Need help with 316 S.S.
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    Oklahoma
    Posts
    359
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    53

    Default Need help with 316 S.S.

    Hi everybody,

    I usually dont cut 316, and this project might be a long term customer if I can get my tooling to last. It seems that we are blowing through inserts faster than I anticipated. Maybe I'm just not used to 316. I'll list my processes, speeds and feeds, along with inserts and tooling so maybe you guys can tell me whats needs changed. I know we are all busy so thanks in advance.

    Facing/turning, roughing/finishing - 500 sfm /.085 max-.03 min doc /.006-.009 ipr feed(insert sandvik "ccmt 12 04 08-mm 2025")
    -inserts are lasting around 3-4 parts

    Thread mill 1/4-npt - 200 sfm /.0015 ipr feed / tried one pass. nope, tried 4 passes, nope, kennametal insert (grade kc635m)
    -having tons a trouble with this. First insert broke, second chipped cutting edge.

    -Thread milling is my main concern as it seems to hate it. A ton a vibration and inserts are not cheap. My fear is I'm getting some deflection in the spindle which is not allowing full cut on the thread. Should I try to tap it instead?


    Boring, roughing/finishing - 400 sfm /.002-.004 ipr feed / .015 doc (insert is vpgt 221f, which is an older insert).
    -I cant find a tool that has a 35 deg insert set at 107 deg lead like this one (https://www.mscdirect.com/product/details/51865111) but smaller. I have to clearance the insert to keep from rubbing the part. starting with 3/8 hole .210 deep.
    -this insert lasts a little longer, 5-6 parts.

  2. #2
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    906
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    350

    Default

    A few questions. You say 3-4 parts, how many minutes in cut is that? Are you using high pressure coolant or regular flood? Also, is the threadmilling done on a mill with a good, rigid setup, or on a lathe with live tooling?

  3. #3
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    Oklahoma
    Posts
    359
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    53

    Default

    Flood coolant. The part is faced on both sides, two spindle chuck. First side is one face pass .035 doc, and one turning pass .072 doc, total time may be 1'30". Second side is three large facing passes .085 doc, and a contour with 3 rough cuts and a finish .05-.03 doc, total time may be 3'-4'.

    So in three parts its 9-12 minutes on the second side that is the side that is changed most, which makes sense since it does more work.


    Thread milling is on an old fadal vmc. Its not the most rigid machine. I have successfully thread milled 304 s.s. using the same tool with almost no issues.
    Last edited by Tap_or_Die; 03-24-2020 at 12:10 PM. Reason: added more comments

  4. #4
    Join Date
    Dec 2009
    Country
    CANADA
    State/Province
    Ontario
    Posts
    35
    Post Thanks / Like
    Likes (Given)
    20
    Likes (Received)
    49

    Default

    316 can be all over the map. Get it setup one day and cuts great. New batch of material can take out all your tools.

    If it is a production job that keeps coming back buy Schmolz Bickenbach Ugima material. If you start worrying about the price of it stop. You are going to get it all back. Carpenter also had a good 316 stainless as well but I haven't used it in awhile.

    I've found you can't beat the Walter WSM10S inserts for non interrupted cuts. SFM you are running is probably high. When you walk through jobs running stainless in production volumes and take a look at how fast the spindles are turning you will be surprised how slow they are actually running. 316 is easy to run reliably once you get good material but it does run slow.

    But I'd start with tracing the material if you can. Might get some answers.

  5. Likes DanASM, Tap_or_Die liked this post
  6. #5
    Join Date
    Dec 2009
    Country
    CANADA
    State/Province
    Ontario
    Posts
    35
    Post Thanks / Like
    Likes (Given)
    20
    Likes (Received)
    49

    Default

    Quote Originally Posted by Tap_or_Die View Post


    Thread milling is on an old fadal vmc. Its not the most rigid machine. I have successfully thread milled 304 s.s. using the same tool with almost no issues.
    If this is the case can you try different material?

  7. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,100
    Post Thanks / Like
    Likes (Given)
    4657
    Likes (Received)
    3077

    Default

    Could be a bad batch of material because 316 can cut really nice if you have the right speeds and feeds.
    A lot of people prefer it over 304, I'm one of them.

