HSS vs. Ti

[65535]

Can HSS work on Titanium or is carbide required. Workpieces are .375" 6Al4V titanium bar stock. Also are cobalt steel drill bits the way to go?

 

[G1K]

I've tried HSS on Ti it was with a mini lathe from HF, and the ti laughed at the cutter, but I'm not sure if it was the cutter or the lathe. I've used a hss 1/8" end mill on Ti with out issue, but the end mill didn't last as long as a solid carbbide one.

Ryan

 

[Anglepoise]

Yes...HSS works fine on Ti as long as you don't push it too hard.
However cobalt drills are the way to go in coring out a hole.

The trick with Ti is very sharp tools, go slow ( heat ) and keep the feed on.

Now of course if you have a $50,000 turning center you will be using Carbide inserts, but for hobby use, HSS is fine.

 

[precisionworks]

HSS, both end mills & twist drills, is capable of working in tougher materials IF you go slow on SFPM, feed as hard as the machine will take, and use heavy flood coolant. I've drilled quite a few holes in Ti64, and a zillion holes in AR400 ... they are surprisingly similar in machining characteristics.

AR400 (Abrasion Resistant) plate is just a little more diffucult than Ti64 in machinability, but the settings for AR400 work well for Ti64. AR400 runs 400 Brinell hardness, with 200 Ksi tensile strength. Ti64 runs 389 Brinell, with 180 Ksi tensile.

AR400 is often drilled with HSS twist drills, but the speed is glacial compared to drilling more easily machined materials - 25 SFPM is screaming fast, which means a 1" diameter drill turning 95 rpm. With heavy flood and using a peck cycle. No surprise then that the parameters for Ti64 drilling are 20-25 SFPM, heavy flood, peck cycle. So it can be done, takes forever, and the drill bit will need frequent resharpening.

Most every drill manufacturer recommends carbide drills for hardness exceeding 275 Brinell. Carbide drills can be either solid carbide (which looks like an ordinary drill but with a coolant-through hole), or inserted carbide indexables:

Some indexable drills, like the Iscar DR shown above, can be used in the lathe to first drill a starter hole, then shifted off center & used as a boring tool. The biggest advantage of carbide drills is that they run at 2x or 3x the speed of HSS. The indexable drill adds the ability to change the insert & keep on drilling.

Most everything above applies to end mills as well. Solid carbide end mills have a real advantage over HSS because of reduced flex, which means less chatter & a better surface finish - plus a longer time between sharpenings. Indexable end mills are also attractive for short reach milling, but cannot be extended as far as the solid carbide tool.

 

[Anglepoise]

Can HSS work on Titanium or is carbide required. Workpieces are .375" 6Al4V titanium bar stock. Also are cobalt steel drill bits the way to go?

.....and I forgot to mention 'Anchorlube' as a great coolant,lube for
drilling Ti. For those of us that do not have or use flood coolant this is a great product, and can be applied with a squirt bottle or brush.

and their websitehttp://www.anchorlube.com/lube/

 

[precisionworks]

David,

There was some comment on G-771 on Practical Machinist, December '08. Sounds like some great stuff. Where do you buy it (McMaster shows Anchorlube but doesn't state G-771, Fastenal only carries 8 oz bottles).

 

[Anglepoise]

David,

There was some comment on G-771 on Practical Machinist, December '08. Sounds like some great stuff. Where do you buy it (McMaster shows Anchorlube but doesn't state G-771, Fastenal only carries 8 oz bottles).

I buy it from a Canadian tool supply house in Vancouver, Canada called
"Thomas Skinner". I just buy the small squeeze bottles that last me a long time ( hobbiest ) but would guess you could get it direct

http://www.anchorlube.com/lube/

 

[65535]

Thanks for the info guys. I'm planning a couple of trit pendants out of some bar stock I purchased on ebay. The operations will be done on a Taig Micro Lathe II using collets and indexable carbide tools. I will be boring out the bar to fit the tritium tubes then either drilling or milling holes or slots like Barts pendants. I would assume for such small quick work I could get away with simple mineral oil for lube rather than using a flood or expensive stuff due to the low quantity.

 

[precisionworks]

If you've ever tried Type 316L stainless, Ti64 is similar. Slow SFPM, lots of lubrication, as much feed as the tool & machine will tolerate. Use a peck drilling cycle to keep chips cleared out of the hole, and never let the drill dwell in one place - it needs to be either feeding or withdrawing.

Piece of cake:crackup:

 

[65535]

The machine's not running yet. Still need a chuck motor tail stock and tooling (hopefully I can grab a mini Phase 2 style tool holders hehe) Luckily since there are no threading operations possible on this lathe I won't spend too much on tooling. 3/8" carbide insert toolholders should be about it.

 

[Anglepoise]

The operations will be done on a Taig Micro Lathe II using collets and indexable carbide tools. I will be boring out the bar to fit the tritium tubes then either drilling or milling holes or slots .............

65535,
Now I know the lathe you will be using, I would like to modify my previous reply to you.

The problem you will run into is irrespective of HSS or Carbide.
Due to the lack of power, you will have to take very small cuts ( DOC ).
Nothing wrong with that, but Ti work hardens so your tools must be sharper than sharp.
Now unless you can get ground, hi positive inserts, I think you will be better off with HSS. Any negative insert will just stall the motor.

