Constant Surface Speed inexperience. - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 40 of 40
  1. #21
    Join Date
    Aug 2009
    Country
    AUSTRALIA
    Posts
    522
    Post Thanks / Like
    Likes (Given)
    108
    Likes (Received)
    72

    Default

    In my experience with lessor grade inconels a 45 degree approach makes a huge difference. As stated a sharp tool, and 45 degree chamfer at cut start. Sandvik make a cnmg insert with a 45 degree corner on it, never used it though. An snmg or button tool were my first choice. I’ve also used a small 45 degree inserted, shanked milling cutter as a boring tool. So much better then any 90 degree or thereabouts tool.

  2. #22
    Join Date
    Jul 2011
    Location
    Scranton, PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    6

    Default

    Quote Originally Posted by number 2 View Post
    In my experience with lessor grade inconels a 45 degree approach makes a huge difference. As stated a sharp tool, and 45 degree chamfer at cut start. Sandvik make a cnmg insert with a 45 degree corner on it, never used it though. An snmg or button tool were my first choice. I’ve also used a small 45 degree inserted, shanked milling cutter as a boring tool. So much better then any 90 degree or thereabouts tool.
    Well ive gotta figure something out for.monday morning. This is a hot job. Hoping i can figure out the tooling and css to maken it work

  3. #23
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,516
    Post Thanks / Like
    Likes (Given)
    1193
    Likes (Received)
    2502

    Default

    Quote Originally Posted by nissan300ztt View Post
    Well ive gotta figure something out for.monday morning. This is a hot job. Hoping i can figure out the tooling and css to maken it work
    You've been given the answers with the Tooling you have.

    Machine a 45° angle at the entry to the Roughing pass.
    Talk to your people about better Inserts.
    Slow your SFM down to 80.

    If the Machine doesn't have the torque at 30-40 RPM, then get the lift truck, haul them bars over to an Engine lathe and start Turning them down to a usable Diameter. If you don'thave a manual lathe that'll do it, haul them over to the Mill and start Milling the diameter. Just get the chips coming off somehow. If the CNC lathe has live tools use them. Maybe start work on the IDs until the Tooling arrives. Can't just stand there with your thumb up your ass.

    R

  4. Likes nissan300ztt, Matt_Maguire, eaglemike liked this post
  5. #24
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    2,039
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    948

    Default

    Quote Originally Posted by number 2 View Post
    Sandvik make a cnmg insert with a 45 degree corner on it ...
    I can't imagine a cnmg working well on inconel. I've always used positive rake, sandvik knux inserts worked okay but the edges wear fast.

    But if he can't even buy a box of inserts, hell. May as well just close up the shop. That's stupid.

  6. Likes eaglemike liked this post
  7. #25
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    597
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    201

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    I can't imagine a cnmg working well on inconel. I've always used positive rake, sandvik knux inserts worked okay but the edges wear fast.
    Aside from Ceramic cnmgs are the way to go. on our bigger 20"+ dia parts we ran cnmg643 in h13 cutting half insert width close to 1/2"? with 1/2" round ceramics we were taking .200 depth of cut.
    The pressure that was generated was incredible we were running 100hp-150hp motors on old HES lathes.

    Hell my old 1990 hitech 20sII with a 8" chuck was taking .1 DOC on ceramics and about he same with CNMGS.
    one money saving trick with carbide on inconel is you use the cheapest carbide insert you can because its going to chew them up the same no matter what the cost, your going to get the same life.

    greenleaf ceramic guy and the sandvick practically lived in our shop. we were Garrett aviation and greenleafs test shop for whisker ceramics on inco waspoly and haynse/mars and a few others ( aka Ballbustrum )

    positive rakes work good for finishing only on inco with light finish cuts.

  8. #26
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    1,004
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    412

    Default

    If you have a live A and/or B axis, do spinning tool roughing. R inserts, coolant, lighter cuts, but more feed. Last liberty is velocity of cut. Once found the right speed, program G96 SXXX just before cut and enjoy.

    I agree with the opinion that the setup should be rigid and sound.

  9. #27
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,436
    Post Thanks / Like
    Likes (Given)
    533
    Likes (Received)
    765

    Default

    Quote Originally Posted by nissan300ztt View Post
    Yeah. Im going from 8.05" to 4.01" and then operation 2 is gonna a bore from 2" to 4.20" my boss is gonna hate me. Guess were spending money
    so you're gonna turn it down to 4.01 then bore it to 4.2? I'd say inserts may be the least of yer worries with those dims....

  10. #28
    Join Date
    Aug 2009
    Country
    AUSTRALIA
    Posts
    522
    Post Thanks / Like
    Likes (Given)
    108
    Likes (Received)
    72

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    I can't imagine a cnmg working well on inconel. I've always used positive rake, sandvik knux inserts worked okay but the edges wear fast.

    But if he can't even buy a box of inserts, hell. May as well just close up the shop. That's stupid.
    This is the CNMG I refer to:
    Google Image Result for https://image.slidesharecdn.com/56f06b56-0a58-4f76-b76a-7d376519c122-160225030513/95/heat-resistant-super-alloys-application-guide-17-638.jpg?cb=1456371986


    If you can’t get a decent doc to work with a regular insert use 75% or there a bouts of the nose radius. More cuts but it will work better.

    A 45 degree angle, or some angle less then 90 will make it much more successful.

  11. Likes Philabuster liked this post
  12. #29
    Join Date
    Jul 2011
    Location
    Scranton, PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    6

    Default

    Quote Originally Posted by litlerob1 View Post
    You've been given the answers with the Tooling you have.

    Machine a 45° angle at the entry to the Roughing pass.
    Talk to your people about better Inserts.
    Slow your SFM down to 80.

