Need some advice on working with 6AL-4V - already having trouble!

Hi,
Have some .750 round bar, need to make .250 and .3125 holes through it. Have a B-port 1J.

Tried plunge mill w/ solid carbide, 4-flute TiN coated center cutting. Dry.
Failed to keep the pressure on, it rubbed and now the bottom of the hole is too hard to cut, shattered the cutter. And the next one.
Looked at the specs for annealing the piece, I don’t have the equipment to put that much heat on it for the required amount of time.

Considering ordering some Fullerton 3412-Fantom 2.0, carbide, 5 flute FC-20 coated.
Would try to cut through the hard spot - is an option I should try?
Or is there a better end mill for 6AL-4V? ( will strive to improve my technique)

On the rest of the holes, should I stop plunge milling, and try a drilled pilot hole first?
Have some M42 cobalt drills that might work.
Would use some Huber’s Hab-cool 318, a high sulphur cutting oil with the drill bits.
Thanks,
Frank

I've done a fair bit of drilling and some milling of 6Al4V and found going on the low side of sfm and keeping a good steady feed is important. I've cut it both dry and with flood cooling and the cooling is way, way better. Tools heat up quickly and keeping things cool is critical.

Here's a good reference:

https://www.timet.com/assets/local/documents/technicalmanuals/DesignandFabrication.pdf

They talk about drilling on pg. 18 and give geometries/speeds & feeds on pg. 20.

Note for annealed material (probably what you have) they recommend 20 - 50 sfm, that equates to only 244 - 611 rpm for your 5/16" drill.

I tried a bunch of different drills but found Dormer's "R10CO" 135* cobalt split points to be excellent.

http://selector.dormertools.com/web...e-data-sheet.pdf/R10CO?searchaction=Technical

I'd spot with a carbide spotting drill first.

For your hardened hole you might be fooked.

Yes, the best tools for Ti are Highspeed steel run at very low speed and steady, moderate feed. Very sharp tools give a mirror finish with very little effort. If you try to hurry with Ti you will regret it and doubly if you do not feed constantly.

Hi fish123:
Why are you trying to make a hole by plunging an endmill into the solid, especially in titanium?

The problem is that you are loading the cutter way more than it was designed for, and the outcome is that you cannot keep it shearing a chip, the cutter rubs, the bottom of the hole work hardens and now you need more axial force than the cutter can take.

If you cannot interpolate the hole (and on a manual mill you obviously cannot without a rotary table) you MUST get a pilot hole in before you plunge with your cutter.

However, I'm guessing the work hardened zone is not very deep.
If you take a carbide or cobalt HSS spotting drill (use a 118 degree one for its stronger point) and poke it into the hole with a bit of Rapidtap or other magic goo on it, you'll pop right through that hard bit and be able to pre drill the remainder of the hole without effort.

Run your cutting tools SLOW...on a manual mill 80 IPM is more reasonable than 300 IPM.

Make sure you keep some tapping fluid in the hole too, and you'll find titanium not too difficult to machine.
Avoid two processes though: (especially on a manual mill) don't ream and avoid power tapping.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

fish123 said:

Hi,
Have some .750 round bar, need to make .250 and .3125 holes through it. Have a B-port 1J.

Tried plunge mill w/ solid carbide, 4-flute TiN coated center cutting. Dry.
Failed to keep the pressure on, it rubbed and now the bottom of the hole is too hard to cut, shattered the cutter. And the next one.
Looked at the specs for annealing the piece, I don’t have the equipment to put that much heat on it for the required amount of time.

Considering ordering some Fullerton 3412-Fantom 2.0, carbide, 5 flute FC-20 coated.
Would try to cut through the hard spot - is an option I should try?
Or is there a better end mill for 6AL-4V? ( will strive to improve my technique)

On the rest of the holes, should I stop plunge milling, and try a drilled pilot hole first?
Have some M42 cobalt drills that might work.
Would use some Huber’s Hab-cool 318, a high sulphur cutting oil with the drill bits.
Thanks,
Frank

Click to expand...

Jesus man! Don't do that!

Cut off the hardened piece, and throw it where you won't be reminded so often that you done somethin' dumb.