  8. Likes Tap_or_Die, SIM, kevin66, Chazsani, aj liked this post
  9. #7
    Join Date
    Mar 2019
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    238
    Post Thanks / Like
    Likes (Given)
    126
    Likes (Received)
    122

    Default

    Quote Originally Posted by enginuity View Post
    316 can be all over the map. Get it setup one day and cuts great. New batch of material can take out all your tools.

    If it is a production job that keeps coming back buy Schmolz Bickenbach Ugima material. If you start worrying about the price of it stop. You are going to get it all back. Carpenter also had a good 316 stainless as well but I haven't used it in awhile.

    I've found you can't beat the Walter WSM10S inserts for non interrupted cuts. SFM you are running is probably high. When you walk through jobs running stainless in production volumes and take a look at how fast the spindles are turning you will be surprised how slow they are actually running. 316 is easy to run reliably once you get good material but it does run slow.

    But I'd start with tracing the material if you can. Might get some answers.
    Either go with the Ugima from Schmolz or "Project 70" from Carpenter. Its all 316SS. Makes a huge difference and you will be so happy when it machines consistently.

  10. #8
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    Oklahoma
    Posts
    359
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    53

    Default

    I cant, its customer supplied for a test run. Ill ask where they are sourcing the material.

  11. #9
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    906
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    350

    Default

    9-12 min. isn't terrible for tool life but it isn't great, either. As stated earlier by others, it could be your material. IIRC, 316 SS can have a wide range of nickel content which makes a big difference on tool life.

    FWIW, I did look up the Sandvik grade and it looks like the right one. That said, I have found it's usually worth it to try different grades and/or brands in a difficult application. You could check out Ingersoll's TT9xxx line-up.

  12. Likes Tap_or_Die liked this post
  13. #10
    Join Date
    Feb 2004
    Location
    Staten Island NewYork USA
    Posts
    3,842
    Post Thanks / Like
    Likes (Given)
    1144
    Likes (Received)
    1885

    Default

    North American and Valbruna run very consistent too.

    I'll take 316 over 304 just because of the consistency.

    You said thread mill "insert"...Try with a helical solid thread mill. Yes they are pricey, but not bad if they last for many hundreds of parts. I go with a Mari or Lakeshore carbide for the mills, both with similar results.
    I use 200SFM with a feedrate of 9 IPM (.005 per tooth, 4 flute) and take in 3 passes. I run a line of valves in forged 316SS. Two opposing 1/4" NPT features done in a rotary, so not the most robust fixture, I do in lots of 200-400pcs and I've run multple runs with the same mill.

    My way to machine 316SS...slow rpm, sharp tools and cut heavy...always cut as the rubbing makes a workhardened surface the tools just don't like.

    Turning- - they all work, but I'm a fan of Iscar CNMG 432 IC807 for constancy.

  14. Likes Tap_or_Die, Delw liked this post
  15. #11
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    906
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    350

    Default

    I have had good success with OSG's solid carbide threadmills. They have an A brand one that is right hand cut, left hand flute to reduce vibration. IDK if it's worth it or not.

  16. Likes Tap_or_Die liked this post
  17. #12
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    905
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    328

    Default

    Cant help you on thread milling as I dont thread mill.

    However your lathe issues are not the insert nor the metal its the programming for that style insert.

    316 cuts like butter you just need to apply the right info to the type oif material.

    you should be roughing with a cnmg or trigon 4 series and finsihing with that or a ccmt. I liek the ccmt but wont waste my time roughing with it in the docs you got especially facing.

    Your facing is way to aggressive for a ccmt. your more than likely damaging your inserts when you get to the last .150 dia of the facing op especially at the docs you have,
    you didnt say what nose rad you were using either. for facing with a ccmt requiers a little more finess.

