Results 1 to 19 of 19

Thread: inconel

  1. #1
    nomgis is offline Cast Iron
    Join Date
    Dec 2005
    Location
    chicago
    Posts
    260

    Post

    I have to turn some inconel.What are the best inserts to use for this stuff?Never cut it before have no idea.

  2. #2
    Xjenderfloip is offline Stainless
    Join Date
    Feb 2005
    Location
    Rotterdam
    Posts
    1,236

    Post

    What grade, 600, 625, 750?
    Positive rake, iserts with coating you would use for SS, deep cuts and easy on the feed.
    The insert will crater at where the crest is.
    Most of the time inserts get destroyed at the end of the cut (in the neck of your stock)where the leftovers of previous cuts get ugly.

    If you got a lot to make i would defenatly heat treat it for much better machinebility

  3. #3
    MALICE is offline Member
    Join Date
    Feb 2005
    Posts
    75

    Post

    I would advise against coated inserts, they don't do much good with inconel. Use something uncoated like H13 or H10 (i can't remeber exactly which one) from Sandvik. Positive rake. Use a firm feed like .02"/rev, and low 100's as far as SFM (read the sandvik book for the feeds and speeds) the inserts arent going to last very long so you're better off taking as much material off as you can. Don't expect very much life out of them, i think you're looking at MAYBE 7 mintues of life per insert (constant cutting). Lots of coolant. Don't be surprised if you have to change inserts before you have the part done. When we first started working with inconel, we were beating our heads trying to figure out how to get good tool life until we figured out that you don't get good tool life with inconel.

  4. #4
    pi
    pi is offline Stainless
    Join Date
    Jan 2005
    Posts
    1,684

    Post

    my thoughts exactly. no coating and go with sandvik's aluminum grade inserts.
    .022-.025 feed at .02 doc. upto 185 sfpm.
    if you really want to fly try greenfield ceramics with 1500+ sfpm

  5. #5
    MALICE is offline Member
    Join Date
    Feb 2005
    Posts
    75

    Post

    We take .1" DOC at work on our CNC mills. Go as deep as you can get away with (or as deep as you're brave enough to go). And don't leave the machine!!!! When the insert is done you dont have a very long period of time to pause before things can get exciting. Havent tried ceramics yet.

  6. #6
    Xjenderfloip is offline Stainless
    Join Date
    Feb 2005
    Location
    Rotterdam
    Posts
    1,236

    Post

    Malice, i dont agree with non coated inserts, mainly becuase of what you said yourself:

    we were beating our heads trying to figure out how to get good tool life until we figured out that you don't get good tool life with inconel
    If your inserts with coating last shorter then uncoated, you have the wrong coating/ brand.
    Coating will increase cutting speed.

    But the type of part you make and the difference in inconel grades make it tough to discuss tools in general.
    For example PI says .022-.025 feed at .02 doc. upto 185 sfpm.
    I remember a job where i had to make 15 diaphragm disks, average OD was 24" thinkness was 1 1/4" had to be digged out at 1"from the OD till center at 10 mm thickness, thats 0.393 inch left, meaning almost an inch material removal from 22" to center.
    If i where taking .022-.025 feed at .02 doc. i would still be busy with it.
    I took a kennametal triangular 22 mm finishing insert, 5mm(0.19") doc 0.25(0.014 feed.
    Insert lasted 1 hour, the trick was to put the tool at 45 angle like a " V " (sorry i dont know the words in english )at the workpiece.
    Made 1-1/2 disks a day.
    The only downside was that the 15 mile strings didnt break (i guided them nicely away from everyone )

    I know its not always possible to use your tool like that, but i saw iscar had made an insert with a big nose touching the work like that " V "

    And with smaller workpieces it might work out better with the aluminum grade inserts,(altough i would get grinded+coated).
    .022-.025 feed at .02 doc. for those inserts show that they work great as long as they dont pass the nose radius(confirming the " V "theory)but past the nose it will crater anyway, so in that regard a grinded tool is too weak and will break with dirty cuts.

  7. #7
    nomgis is offline Cast Iron
    Join Date
    Dec 2005
    Location
    chicago
    Posts
    260

    Post

    P.I. that's what I was thinking.I read an article just recently where they were milling it at 6300 sfm. Yes 6300 sfm if it was inconel. So I was thinking of trying the ceramic but never turned it so was wanting opinions thanks!

  8. #8
    Bobw's Avatar
    Bobw is online now Diamond
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    5,293

    Post

    P.I. that's what I was thinking.I read an article just recently where they were milling it at 6300 sfm. Yes 6300 sfm if it was inconel. So I was thinking of trying the ceramic but never turned it so was wanting opinions thanks!
    6300 sfm, that might have been me, it was A286(annealed), also trade named as incoloy. Ceramics are cool, but to use them effectively you have to understand how they work. They don't "cut" they sort of push. Hold a ceramic insert in your hand and if feels like a piece of plastic, kind of like a lego.

