Surface finish 6061 Al

[DavidB]

I have a job in 6061 AL that I did on my Makino.

I know this machine is accurate I can hold 0.008mm on diameter in 15-5ph S.S.

 

My question is when I machine a round cicrle in 6061 AL I'm getting facets on the part.

The code is 1 360 degree Arc so it's not the G-code.The feed rates are quicker for Al than the S.S. but not radical.

I used new Garr unimills with 45 degree helix.

Is this material none for this?

Any ideas?

[HevyMetl]

Do you have M250 G5 P10000 (SGI HIGH ACCURACY) active? That would be my first question. I haven't noticed it on the copper electrodes I have cut in my Makino. But I have not cut aluminum in this machine. I know alot of help I am.

[Guest]

On our Mori's I machine very fussy and some not so fussy round holes in 6061 all the time without issue.

 

The one 360° actually might be the issue. Are you doing that using an R code. We found we got much better cicular motion relying in IJK instead of R and have not ahad a problem since.

[Chris Rizzo]

what kind of facets? code or machine related facets like a linerized spline or bumps at direction changes (quadrants), or tool-related facets like chatter and ripples?

[DavidB]

The code is a 360 arc using I and J.

Machine has G05 P10000 (SGI).

I would not think this would make a differance for a 2D contour using 1 line of gcode.

[Gary]

What speed and feed you running. You could always trade me for are haas it does nice on alum.

[crazy^millman]

How old of a machine David?

When is the last time a ball bar test was done?

Does the machine have some type of dynamic compesation parameters to control axis moves?

Have you tired breaking up the arc into 1/2 arcs or even 1/4 arcs? I have seen this make a difference on some machine as to how they handle arcs.

 

HTH

[DavidB]

I did a job before this Al job in 15-5PH S.S and I was holding 0.008mm on diameter with a great surface finish.

I can bet my bottom dollar it's not the machine.

Thats why I was asking more about the material or the selection of cutting tool.

I did this late afternoon Saturday, so Monday I'll check out the fixturing, the more I think it's vibration through fixturing.

I cut it at 18000 RPM and 2500mmmin

 

quote:

---

or tool-related facets like chatter and ripples?

---

[DavidB]

 

[crazy^millman]

Ok well that explains it. It is harmonics in the tool and toolholder I would be willing to bet. I have found for finishing you need ot not be balls to the walls espically with Carbide. Carbide has a tendency to sine curve at certain rpms. I would say try the oppsite of what you are doing now. I would look at like 6000 rpms 500mm/min and see what you get looking at the part look at a 25.4 mm tool for finising to keep your surface speend and help dampen the harmonic effect.

 

HTH

[Fig sign]

+1000 to Ron ~!

[Chris Rizzo]

quote:

---

Carbide has a tendency to sine curve at certain rpms

---

what is carbide sine curving?

 

Your problem looks like a tooling issue for sure. If you ran the same job in s.s. and now your in al I'd say all previous f/s data are void on the new material. Speed and feed over ride buttons are your friends in finding the sweet spots with the different material. What kind of cutter? I prefer 3 fluters for al finishing. The odd-number of flutes reduces the chatter/wavyness that 2 or 4 fluters will give you.

 

hth

[Tom Szelag]

I can't imagine why 3 flutes would reduce chatter relative to 2 or 4. The odd number shouldn't do anything, its all about the frequency of tooth strikes relative to the natural frequency of your toolholder, which is as much a function of what RPM youre running as number of teeth, unless theyre offset and not equally spaced. Think Z-carbs have that. Slick idea.

 

That said, the sine-waving I think is describing a tool's natural frequency and how it can vibrate and the right frequency relative to how fast youre traveling to make a wavy surface finish. Tungsten carbide, being 3 times as stiff and twice as dense as steel, I'd think would have a tendency to have natural resonant frequencies much higher than your regular HSS cutter. Thus, easier to vibrate at high frequencies, albeit the amplitude is smaller.