    I use 350-400 sfm on cutting 316 od feed runs between .006-.008 I use pretty much only sandvick.
    rough faceing wnmg or cnmg 432 nor more than .050 doc at .004-.005 then once I hit .200 dia I slow it up to .001-.002 feed. this also highly depends on what your max rpm speed is set at. If I want to hog off the faces I use a SNMG or CNMG 432-434 with a holder that holds the insert at 90º

    roughing o.d. 350-400 SFM doc .050-.100 depending on how big the dia of the part is .006-.008 feed depending on the tool nose rad as well.
    Generally you should use a 432 min for roughing as you can turn a tad faster in feed rates and DOC.
    after your done roughing take that same tool and face any faces past the Z 0 face too with in .003 size. its better to start from the largest o.d. and run a few thou from the smaller o.d.

    finishing Separate tool cnmg wnmg or ccmt with with a rad that you can use and interpulate fillet rads. DONT Plunge into them thats dumb and blows inserts and gives you a crappy fillet.
    I leave .003 on the faces for all finish passes(see above) and .010 for o.d.

    again biggest nose rad the better that you can still interpolate any fillet rads with.

    as far as your bore ccmt works great if you have one small enough to clear your bore. if not solid carbide b-bars by internal tool and other manufacturers work fantastic, doc you need to be light on small bores as well as SFM sometimes by 50%.

    What ever you do dont ask your customer what grade his 316 is, where it came from or can he change it cause its too hard for you to cut Cause its not and you will look like a fool in doing so on 316 or 304 stainless.

    Dont know what type of machine you got you said 2 chucks so I assume its a decent machine you shouldnt have any issues as I can cut the stuff on my little Miyano all day long with no issues just like I can on my 10" chuck machines just lighter cuts on the Miyano.

    Just remember its just another "COMMON" Material that gets cut every single days by tons of shops with NO PROBLEMS.

  18. Likes Tap_or_Die, mmurray70, Chazsani liked this post
  19. #13
    Join Date
    Jan 2013
    Location
    Plainfield, Indiana, USA
    Posts
    1,796
    Post Thanks / Like
    Likes (Given)
    1373
    Likes (Received)
    945

    Default

    I like 300 sfm max for 304/ 316 on a lathe. The slower rpm is more than made up for by not chasing tenths, changing tool inserts.
    Thread mills should require multiple passes . . . it sounds like you are taking one pass. Again, longer cycle time is faster than change dull/broken tools.

  20. Likes Tap_or_Die liked this post
  21. #14
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    Oklahoma
    Posts
    359
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    53

    Default

    Quote Originally Posted by Delw View Post
    Cant help you on thread milling as I dont thread mill.

    However your lathe issues are not the insert nor the metal its the programming for that style insert.

    316 cuts like butter you just need to apply the right info to the type oif material.

    you should be roughing with a cnmg or trigon 4 series and finsihing with that or a ccmt. I liek the ccmt but wont waste my time roughing with it in the docs you got especially facing.

    Your facing is way to aggressive for a ccmt. your more than likely damaging your inserts when you get to the last .150 dia of the facing op especially at the docs you have,
    you didnt say what nose rad you were using either. for facing with a ccmt requiers a little more finess.

    I use 350-400 sfm on cutting 316 od feed runs between .006-.008 I use pretty much only sandvick.
    rough faceing wnmg or cnmg 432 nor more than .050 doc at .004-.005 then once I hit .200 dia I slow it up to .001-.002 feed. this also highly depends on what your max rpm speed is set at. If I want to hog off the faces I use a SNMG or CNMG 432-434 with a holder that holds the insert at 90º

    roughing o.d. 350-400 SFM doc .050-.100 depending on how big the dia of the part is .006-.008 feed depending on the tool nose rad as well.
    Generally you should use a 432 min for roughing as you can turn a tad faster in feed rates and DOC.
    after your done roughing take that same tool and face any faces past the Z 0 face too with in .003 size. its better to start from the largest o.d. and run a few thou from the smaller o.d.

    finishing Separate tool cnmg wnmg or ccmt with with a rad that you can use and interpulate fillet rads. DONT Plunge into them thats dumb and blows inserts and gives you a crappy fillet.
    I leave .003 on the faces for all finish passes(see above) and .010 for o.d.

    again biggest nose rad the better that you can still interpolate any fillet rads with.

    as far as your bore ccmt works great if you have one small enough to clear your bore. if not solid carbide b-bars by internal tool and other manufacturers work fantastic, doc you need to be light on small bores as well as SFM sometimes by 50%.