    If the Machine doesn't have the torque at 30-40 RPM, then get the lift truck, haul them bars over to an Engine lathe and start Turning them down to a usable Diameter. If you don'thave a manual lathe that'll do it, haul them over to the Mill and start Milling the diameter. Just get the chips coming off somehow. If the CNC lathe has live tools use them. Maybe start work on the IDs until the Tooling arrives. Can't just stand there with your thumb up your ass.

    R
    100% agreed. I will definitely have an approach monday morning.

  13. #30
    Join Date
    Jul 2006
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    4,589
    Post Thanks / Like
    Likes (Given)
    18427
    Likes (Received)
    4306

    Default

    These Sandvik CNMX 432 inserts do work on 718. I had good luck with them. Just need to grind a flat on the toolholder's anvil for clearance so the anvil doesn't cut into the work. Also best to reduce feedrate by 50% about 1/8" away from the end of the cut when cutting up to a 90° shoulder.

    https://www.mscdirect.com/product/details/65332777
    Attached Thumbnails Attached Thumbnails sandvik-cnmx-insert.jpg  

  14. #31
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    2,039
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    948

    Default

    Quote Originally Posted by Delw View Post
    Aside from Ceramic cnmgs are the way to go. on our bigger 20"+ dia parts we ran cnmg643 in h13 cutting half insert width close to 1/2"? with 1/2" round ceramics we were taking .200 depth of cut.
    The pressure that was generated was incredible we were running 100hp-150hp motors on old HES lathes.
    Well, I'll take your word for it cuz Garrett does more big inc than me. I'd be pretty nervous about negative rake in inconel but if it comes up again, will give it a try ... next time I have a 100 horse spindle

    For smaller stuff, knuxes worked okay. Ate a lot of inserts but worked all right and didn't make the part 800* F

  15. #32
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,516
    Post Thanks / Like
    Likes (Given)
    1193
    Likes (Received)
    2502

    Default

    Gurutzbe B1400 is the only up to date-ish CNC Lathe currently on the new market, with 100hp. as an option. Okuma has a VTL with 60.

    R

  16. #33
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    597
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    201

    Default

    Quote Originally Posted by litlerob1 View Post
    Gurutzbe B1400 is the only up to date-ish CNC Lathe currently on the new market, with 100hp. as an option. Okuma has a VTL with 60.

    R
    Bob these were old machines made by HES some of the 1st cncs huge ass numerx control bow about 5 foot tall 3 foot square. if I recall the motors were org 50 or 75hp.
    the shop I worked at put 6" spacers under the head to raise it. and fagor controls.
    we had 2 old ones and one new one( 1991).

  17. #34
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    597
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    201

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    Well, I'll take your word for it cuz Garrett does more big inc than me. I'd be pretty nervous about negative rake in inconel but if it comes up again, will give it a try ... next time I have a 100 horse spindle

    For smaller stuff, knuxes worked okay. Ate a lot of inserts but worked all right and didn't make the part 800* F
    I think you missed the part were I said we cut Inco in hitachi sekie Hi-tech 20sii with a 8" chuck. that was an LM guide machine.
    My Miyano knc 45 cuts inco very well with cnmg432, Last job we did was around 500 pcs 3/4" dia cut to .06-.375 dia with features used less than a box of inserts for rgh and 2 or 3 for finish. held .0003 and 63 or better finish all week long. I did use a coated cnmg for these forget which ones(1025?) but they were cheap sandvicks

    positive rake or negitive rake your going through about the same amount of inserts maybe a 10% less but you will save on the cost of inserts in the long run.
    I'm an old school guy I run slow.

  18. #35
    Join Date
    Jul 2011
    Location
    Scranton, PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    6

    Default

    Thanks for all the input guys. I think i nailed it.
    I ended up just using standard CNMG 2025 sandviks. Bi thinknit came out well
    And apparently this was "aged" inconel 55 rockwell...from what I was told.
    20191014_131528.jpg

  19. Likes eaglemike liked this post
  20. #36
    Join Date
    Sep 2016
    Country
    UNITED KINGDOM
    Posts
    28
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    2

    Default

    Depending on what you are actually making, we have done some large inco parts with a lot of turning.
    I normally would use an snmg and form a 44degree angle. Call a cnmg up and remove the angle the snmg has produced to desired profile. Speed low, Feed high.

  21. #37
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,516
    Post Thanks / Like
    Likes (Given)
    1193
    Likes (Received)
    2502

    Default

    Quote Originally Posted by nissan300ztt View Post
    Thanks for all the input guys. I think i nailed it.
    I ended up just using standard CNMG 2025 sandviks. Bi thinknit came out well
    And apparently this was "aged" inconel 55 rockwell..
    Love it when people follow up.

    R

  22. Likes nissan300ztt liked this post
  23. #38
    Join Date
    Jul 2011
    Location
    Scranton, PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    6

    Default

    Quote Originally Posted by litlerob1 View Post
    Love it when people follow up.

    R
    Yeah. Now im in the process of boring it. Thats cutting easy.

  24. #39
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    67
    Likes (Received)
    136

    Default

    ive used cnmg on 625/718 and was having allsorts of issues with the insert chipping at the DOC line. didnt matter the feedrate or css. eventually i ended up going with .03 shallow DOC but at .060/rev feed at 150sfm...got 3 times the life out of the insert and shaved 4 minute off the cycle time

  25. Likes nissan300ztt, Fancuku liked this post
  26. #40
    Join Date
    Jul 2011
    Location
    Scranton, PA
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    6

    Default

    All bored to size. .001" under size, within tolerance.
    Bored from 1.3" to 5.526" at the large radius.
    20191015_130049.jpg


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
  •