 

But hell. What do I know.

[Kevangel]

sometimes using a "too large dia. cutter" can also contribute to chatter because of larger surface contact area. Also all of above, RPM (too high and need more ridgid fixturing)

[Quickmike]

Just a thought but I wonder if it is the natural resonant frequencies of the part maybe along with the cutter or just the part itself. I think the smaller cutter diameter idea is good as well to help reduce cutting pressure.

[88Matt]

we cut 6061 every which way to sunday here and hold fery tight tolerences in most cases with good surface finishes. I personally love cutting it. Try a 3 fluted high helix cutter for Al, not steel. Cuts like butter!

 

I haven't tried them yet, but i read about some variable helix endmills in MMS that were designed specifically for reducing difficult harmonic and vibration problems. They may be worth a try.

 

FYI: Actually the number of flutes does make a difference for many reasons.

 

Matt

[Tom Szelag]

What are the reasons? Goin with a 3 flute cutter I'd imagine you'd have a larger 'core' diameter for an overall more rigid cutter. But by the same token, going to 4 would be even more rigid, so by that token 3 should not inherently have an advantage over 2 or 4, as someone earlier was talking about. Over 2, yes.

[Hardmill]

Its not about a 4flt being more rigid, its geometry

isnt correct for alum. (not enough relief)

Use the 3 flt, the third flt will keep the tool engaged

and cut down vibration.

 

 

PEACE

[Chris Rizzo]

quote:

---

I can't imagine why 3 flutes would reduce chatter relative to 2 or 4.

---

They do. I'd rather spend money on a pet rock than a 2 or 4 flute cutter for AL. There is no comparison around here. Give me your address and I'd be happy to send you some old 3 fluters you can play around with ...

 

Here is a great article from Mondern Machine Shop about asymetrical cutters.

[crazy^millman]

I been busy but I have to agree on all the above points about a 3 flute. Sine curving as I call is natural in almost all round object. I got a good lesson on this from neculear engineers and turbine shaft. as you get a round part rotating it creates a sine curve in the part. using the weight, rpms, and length there is a formula that can tell you how much movement a part is going to have. Now granted these were 140 ton turbine shafts but He explained to me that ever rotating part has some type of this going on. We did all the math and needed .029 clearence for packing that went around the different sections of the turbine. I have seen carbide endmill running at 10,000 rpms bend 10 to 20 degrees and never break rubbing against a wall so my point is all material is flexabile when conditions are right and if it is the it can move and cuase problems. Just my 2 cents worth.

[john_070]

more of an illusion then any thing might try heavier finish cut more chip load.

[35K chipper]

is the tool in a collet or a concentric tool holder? is the tool running true? is it a balanced tool holder? use a 3 flt. destiny viper (stealth )!!!

 

hope this helps.

 

35k chipper

[MetalMarvels]

I am with Chris and hardmill. The Niagara 3-flute 45 degree helix for aluminum mills are fabulous for producing nice finishes at relatively high feed rates - not unlike the Destiny units. I won't go back to a 2 flute at this point.

[Roger Peterson]

I don't know exactly why, and I don't care, but 3 flute cutters (in general) will give you a much better surface finish. Expecially if you are "profiling" with the side of the cutter. You can get good finishes with 2 and 4 flute endmills but you will need to play with your feeds and speeds as well as take a "larger" finish pass. In the end a 3 flute is much less goofing around for a superior finish. If you are doing surface toolpaths with a ball endmill there are a variety of things you can/should do that go beyond cutter selection. Increase your finish pass stepover, make sure you are not cutting with the very tip of the tool (tilt your part or use a bull nose). Something as simple as bolting a steel bar to your block can change the harmonics enough to drastically change the finish. Instead of clamping in a vise, bolt to a thick steel block, etc... One last thing, heat shrink tool holders aren't just for hard milling...

 

 

HTH

[?Mark]

off topic:

MetalMarvels, where have you been?

Over a year since your last post...

Welcome back