Chatter. Could go for some creative programming or...?
Close
Login to Your Account
Results 1 to 18 of 18
  1. #1
    Join Date
    Feb 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    115

    Default Chatter. Could go for some creative programming or...?

    So we Turn, chucking on to a (304ss) 4ft long, 5in diameter part with a 1.25" diameter shaft 8" long, centered, in a CNC with tailstock.

    Trouble is, when turning the small shaft for a bearing fit, there is a LOT of chatter. I suppose the solution for the past umpteen years has been to have the operator toggle the speed/feed override continuously, which works "well enough" ...

    Lathe is a 1998 Yang, Fanuc, turret type with tailstock, no accommodation for a steady or follower.

    Is there a way to simulate the toggling from a programming perspective, akin to having it ride some sine wave perhaps? I'm running it now and would love to fix this age old problem while sparing my hands.

  2. #2
    Join Date
    Jul 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    54

    Default

    What is your G50 value? Your G96 value? Also, what is your insert geometry for the rougher? I'm assuming the chatter is during the roughing cycle?

  3. #3
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,559
    Post Thanks / Like
    Likes (Given)
    553
    Likes (Received)
    930

    Default

    Is your turning tool optimized for the application? Give some specifics. Your length to diameter ratio is pretty nuts with no follow or steady rest.

  4. #4
    Join Date
    Feb 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    115

    Default

    Likely capped at 450rpm, wouldn't surprise me if they programmed it straight rpm and not sfm. I'll check tomorrow, I'd venture to say it's pretty basic.

    55deg .032R GP chipbreaker AlTin coating

    Same tool roughing/finishing (I KNOW!)

    I'm tempted to rewrite it all together to get roughers and finishers in there.

    There's a lot to be done from a technical standpoint but I doubt I could get them on board with revamping what's "worked" for 20 years, but I'mma try.

  5. #5
    Join Date
    Dec 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    155
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    44

    Default

    Quote Originally Posted by Hardened View Post
    ...55deg .032R GP chipbreaker AlTin coating

    Same tool roughing/finishing (I KNOW!)
    Iscar insert? Try a -TF.

  6. #6
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    7,632
    Post Thanks / Like
    Likes (Given)
    743
    Likes (Received)
    3619

    Default

    My go to default on getting rid of turning chatter is to lower the RPMs then bump the feed up.

  7. #7
    Join Date
    May 2005
    Location
    CA
    Posts
    1,133
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    291

    Default

    Possibly...

    Rough with the tool you have at a high enough feed rate to avoid chatter (reduce depth of cut if necessary).

    Finish with .016" radius insert (or even sharper), at higher speed and lower feed rate.

  8. #8
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    3,016
    Post Thanks / Like
    Likes (Given)
    7106
    Likes (Received)
    2555

    Default

    You need a positive/single sided insert for sure. Something with a thin PVD coating, and probably intended to finish stailess or super-alloys. These will have a sharper cutting edge, and will cause less deflection & cutting pressure - which is what upsets the part & creates chatter in the first place.

    I'd recommend a smaller nose-radius too.

  9. #9
    Join Date
    Aug 2012
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    88
    Post Thanks / Like
    Likes (Given)
    20
    Likes (Received)
    31

    Default

    This won't help the current situation, but if you look at new machines (or even used up to about a decade old), some of them have that harmonic spindle speed control feature built in so you don't have to play with the speed over-ride. My Okuma and my Hardinge have it and it works great. Just set the amplitude and period of the spindle speed oscillation and the finish is beautiful. Turn it on and off with an M code. My Haas has it too, but the machine is not as rigid so it can't achieve the same finish on the same parts.

    With your current machine, I agree with sharp and small radius -- I use .008 nose radius for finishing.

  10. Likes gorrilla, AARONT liked this post
  11. #10
    Join Date
    May 2007
    Location
    Central Texas, West and North of Austin
    Posts
    1,627
    Post Thanks / Like
    Likes (Given)
    178
    Likes (Received)
    531

    Default

    I was gonna say, before TC beat me to the punch, this problem has been approached by Okuma I know, and I figure likely many others, with a harmonic speed variation program, which does the same thing as you standing there floating the spindle speed up and down.
    Why in the hammer headed hell you are seeing resistance to writing a program with separate rough and finish tools I'll never understand. That's SOP around here. We run hundreds of shafts about every 90 days. Bearing fits typically in the +/-.0001 range. The smaller tool nose radius could likely solve your problem, as could the much more positive geometry. But any of these is gonna force you to re-write the program to include a separate finish tool. Which I think you need anyway.
    Just because "it's the way we used to do it" has probably cost more in lost production than any phrase in history.
    Since you are not likely to get a new machine with the fancy software to vary the speed automatically, I'd say look into the separate finish tool, and play with geometry. Good luck convincing somebody above you to spend the money, which is exactly why they are resisting.