    What ever you do dont ask your customer what grade his 316 is, where it came from or can he change it cause its too hard for you to cut Cause its not and you will look like a fool in doing so on 316 or 304 stainless.

    Dont know what type of machine you got you said 2 chucks so I assume its a decent machine you shouldnt have any issues as I can cut the stuff on my little Miyano all day long with no issues just like I can on my 10" chuck machines just lighter cuts on the Miyano.

    Just remember its just another "COMMON" Material that gets cut every single days by tons of shops with NO PROBLEMS.
    Thank you Sir, Exactly what I was looking for. Ill give a shot. Like I said, I havent ran much 316. Only other job was a small 1/4" pin with a 7/32 blind hole 1/4 deep. Material is already to size so its just face, drill, partoff. Also Im using .03 rad on all tools except for the boring bar. I have some solid carbide bars that should work as well.

  22. #15
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    128
    Post Thanks / Like
    Likes (Given)
    318
    Likes (Received)
    42

    Default

    Only 3-4 parts with only 4 roughing passes doesn't sound right.
    I have a part that I run often in 316 where the diameter starts at 4.25" and goes down to .414" so it's a lot of material removal. 400 SFM, .08" DOC, .01 IPR feed. I use CNMG432 inserts and get 4 parts per cutting edge.
    And why are you using 35 degree inserts for boring? That's a weak insert. And I would use a thread bar for the 1/4" NPT thread.

  23. Likes Tap_or_Die liked this post
  24. #16
    Join Date
    Jul 2007
    Location
    Missoula Mt
    Posts
    287
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    101

    Default

    For tool life slow sfm(rpm) and avoid light cuts and slow feeds, lots of coolant...Phil

  25. Likes Tap_or_Die liked this post
  26. #17
    Join Date
    Jan 2003
    Location
    Canada
    Posts
    11,380
    Post Thanks / Like
    Likes (Given)
    5698
    Likes (Received)
    3506

    Default

    2025 grade is old and soft, try 2220 or 1115.
    I run closer to 350-400sfm usually.

  27. Likes Tap_or_Die liked this post
  28. #18
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    906
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    350

    Default

    Quote Originally Posted by Fancuku View Post
    ................And I would use a thread bar for the 1/4" NPT thread.
    Look at his previous posts. He's threadmilling it, not single point on a lathe.

    >>> OP
    You mentioned you are using .03 rad CCMT inserts. If you are going to go with CCMT, you need a smaller radius. I use .03 for roughing with a CNMG 432 which is WAY more robust than a CCMT 32.52. The problem with such a large radius is feeding hard enough to break a chip and be productive means probably cracking or chipping the insert. FWIW I use a Ingersoll CCMT for finishing stainless, but I use an .008 radius with a .03 doc. Max feed for a nice surface finish is .004 but it's super stable and free-cutting.

  29. Likes Tap_or_Die liked this post
  30. #19
    Join Date
    Jan 2003
    Location
    Posts
    419
    Post Thanks / Like
    Likes (Given)
    79
    Likes (Received)
    121

    Default

    Lots of good info here. I would also recommend a solid carbide threadmill. An insert tool this small cant be any good at all.

    If your threadmilling setup isnt rigid enough consider programming it to spiral in from the top. Little slower this way but you only cut one tooth at a time so much better for weaker setups. This is also a great way to get another shift out of a threadmill with a tooth chipped in the middle. Tools lasts a long time like this, tip does most of the work and rest of tool stays like new to give a nice finish. I would still do multiple passes, maybe 2 rough plus finish.

  31. #20
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    128
    Post Thanks / Like
    Likes (Given)
    318
    Likes (Received)
    42

    Default

    Quote Originally Posted by ChipSplitter View Post
    Look at his previous posts. He's threadmilling it, not single point on a lathe.
    I know he is threadmilling on a Fadal mill. I was suggesting he use single point threading on the lathe.


Tags for this Thread

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
  •