don't have a tool in the spindle, or that your effective Z zero is offset from center...

so that leaves you being the only one in the know, and what those things don't know won't hurt them...as long as you don't crash