    What they do is generate a huge amount of heat, and with that heat they plasticize the metal in front of the insert. The metal gets gooey soft, and the plastic feeling insert has no problem pushing it out of the way. The ceramic insert, being ceramic doesn't feel the heat too much since it is an incredible insulator. your tool doesn't melt, and the hot metal on the part goes away before it can radiate that heat into the rest of the part.

    Now, Kennametal told me that it was impossible to run their ceramics on the parts we were running because it was too soft(13C). I sent them a video of their tools working. 3000sfm wasn't enough SFM to create enough heat to allow the ceramics to work. On some material, 3000sfm may be too much due to the heat generated. On a lathe, your insert is going to be in there and working, so the SFM will be lower, to keep the amount of heat correct, if your running an interupted cut, as in hex bar or on a mill, you need to crank up the SFM to keep the heat going, its everything opposite of everything you've ever learned about cutting metal, but it works. On a carbide insert, a chipped edge means slow it down, on a ceramic, it means speed it up, or more feed. Wierd little critters.

  9. #9
    Bobw's Avatar
    Bobw is online now Diamond
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    5,293

    Post

    If your inserts with coating last shorter then uncoated, you have the wrong coating/ brand.
    Coating will increase cutting speed.
    I will disagree with this statement, from personal experience. On the A286 in the above post, we ran a large enough lot to get a lot of data on our tools. I kept track of it, afterall, tools are money. The TiAlN coated carbide tools actually had 30% less tool life consistantly. I had two different people tell me the same thing, the process that puts on the coating dulls the edges slightly, and as PI said, high nickel alloys like to be sheared and respond incredibly well to aluminum type tooling, very positive, very sharp and high shear.

    On other materials, coatings will help you, we ended up with about 80 1/2" carbide roughers beat to hell from the A286 job and the coated ones resharpened, with the flutes naked and the OD coated will outlast the uncoated resharps by about 50% on conventional materials.

    High nickel alloys are wierd. As an example we found that at 100sfm we would get 180 minutes of tool life(about 3 parts). At 130 SFM with the same tool path, same chipload we would get 300 minutes of tool life. So at a higher metal removal rate, we got a higher dollar per metal removal rate of a very large% This held true for the coated and uncoated versions.

  10. #10
    metlmunchr is offline Diamond
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,267

    Post

    One of my customers makes literally tons of inconel parts, from small ones up to some 5ft or more in diameter. A walk thru the place leaves no doubt they know how to cut the stuff. Every part looks like its been chromed.

    They have an extensive tool grinding shop in house, and run a lot of inserts that are modified prior to use. Stuff like CNMG's in a Kennametal K68 grade (ancient aluminum grade) ground on an angle across the top surface at the corners to produce a high positive rake. On-edge triangular grooving inserts where they start with a coated insert and grind the top side to get rid of the coating, but leave the coating intact on all other surfaces. Lots of other sorta strange looking modifications too, but the one thing that seems consistent is that the cutting edge is uncoated.

    They also run lots of Greenleaf ceramics wherever possible. They seem to know how to make it all work productively, and the recommendations from malice, pi, and bobw all fit right in with what I've seen them doing.

  11. #11
    Xjenderfloip is offline Stainless
    Join Date
    Feb 2005
    Location
    Rotterdam
    Posts
    1,236

    Post

    Keep the thoughts and experience coming, super alloys are always an interesting subject.

    Material grades make all the difference, with inconel 600 or 625 you can indeed get away with noncoated, when its annealed, but its totally different from incoloy 800(HT) or 825.

    Most ideal situation with milling would be round insert so the edge where material and air meet is wider, or "negative"

    Wich makes me think, in theory a roughing mill with extreme high ribbs should do better, unfortunatly i dont have much experience with milling it, other then with HSS, so i dont know.

    I have turned alot of inconel and everytime the material is different, sometimes it is forged(you know when the material has flats), sometimes burned from plate, clean rods however always seem concistant in hardness/toughness, but always a bit harder.

    I have used noncoated inserts but i always had to lower the cutting speed, compared to coated, however the sharpness of noncoated seemed to react better mainly becuase of less friction, not so much becuase it has no coating, it seems that most coatings are too brittle or cause too much of a negative "rounded" cutting edge, thats why i tend to use coated (grinded) finishing inserts on operations where you have to use 90° tools.
    But with roughing a rod it seems that a very allround cnmg insert at a 45° approach(yes i found the word [img]smile.gif[/img] ) has an extremely long life.
    In this case its not nessecary to have noncoated insert, it will only slow down.

    So why is it that a negative approach (or a round insert)does brittle the coating on the material/air border less?
    My guess is a few things, thermoshock, the wider the border, the less chance of thermoshock.
    Less pressure per mm˛, spreading the heat, thus less placticising of the coating.

    A few things to try:

    High pressure coolant(40bar+)\

    Turning with inert gas (would that be MIG turning )

    Extra coated insert, TiN/TiCN/TiNTiN/TiCN/TiNTiN/TiCN/TiN on a supersharp super endurable carbide with diamond hardness, yet super tough(im afraid we have to wait a few years for that)

    Anyway, just rambling a bit

  12. #12
    pi
    pi is offline Stainless
    Join Date
    Jan 2005
    Posts
    1,684

    Post

    DO NOT USE COATED INSERTS ON INCONEL!!! IT'S THAT SIMPLE. material sticks to the coating and the insert chips. need the heat from the uncoated insert so the material will melt and flow.

