Problem- titainium

[BRIAN SIMP]

Having alot of insert breakage working with this stuff. I use an iscar milling tool with a HM90 APKT 100312PDR IC908 tailn coated. Speed of about 260 sfm and 15-20 ipm.
does anyone have any ideas on some new grades ? ic328 or the alum. ic28 maybe some ideas on speed and feed. thanks

[JROM]

just pretend it's stainless steel. and make shure to use alot of lube. titainum likes to get married to other metals so it will build up on your tools if your not carefull. That's what is breaking your tools.

[naytep]

Look up your SFM in the MH or other source. I think that you should be down around 90 SFM and .005" feed per rev per flute. Those number work well with Alloy X.

[bugzpulverizer]

My experience is you need a high chip load on tools. Tools need to cut not rub. If they start rubbing and heating up, they will break down faster than you can say "e-stop." Lot's of coolant!

[mc-motorsports]

I was always told don't use coated inserts or endmills on titanium or aluminum, you get a better finish anyway. Something along the lines of galling? You could always go to PCBN, EXENSIVE! blah, mistakes including improper feeds and speeds are too expensive. If your doing MAJOR production and have time to tune your feeds and speed, might be the way to go.

[SORCHEROR]

coated inserts on titainium and aluminum always get build up in them,i use uncoated
on them without any issues,try cutting with more chip load it helps

[davereagan]

Call your Iscar guy. You' paying for that knowledge base. 260 sfm is mighty high for Titanium alloy. I'm assuming it's 6Al-4V you are cutting. TiALN inserts (IC908) will last longer dry than wet. I've proven this to myself repeatedly on several different materials.

Dave

[rhundl]

We cut alot of 6al-4v and we have alot of success... To me it sounds like your speeds and feeds are way off. I want to say off memory we are running around 75 sfpm with like a .005 chip load. Bugzpulverizer was right, too slow of feed and you will have major problems but too high of speed will have the same results. Try recalculating your feed and speed with the figures above... We cut dry and wet and have about the same results either way

[dertsap]

i agree with the majority , sfm is to high ,
if the inserts are rated for titanium then they should be able to do it , the manufacturers guidlines should be the best info you can get ,

if your heavily engaged into the material you will need to be keeping the chips cleared , if the tool sucks those chips back into the cut your tool will take an immediate beating ,if youve got thru spindle coolant then i would suggest using it ,
rhundl's suggestion would be your best bet at 75 sfm to start , also try pouring some straight consentrate into the machine to up the oil percentage as well

[K&Y]

Originally Posted by mc-motorsports I was always told don't use coated inserts or endmills on titanium or aluminum, you get a better finish anyway. Something along the lines of galling? You could always go to PCBN, EXENSIVE! blah, mistakes including improper feeds and speeds are too expensive. If your doing MAJOR production and have time to tune your feeds and speed, might be the way to go.

I think you may have gotten PCD and PCBN mixed up in this case, as PCD is used in non-ferrous applications, and PCBN is used to turn, bore and face hard materials. As far as mistakes with improper feeds and speeds, there is a lot of information out there to help you out when it comes to determining what speeds and feeds may be right for your specific application. (Please see attached Speeds and Feed charts for PCD).


As far as the difficulty with Titanium, I'll repost what I said in another thread. Hopefully, this will give you a good starting point:

"We have had experience with this very material with a few clients in the aerospace industry already. I can give you some very basic specifications and it should give you a very good idea of where you should be. Bear in mind, these results were attained using PCD inserts, as opposed to carbide inserts. As far as the coolant option, you can substitute your own brand of coolant. This is just what had been chosen for this particular test.


Workpiece:........................Ti-6Al-4V
Cutting Speed:...................120 m/min.
Feed Rate:........................0.127 mm/rev.
D.O.C.:..............................0.010"
Tool:.................................SPG 422 (fine grain PCD insert) with an 11° relief/front clearance angle
Tool Holder:........................CSSPR, 45° lead
Lathe:...............................Okuma


I hope that this information can at least give you a good starting point with your project. If you need any more info or have any questions, please feel free to ask. I'd be happy to try and help."

[ImanCarrot]

Just a quick thought... you are Climb milling, not Conventional milling aren't you?