During this process, if you work harden an area, then you might get belt slippage or motor stall as the cutting tool tries to bite into the now hardened workpiece.

You will just have to give it a try and see how it goes.

 

[65535]

http://littlemachineshop.com/products/product_view.php?ProductID=1680&category=-1550042347

or

http://littlemachineshop.com/products/product_view.php?ProductID=3417&category=-1550042347

I honestly can't find the difference between those inserts. The one doesn't list corner radius but otherwise they seem identical.

Those would be what I would logically use. (right?)

It sounds to me like I should crank the speed (7000rpm limit IIRC) and shave the Ti rather than try to cut it.

What worries me the most is when I try to make the holes in the side for visibility that it's going to be a royal pain.

I plan on buying the milling vice which bolts onto the cross slide and allows vertical moving and clamping so I would be able to use a collet and endmill or drillbit to machine the piece. I'm hoping once I get the piece turned to what I want I can mill flats on 4 sides and then drill a few holes.(or use a small endmill and make slots instead)

Any suggestions?

 

[Anglepoise]

Both the inserts you link to have 'C' as the second letter in their description.
This means that the FRONT clearance is 7° , but this sadly says nothing about the TOP RAKE which I suspect is neutral AT THE ACTUAL CUTTING EDGE.
It is the Top Rake that defines if the cutting tool or insert is positive or negative.
Now cutting aluminum, one can get away with murder, but Ti is not going to cut you any slack. Also both those inserts are pressed carbide as opposed to ground. Pressing will NOT give you a sharp edge.

Also any carbide insert will possibly chip in any setup that is not rigid.
I still maintain HSS is the way to go. You can sharpen it to give at least 10° top rake and it can be given an edge way sharper that pressed carbide inserts.



I would search out the help and guidance of someone that has a similar machine.

 

[65535]

My issue is I don't own a grinder outside of an angle grinder and dremel. If I hand honed those inserts (diamond lapping on a 1200mesh plate?) to have a good positive cutting rake be good? I'll try out some HSS just gotta get me some grinding stuffs for the dremel.

 

[KowShak]

http://littlemachineshop.com/products/product_view.php?ProductID=1680&category=-1550042347

or

http://littlemachineshop.com/products/product_view.php?ProductID=3417&category=-1550042347

I honestly can't find the difference between those inserts. The one doesn't list corner radius but otherwise they seem identical.

There are a couple of differences between those two inserts...

Their ANSI codes are...

TCMM-221 and TCMT-21.52

The first insert ends in 'M' where as the second ends in 'T', they're both a single sided insert, with a hole in the middle and a chipbreaker but the hole in the 'T' designated insert has a countersink that the 'M' doesn't have.

The the three numbers following each insert code designate size, the first number is the "inscribed circle" i.e. insert size, second number is thickness and third number is corner radius. The "inscribed circle" size is the diameter of a circle that would fit inside the outline of the insert.

Looking at the two numeric codes you can see that the two inserts are not the same thickness (2 x 1/16" vs 1.5 x 1/16") and they have different corner radii (1 x 1/64" vs 2 x 1/64").

This page has a guide to insert ANSI codes.

Both the inserts you link to have 'C' as the second letter in their description.
This means that the FRONT clearance is 7° , but this sadly says nothing about the TOP RAKE which I suspect is neutral AT THE ACTUAL CUTTING EDGE.

I wasn't sure whether you were right about that, so I checked the Sandvik catalog for their toolholders suitable for inserts with the same clearance as those two. You are right, they specify rake angle as 0 degrees with a flat topped insert, which is what those inserts are.

You could raise the tool above centre to get positive rake, the inserts have clearance to do a certain amount of that, but I'm not sure how successful it would be.

 

[gadget_lover]

Whether you need the counter-sink depends on your tool holder.

If you need a sharp tipped (but short lived ) tool, use one that ends in a 0, as in TCMT220 or TCMT21.50

By short life, I mean relatively short. It will dull and need to be sharpened or replaced quicker than one with a bigger radius. I can't say how many surface feet of cutting is expected from a modern coated carbide tool. I do know that I use mine much longer than one should. :)

I've honed tools using a little diamond wheel in a dremel. It works OK. Not optimal, but OK. It's not hard to do either.

Daniel

 

[precisionworks]

I can't say how many surface feet of cutting is expected from a modern coated carbide tool.

The minimum running minutes, which you'll see when running maximum DOC, maximum SFPM, maximum IPR (which usually means a high horsepower machining center) is 20-25 minutes. If you are running a high hp spindle with CNC controls & manual tool change, double that to 40-50 minutes. High hp plus manual controls will get somewhere over an hour.

Low hp, small DOC, easy IPR, etc., and they'll last for many hours:D

 

[wquiles]

Man, this is a very informative thread ;)

Will
(fly in the wall - listening and learning ...)

 

[precisionworks]

sounds to me like I should crank the speed ... and shave the Ti rather than try to cut it.

Set the spindle so the speed is 20-25 sfpm, which depends on part diameter.

 

[mcmc]

I don't even know what they're talking about but I feel smarter just reading it =) plus it sounds cool.