Best Tool For Roughing Titanium?

[allloutmx]

We have a long standing order for an aircraft part where we remove approximately 75% of the material with (2) 1/2" diameter endmills. Material is 6al4v. Im averaging about 20pcs per tool utilizing dynamic tool paths around the profile.
This job was running when I got here, and the person that started the project is no longer here so Ive been working my way through some of the issues in the process. At this point Ive tried a few different tools and manufacturers but so far, am have the most success with my 5flute reg length and 6 flute stub Titan brand endmills(what an unfortunate brand name). Ive thought about trying to rough the profile with an insert tool but my exploratory toolpaths show a much greater cycle time and even if I use a larger diameter insert tool, ill still need to come back in with the 1/2" tool to clean out the smaller rads.

Curious, who is making the best endmills for milling titanium and in which configuration? mainly looing for tool life improvements.

Currently running about 350ish SFM and .0067chipload. 6% radial DOC on an OKK Horizontal


Thanks In Advance.

 

[just Dave]

I can’t wait to see answers!!!!

 

[implmex]

Hi alloutmx:
I cut a fair amount of Ti6Al4V titanium too, and what I've found after some experimentation is that I cannot beat the MRR of a solid carbide endmill with an insert cutter.
But you must be aware that I say this as the proud owner of a Haas Minimill so I can hardly make a useful comparison with your OKK.
Also I don't need to make time on what I cut, so I can afford to baby the beast in a way you may not be able to.

I run, as my typical roughing cutter, a bog standard TiAlN coated 4 flute 5/16" diameter Garr endmill.
I do it because they are cheap to buy and are stiff enough that I can remove just as much metal per unit time with them as I can with a 1/2" cutter at twice the cost.
I also run at about 6% stepover and typically 1/2" DOC...all my Minimill can take before it starts to wobble.
I can't remember offhand what chipload I'm running but yours sounds about right.

Titanium specific cutters have been a great waste of money on my setup, so with sore disappointment in my heart I went back to the Garrs.

I encourage you to conduct some empirical experiments on some scrap stock.
See what works for you...push it to failure if you're minded to and make your decisions.
That's what I did, and that's how I came up with my own very personal formula for cutting Ti on my own machine.
I use it for everything now, and don't even think about it or try to tweak it anymore.
I have a bazillion 5/16" 4 flute Garr cutters in the cutter drawer.
I steadily go through them.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[allloutmx]

Hi alloutmx:
I cut a fair amount of Ti6Al4V titanium too, and what I've found after some experimentation is that I cannot beat the MRR of a solid carbide endmill with an insert cutter.
But you must be aware that I say this as the proud owner of a Haas Minimill so I can hardly make a useful comparison with your OKK.
Also I don't need to make time on what I cut, so I can afford to baby the beast in a way you may not be able to.

I run, as my typical roughing cutter, a bog standard TiAlN coated 4 flute 5/16" diameter Garr endmill.
I do it because they are cheap to buy and are stiff enough that I can remove just as much metal per unit time with them as I can with a 1/2" cutter at twice the cost.
I also run at about 6% stepover and typically 1/2" DOC...all my Minimill can take before it starts to wobble.
I can't remember offhand what chipload I'm running but yours sounds about right.

Titanium specific cutters have been a great waste of money on my setup, so with sore disappointment in my heart I went back to the Garrs.

I encourage you to conduct some empirical experiments on some scrap stock.
See what works for you...push it to failure if you're minded to and make your decisions.
That's what I did, and that's how I came up with my own very personal formula for cutting Ti on my own machine.
I use it for everything now, and don't even think about it or try to tweak it anymore.
I have a bazillion 5/16" 4 flute Garr cutters in the cutter drawer.
I steadily go through them.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

Marcus-

Thanks for the intel. I have yet to try the Garr against my current setup but will do in due time.

 

[crossthread82]

My vote would be a 7 flute XT7 from Swiftcarb w/ chipsplitters and MDC coating. They've worked good in the limited Ti that I've done. YMMV

 

[empower]

We have a long standing order for an aircraft part where we remove approximately 75% of the material with (2) 1/2" diameter endmills. Material is 6al4v. Im averaging about 20pcs per tool utilizing dynamic tool paths around the profile.
This job was running when I got here, and the person that started the project is no longer here so Ive been working my way through some of the issues in the process. At this point Ive tried a few different tools and manufacturers but so far, am have the most success with my 5flute reg length and 6 flute stub Titan brand endmills(what an unfortunate brand name). Ive thought about trying to rough the profile with an insert tool but my exploratory toolpaths show a much greater cycle time and even if I use a larger diameter insert tool, ill still need to come back in with the 1/2" tool to clean out the smaller rads.

Curious, who is making the best endmills for milling titanium and in which configuration? mainly looing for tool life improvements.

Currently running about 350ish SFM and .0067chipload. 6% radial DOC on an OKK Horizontal


Thanks In Advance.

give Fraisa tools a try, their MFC line should do great!

 

[Orange Vise]

What's your current tool length and what's the max axial DOC required?

I've got something I can send you to try out.