  12. #11
    Join Date
    Feb 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    115

    Default

    Figured I'd chime back in with some more info and pics, small shaft chatter throughout, wider portion chatters 1st 10 inches.
    G50 1000
    No G96, S500 for shaft (slow IMO) S350 body (Eh) feeds are in IPM and God Knows WHy
    Machine is 1996 vintage so likely no okuma-esque anti-chatter, nothing in the programming manual.
    I agree with finish tools, would help us keep things tighter too, I'm going to get a copy of the program and modify it.

    Is there a way I guess to go G96=A
    A= a number between lets say 400 and 500 where once it gets to 500 it goes down to 400, and this shift takes X amount of seconds.

    https://i.imgur.com/tmdAD59.jpg

    https://i.imgur.com/Ai0XOG7.jpg

  13. #12
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,674
    Post Thanks / Like
    Likes (Given)
    1238
    Likes (Received)
    2618

    Default

    Quote Originally Posted by Hardened View Post
    Is there a way to simulate the toggling from a programming perspective, akin to having it ride some sine wave perhaps? I'm running it now and would love to fix this age old problem while sparing my hands.
    Okuma does that, it's not great result, I wouldn't use it to finish. But to answer your question YES of course you could long hand the code in segments that changes the RPM thus the frequency. But I don't thing that is the best solution.

    In post #4 you said you are running it, but use words like "likely" and "wouldn't be surprised" what is it? If your use 450 RPM at 5" diameter in 304 thats 588 SFM a wee bit fast. At 1.25" it's 150 SFM, a little slow for Turning but hey?

    Are you using CSS or CRPM?

  14. #13
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,547
    Post Thanks / Like
    Likes (Given)
    5788
    Likes (Received)
    8173

    Default

    I have a face grooving job that likes to chatter if I allow it to. So I go a little bit and then change the RPM, and go some more, and then change back. Not a nice canned cycle, but git's the job done.


    If you told me that you was having issues with chatter on the 5" portion - I would understand (BTDT) but I haven't had issues on the stub ends like you are.

    ???

    --------------------

    Think Snow Eh!
    Ox

  15. Likes mikiemus liked this post
  16. #14
    Join Date
    Sep 2012
    Country
    SWEDEN
    Posts
    65
    Post Thanks / Like
    Likes (Given)
    22
    Likes (Received)
    16

    Default

    Doing a cut with right angle of cutting... 87, 83, 75, 63 degree angle of cuttingtool is one thing. do the right cuttingspeed is one thing. Make variable cuttingspeed to avoid shatter is a pain in the butt, but doable in a machine that has not that option. G1 some or part of inch and change speed during that distance, change it on the next distance.. etc. (yes programming pain in the butt) Everything pends on how many parts you want to do, in what of machine. If you can not do scrap parts for test, your in the cloud and grey zone. Use your scrap parts to learn from it, and do small steps at the time. Smaller dia and your ok, works on the greater. Have patience sacrifice some time and try it out. Smaller cutting dia speed and cutdepth.. use to be the treat. Milling or Turning.
    Cheers

  17. #15
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,674
    Post Thanks / Like
    Likes (Given)
    1238
    Likes (Received)
    2618

    Default

    Quote Originally Posted by mikiemus View Post
    Doing a cut with right angle of cutting... 87, 83, 75, 63 degree angle of cuttingtool is one thing.

    What do you mean by that? (This is a Turning)

  18. #16
    Join Date
    Sep 2012
    Country
    SWEDEN
    Posts
    65
    Post Thanks / Like
    Likes (Given)
    22
    Likes (Received)
    16

    Default

    Quote Originally Posted by litlerob1 View Post
    What do you mean by that? (This is a Turning)
    The angle the edge is positioned towards the cutting. A 87 is 3° rake (I think its called)
    Usually a standard VBMT, DNMG has 3-5°, but there is those others aswell.
    Why different angles? If you can get 100% of the cutting load axial then the radial force is minimal, and shatter minimal.

    Long bars use to climb up on the cutting edge and get out of Y pos, = shatter.
    If nothing works at all, and your workpiece is a straight bar, try a piece of plastic or similar
    above the cuttingtool, pressing slightly downwards on the bar preventing the bar from climbing.

  19. Likes sinha liked this post
  20. #17
    Join Date
    Dec 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    211
    Post Thanks / Like
    Likes (Given)
    355
    Likes (Received)
    86

    Default

    Sometimes when working on shaft work near the center end it is helpful to cut towards the center so it is loading positively instead of towards the chuck possibly bowing and unloading your center support.

  21. #18
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,547
    Post Thanks / Like
    Likes (Given)
    5788
    Likes (Received)
    8173

    Default

    Quote Originally Posted by mikiemus View Post
    If nothing works at all, and your workpiece is a straight bar, try a piece of plastic or similar
    above the cuttingtool, pressing slightly downwards on the bar preventing the bar from climbing.

    Could be a mounting challenge, but that is a simple follow rest eh?


    ---------------------

    Think Snow Eh!
    Ox


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
  •