6AL4V help needed - Shallow 3D milling & chip welding

Gentlemen. Haas VF-2ss. I'm working on some 6AL4V parts that have very shallow (about 12º max from horizontal) and I'm getting welded chips in the finish pass. The finish itself is great aside from the welded chips. Not torn at all. I made the exact same parts out of a nasty batch of 304 with zero issues earlier today, same setup, same tooling, etc. Coolant is in excellent shape and at 8% (1% over nominal). Runout is less than .0003".

Everything else about the parts is working great. Finishes and sizes are perfect, it's just this shallow surface that is having issues.

Roughing with a 3/8" 5 flute endmill leaving .005" (as programmed), semi finish with identical tool as the finisher (1/8" 4 flute AlTiN coated Imco ball nose.) leaving .002". .028" stepover for both 1/8" ball nose tools. Parts are highly cosmetic and the customer requested this stepover to get a pattern. All the welded chips look to be on the conventional milling side, which of course makes perfect sense.

I'm at 12,000 RPM, which should be 97 SFM at my calculated effective tip diameter of .031". 50 IPM. I tried 6,000 RPM and 25 IPM for shits, and really nothing changed, which was surprising.

Two brand new tools made no change.

Any thoughts?

Here's one at 171x:


And a normal picture:

My first thought is to try a ZrN coated aluminum-specific 3fl stub for the finish cuts, the idea being the higher shear fluting may cut more cleanly, and with just a light chip load may give you adequate life. This is just a gut feeling (haven't tried it myself), and may be the large dinner I just had fogging my brain.

Edit: With most three flutes only one is cut to center, so use a two flute instead to have two working edges near the center.

Also, that's pretty wide/deep for a finishing cut, basically a trough. If you need that per customer request, only leave a couple thou for the cut, more and perhaps you're loading the tool too much.

Milland said:

Also, that's pretty wide/deep for a finishing cut, basically a trough. If you need that per customer request, only leave a couple thou for the cut, more and perhaps you're loading the tool too much.

Click to expand...

It's indeed needed for the design. The semi finish tool is leaving .002". First trial for the morning will be re running the finish tool and see what that does.

Milland, thanks for the help. I had some uncoated 2 flute ball nose tools on hand and just swapped that in. Major improvement, no welded chips to speak of but it was still torn looking on the conventional cut side. The final step to get a good finish was to skip the semi finish tool altogether and take a heavier bite at a reduced feedrate. Perty.

Now the question is tool life. My tool salesman is grabbing what they have in stock so if we need more in a hurry, he'll have them in his truck already. Gotta appreciate that.

Torn surface finish is common when conventionaly milling with a ballnose.

Try to switch to climb, if possible.

zero_divide said:

Torn surface finish is common when conventionaly milling with a ballnose.

Try to switch to climb, if possible.

Click to expand...

Yeah, I had previously started writing that he should try two passes per trough with a small offset to maintain climb milling on each side, but decided the programming and extra time would be prohibitive. Glad Matt found that the deeper pass with slower feed works well.

Just to wrap this up, the new 2 flute uncoated tools were good for 6 parts, which is 656 linear inches of cut total. Ehh. Failure mode was not welded chips like before, but a slightly torn surface. The tools are still fine for just about anything else.

What happens if you cut it to finish depth with a 2-flute and then cut it again at the same depth with a fresh cutter?

Matt@RFR said:

Just to wrap this up, the new 2 flute uncoated tools were good for 6 parts, which is 656 linear inches of cut total. Ehh. Failure mode was not welded chips like before, but a slightly torn surface. The tools are still fine for just about anything else.

Click to expand...

If you get some coated stubs in I'll be interested if you see a longer effective life.

12,000 RPMs and your wondering why its melting? seriously? I think you know the answer to that.....DOH

charlie gary said:

What happens if you cut it to finish depth with a 2-flute and then cut it again at the same depth with a fresh cutter?

Click to expand...

That job is done now, and probably won't ever repeat. The uncoated 2 flute did well on its own without a finish pass.

The testing I did with the original 4 flute tools, though, showed that a 'spring pass' did wipe the welded chips off, but at the same time made a torn surface. I'm still pretty new to Titanium, but it doesn't seem to like spring passes very much. Gotta take a bite.

Johnny Larue said:

12,000 RPMs and your wondering why its melting? seriously? I think you know the answer to that.....DOH

Click to expand...

Oh boy... It wasn't melting, it was welding chips... two completely different things. And with a .002" DOC and .028" stepover, that results in an effective diameter of .031". At 12,000 RPM, that is 97 SFM.

Milland said:

If you get some coated stubs in I'll be interested if you see a longer effective life.

Click to expand...

If we get this or another similar job back in, we'll definetely try a coated 2 flute just to see. My bet is that the surface finish will suffer again with the coating. The uncoated tools I was using were just a cheap, double ended SGS, so the tool life isn't really that big a deal compared to the overall cost of these parts.