 

[empower]

What's your current tool length and what's the max axial DOC required?

I've got something I can send you to try out.

you're in the tool business now? holla atcha boi

 

[Orange Vise]

you're in the tool business now? holla atcha boi

Let me know what you need! DM thru IG works well.

 

[guythatbrews]

Alloutmx I don't have anything to add other than good job explaining your process requirements.

Wish everyone did as good!

 

[allloutmx]

What's your current tool length and what's the max axial DOC required?

I've got something I can send you to try out.

Im going .850" deep with my regular length tool. I appreciate you reaching out Eric....its been a while. Hope all is well.

 

[allloutmx]

Alloutmx I don't have anything to add other than good job explaining your process requirements.

Wish everyone did as good!

Ha.... not my first rodeo. Ive been scolded plenty enough to know better

 

[allloutmx]

give Fraisa tools a try, their MFC line should do great!

I would like to try Fraisa- their website is a little hard to understand so Ill likely have to find a rep.

 

[huskermcdoogle]

I would go with a 7 flute Widia/Hanita Varimill III. Smidge longer than you need at 1.25" loc, but they will go and go and go, and tool to tool consistency is great. They also have a chip splitter version if that suits your fancy. But IMHO, with superalloys, chip splitters are typically an early failure point for a tool. You need them when you need them for chip evacuation purposes, but if not needed, most of the time an edge without chip splitters will last longer.

You're speeds and feeds are pretty much right on the high end of where any high performance tool should run. You are @ 2.29in^3 MRR with a 1/2" 5 flute @ 350 sFM and .0067ipt. That is a chip thickness of .0032 (aggressive for a 1/2" in TI, but if it isn't chipping out quickly, go for it).

With the above tool my step off point would be: 210 SFM(1604 RPM), .0043ipt (47.73ipm), .850" axial, .060" radial. This is a chip thickness of .0025", which is a tad more conservative than you were at. Surface footage is also a bit more conservative, especially since we are using much less added speed factor. Should give you much much more tool life being more conservative, and still a little bit faster cycle time. Bonus if you have air travel time, you will have less of it in this case being double the radial. I always did better with heavier radial loads in Ti as long as things were stable and chip evacuation wasn't a problem.

Contact your local Kennametal/Widia rep if you want to test one.

 

[kazlx]

I would like to try Fraisa- their website is a little hard to understand so Ill likely have to find a rep.

Currently talking to a rep from Fraisa for similar situations. Supposedly they have a tool that will ramp at 10*. I'm waiting to get some tools to try out, but I've been really happy with the Helical 6fl Ti stuff.

HEM

www.helicaltool.com

 

[Nagol]

I'd give Gorilla Mill a try. They have some really great tools for stuff like this. I haven't used them in this material but they do have a tough coating for machining tough material. As an apple to apples with what you have you could go with a 6 flute Kong with their WTF coating. Available with a chipbreaker if you want. I've found they make a really competitive product at a really nice price. Prices and inventory numbers are on the website. Feeds and speeds in the book are really nice. I haven't looked super hard but I haven't found anything to compete for job shop machining like I do in the last 4 years. Don't get diswayed by the monkey marketing. It's funny if you lean into it and they really make a great product.

1/2" Diameter Square End (6FKI) | Gorilla Mill

Based in Milwaukee, WI – Gorilla Mill has over 30 years experience manufacturing the best carbide drills, end mills and cutting tools in the industry.

gorillamill.com

 

[allloutmx]

My vote would be a 7 flute XT7 from Swiftcarb w/ chipsplitters and MDC coating. They've worked good in the limited Ti that I've done. YMMV

So...ive never had a ton of luck using an EM with chip breakers, but I thought what the heck, maybe this is a perfect opportunity, and I decided to order a IMCO INCONEX to try, and it was a total fail for me. I would think more flutes/stiffer tool, would be the ideal situation but so far this 5 flute is out performing the 6 flutes ive tried.
Will check out swiftcarb- thanks for the intel

 

[crossthread82]

So...ive never had a ton of luck using an EM with chip breakers, but I thought what the heck, maybe this is a perfect opportunity, and I decided to order a IMCO INCONEX to try, and it was a total fail for me. I would think more flutes/stiffer tool, would be the ideal situation but so far this 5 flute is out performing the 6 flutes ive tried.
Will check out swiftcarb- thanks for the intel

It comes standard without the chipbreakers, I had them add them for my application.

 

[Mtndew]

Someone mentioned Garr, what about Sandvik Plura?

These guys make pretty good end mills, maybe pick one up and try?
https://fullertontool.com/products/end-mills/3116-timill

 

[SWYooper]

I've been using an OSG HP400-1968 (5mm) to rough out a slot in TI 6AL4V with some good high pressure application. The slot is .228W x .5L x .400D so it isn't doing a TON of work, but when I broke this setup down after 5500 pieces (plus another few dozen setup/scrap parts) I was quite surprised with how the tool looked. Cutting edges were sharp, even though the coating had taken a beating. They have a variety in 1/2" as well.

This is in a Swiss machine (Citizen D25) with oil for coolant.