That stuff now has a harder heart than a Granny aged Street hooker. You can get past the hard part, but the cost in time and tools....Usually lots of trips to the drill sharpener, and eventually you manage to punch through the miserable hard layer that otherwise just eats the tools you feed slowly at it...

Use a SHARP drill. Keep the pressure on. Use Coolant. Turn OFF the shop radio, because you REALLY want to hear the very first sign that the drill bit squeaks in the hole, and, when it does, get that drill OUT of the hole as fast as you can, and replace it with a sharp one.

It ain't brain science, it's rocket surgery!

Nothing wrong with the stuff, but you will not get away with being sloppy as far as technique goes. It WILL make you pay!

If you absolutely have to try to save the material, drill from the other side. Expect to lose a bunch of drill bits.

Thanks for al the tips & advice!
I’ll cut off the ruined section of the round bar and try again w/ the suggested methods.

tdmidget said:

Yes, the best tools for Ti are Highspeed steel run at very low speed and steady, moderate feed. Very sharp tools give a mirror finish with very little effort. If you try to hurry with Ti you will regret it and doubly if you do not feed constantly.

Click to expand...

That's really old school.

I had a friend that worked for Curtiss Wright during WWII - B29 engine work and he was telling me that's exactly how they / he figured out how to cut this new fangled material "Titanium" . He claims to be the "guy" that figured out the go "Slow" method (as everyone else was trying to figures out harder and faster). Later he was chief prototype grinder (there) so maybe he had a direct hand on very very sharp tools.

You don't want to hear the magnesium stories lol.

cameraman said:

You don't want to hear the magnesium stories lol.

Click to expand...

I'm burning with curiosity!

I have had good results drilling ti with cobalt HSS drills ground with a multi facet point at 135°

awake said:

I'm burning with curiosity!

Click to expand...

Ti can go up in flames too, just not as easily.

My Ti story. Many moons ago, cutting some 2.5"x4.5" Ti bar at a 45 degree angle, the saw
was a POS, but it could cut at a 45 degree angle, and it was outside one of the bay doors,
running on an extension cord.

15 minute cut on a fresh blade, and it would hold that time as long as the blade didn't
touch anything else. Otherwise it was 45 minutes. So, when people tell you to use NEW
tools on Ti, don't laugh, it makes a huge difference. Ti is just bitchy that way.

Anyways, the swarf rolling out of the saw was so light, and it balled up. A softball piece
of swarf might have weighed a gram. It was so light and thin, it wasn't even sharp, soft as a
ball of cotton.

So I'm sitting here at my desk doing work (, who am I kidding, I was probably reading PM).

And I hear *WOOSH*, not quite an explosion, but as close to it as you get without actually
being an explosion. It sounded like when the guy that takes care of my yard lights a 10 foot high
pile of dry tumble weeds on fire with 3 gallons of gas. Maybe a *BOOF*, but not quite a *BOOM*, but
really close.

I go running, and there is smoldering Ti swarf everywhere, some is in the shop, most outside,
a good 15-20 foot radius from the saw. And of course the saw stopped.. Thank god for circuit
breakers. Apparently something had fallen on the extension cord and exposed the wires, and then
the swarf, and KABOOM!!!.

Nothing like magnesium (that's fun to play with), but Ti goes up to.


My experience with 6-4 Ti. Moderate to low speed, low to medium feed, keep it
consistent. And it takes a LOT of force to cut, its the only material I've
had to choke up on reamers on, otherwise they would bow and cut a funnel, not
a cylinder.

New tools, no matter what, I don't care if you only drilled one hole in aluminum
with that drill. NEW out of the box, SHARP tools.

Really not all that far off of dealing with 304, just need to be a bit more
careful and detail oriented, any mistake or hiccup is going to bite you in the ass. Unlike
304, in my experience at least, its consistent, your #'s that work today will work
tomorrow, they will work next week and next year. 304, you're lucky if your
#'s will work from one end of the bar to the other.

I would advise you to use another type of cobalt drill bits.

ricardos said:

I would advise you to use another type of cobalt drill bits like in this article Who Makes the Best Cobalt Drill Bits? | Webproductradar.

Click to expand...

Very useful for me.

ricardos said:

Very useful for me.

Click to expand...

Fucking spammer doesn't know a file from a drill.