  13. #13
    MALICE is offline Member
    Join Date
    Feb 2005
    Posts
    75

    Post

    The bottom line is, it all depends on exactly what your application is. I'm sure there are some situations where coated may be a better way to go. Others, you're better off going with uncoated. The other thing to consider is this: how many parts are you going to run? If you have a million parts to do, you're probably going to go spend the money on a certain type of inserts especially for that purpose. If you have 3 to do, you may as well just buy inserts that are going to do the job, but you are also going to use for other materials/jobs down the road. For a vague example, you can use Sandvik 1025's to turn inconel, and chances are you'll use them on another type of material. They're not going to last as long, but they won't sit in a shelf collecting dust, never to be used again. On top of that, everyone has a different way of machining. What works for me, may not work so well for someone else. What's acceptable in one shop isn't in another.

  14. #14
    Xjenderfloip is offline Stainless
    Join Date
    Feb 2005
    Location
    Rotterdam
    Posts
    1,236

    Post

    This link will explain better what i mean with insert geometry, and that with better geometry the coating can hold, sandvik has a nice start with this product.

    movie (save target)

    "SANDVIK Coromant has released a new tooling solution for machining titanium alloys and heat resistant super alloy materials........ click to read more

  15. #15
    Join Date
    Jun 2005
    Location
    South Western PA
    Posts
    947

    Post

    I know this thread is kind of old, but Arthur R Warner Co (http://www.arwarnerco.com/)of Latrobe, PA swears up & down the HSS does better than carbide on inconel. They sell HSS cutter ground to carbide insert shapes, molded carbide feature are not available.

    Ted

  16. #16
    JRIowa's Avatar
    JRIowa is offline Diamond
    Join Date
    May 2003
    Location
    Marshalltown, Iowa, USA
    Posts
    7,634

    Post

    need the heat from the uncoated insert so the material will melt and flow
    With Inconel melting at about 2,500 deg F, not on any of my machines.

    We typically run Inconel, Monel, Hastalloy, etc. at about 15-20 SFM with HSS or in the 80-250 sfm range with carbide. And yes, we used coated inserts. We do a lot of castings so we haven't found a ceramic that will work for most of our applications. The biggest thing with any of the high nickal materials is that you need to cut something. Slow the RPM down and pick the feed up.

    Most of our guys don't mind Inconel, it's one of our more predictable alloys. Most of them hate duplex stainless and Nitronic 50.
    JR

  17. #17
    bradleyk is offline Cast Iron
    Join Date
    May 2005
    Location
    Ohio
    Posts
    285

    Post

    JR,

    You're guys would rather machine Inconel than Nitronic 50? The duplex SS I can understand but not the Nitronic.
    Most of my work in the nickel alloys is turning barstock in the strain hardened condition so there will likely be some differences to machining castings. I run Monel much faster than what you are running...about as fast as 300 series SS. My major problem with Monel and a couple of the Inconel grades is tearing.

    I use Sandvik 2025 for roughing and 1025 (PVD) for finishing since I have a mixed production od SS and high temp alloys. They even work well on titanium.

    I posted a question about NPT threading last year
    http://www.practicalmachinist.com/cg.../13/1745.html?
    I still haven't been able find a consistent way to get tool life on NPT thread inserts.
    I have one lathe capable to thread mill but only able to hold the thread mill in an ER collet. We did some threads in Hastalloy but they had lots of chatter (then the tool broke after a couple
    more parts..and broke two more after that).
    As I said in my previous post I don't have problems with other threads (UN, UNJ, whitworth, BSPT) but the NPT is the killer.
    Got any tips?

  18. #18
    JRIowa's Avatar
    JRIowa is offline Diamond
    Join Date
    May 2003
    Location
    Marshalltown, Iowa, USA
    Posts
    7,634

    Post

    Brad,
    Our biggest problem with Nitronic is keeping it straight. We end up with a design that calls for turning down a 1.5" dia. bar to 1.25" for 40+ inches and keeping it straight within 0.005". Take one pass and the Nitronic warps one direction and the next pass it warps another. It gets very frustrating to work with.

    We're a KM shop for the most part. About 90% of our $10K/month budget is KM.

    I'll have to go out this morning and look at our set-ups for threading. Nothing will be pipe, it's our own design threads with a sharp taper on the end.

    Most of the guys here consider 300 series "gravy work". We do a lot of CF8M castings (316) with weights up to 10K lbs.
    JR

  19. #19
    bradleyk is offline Cast Iron
    Join Date
    May 2005
    Location
    Ohio
    Posts
    285

    Post

    I'm running parts much, much smaller than you...now I understand the Nitronic problem.
    We also consider 300 series SS as gravy...especially when compared to the high temp alloys.

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •