OD groove out of round
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 27
  1. #1
    Join Date
    Feb 2021
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default OD groove out of round

    Hey everyone.

    I'm machining 420SS on my 1994 mazak qt15n. The part OD is 1.5" and groove OD is 1.257" (+-.001). The groove is about .8" in front of my jaws.

    The groove is measuring 1.256 one way and 1.258 measuring 90 degrees from the previous.

    I'm using a kennametal top notch NG3189-K 5010 tool. The groove width is .189", so I'm going full width and depth no peck. I'm running 500 sfm at .008" feed/rev. Reducing to .006" feed/rev didn't seem to help. I'm using those feeds and speeds because the finish is good with no chatter.

    Every once in a while it seems like i get a part that is within .001" round. I'm not sure where to go from here.

    Any thoughts?

    -Tyler

  2. #2
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,321
    Post Thanks / Like
    Likes (Given)
    13573
    Likes (Received)
    5152

    Default

    You give it a dwell at the bottom of the groove, for at least a couple revolutions?

  3. #3
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,869
    Post Thanks / Like
    Likes (Given)
    689
    Likes (Received)
    1147

    Default

    Quote Originally Posted by TeachMePlease View Post
    You give it a dwell at the bottom of the groove, for at least a couple revolutions?
    You are absolutely correct. Seen this may times. It is a parameter setting. I don't recall if that early of the Mazak controls have a TPC setting or not. If so, that is where I would make the adjustment.

  4. Likes kevin66 liked this post
  5. #4
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,079
    Post Thanks / Like
    Likes (Given)
    3964
    Likes (Received)
    795

    Default

    Quote Originally Posted by tsabo View Post
    Hey everyone.

    I'm machining 420SS on my 1994 mazak qt15n. The part OD is 1.5" and groove OD is 1.257" (+-.001). The groove is about .8" in front of my jaws.

    The groove is measuring 1.256 one way and 1.258 measuring 90 degrees from the previous.

    I'm using a kennametal top notch NG3189-K 5010 tool. The groove width is .189", so I'm going full width and depth no peck. I'm running 500 sfm at .008" feed/rev. Reducing to .006" feed/rev didn't seem to help. I'm using those feeds and speeds because the finish is good with no chatter.

    Every once in a while it seems like i get a part that is within .001" round. I'm not sure where to go from here.

    Any thoughts?

    -Tyler
    Allow material for a finish pass. Also if you are having problems allow a additional finish pass and check it before finishing. Too whenever you cut corners on processes this is what happens. Many people will also back off the rough and finish and check concentricity preventing scrap. Checking accuracy properly will generally prevent scrapping a first part if one wishes to be careful.

  6. #5
    Join Date
    Feb 2021
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    It's a T32B control. I have a TPS button, but I don't think that is what you are meaning.

    I did a quick search and it looks like parameter p24 is dwelling at the end of a groove. Mine is set for 3 revs.

  7. #6
    Join Date
    Feb 2021
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Trueturning,

    I just tested out a part with a finishing and semi finishing pass. I'm leaving .020" (diameter) on each pass and slowed the feed down to .004"/rev. I am measuring about .0009" to .0011" difference now. Definitely an improvement, but still a wide range.

    Would you leave less on the finishing passes? The groove bottom looks to have very slight chatter marks now.

  8. #7
    Join Date
    Oct 2005
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    21,690
    Post Thanks / Like

    Default

    Quote Originally Posted by tsabo View Post
    Trueturning,

    I just tested out a part with a finishing and semi finishing pass. I'm leaving .020" (diameter) on each pass and slowed the feed down to .004"/rev. I am measuring about .0009" to .0011" difference now. Definitely an improvement, but still a wide range.

    Would you leave less on the finishing passes? The groove bottom looks to have very slight chatter marks now.
    I'm wondering if you work hardened it on the roughing pass.

  9. #8
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    59
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    5

    Default

    Try running two passes, but leave nothing for the second, like a spring pass on a small boring bar. If your not getting chatter add a couple more spins to the dwell.

  10. #9
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    59
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    5

    Default

    I see you are getting chatter. cancel that last thought.

  11. #10
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,869
    Post Thanks / Like
    Likes (Given)
    689
    Likes (Received)
    1147

    Default

    Quote Originally Posted by tsabo View Post
    It's a T32B control. I have a TPS button, but I don't think that is what you are meaning.

    I did a quick search and it looks like parameter p24 is dwelling at the end of a groove. Mine is set for 3 revs.
    Sorry, I meant TPC not TPS. TPC=temporary parameter change. Using this, you can set how many rotations the tool dwells at the bottom of the groove. Sometimes just slowing down your feed rate will solve the problem, but it may initiate chatter.

  12. Likes Trueturning liked this post
  13. #11
    Join Date
    Feb 2021
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Yes. The chatter is very slight. I figure the dwells would be almost like spring passes anyways.

    digger doug - I figured my roughing feed was high enough to get in and out quick without work hardening, but the sfm might be a tad high. I could be doing it wrong, too, as I never turned 420ss and don't have a whole lot of lathe experience. This is my first time grooving.

  14. #12
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,869
    Post Thanks / Like
    Likes (Given)
    689
    Likes (Received)
    1147

    Default

    Quote Originally Posted by Gobo View Post
    Sorry, I meant TPC not TPS. TPC=temporary parameter change. Using this, you can set how many rotations the tool dwells at the bottom of the groove. Sometimes just slowing down your feed rate will solve the problem, but it may initiate chatter.
    Now I see you have your dwell set at 3 revolutions. That should be okay. Any more and you will probably get worse chatter.

  15. #13
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,458
    Post Thanks / Like
    Likes (Given)
    604
    Likes (Received)
    8481

    Default

    If one thinks about the machine making helix cut.
    If it pulls out too fast the helix of your infeed is the groove surface.
    So one needs a dwell or G04, sit there too long if a hard push and you get may get chatter.
    Why does that happen? Is the top or bottom of the chatter size to the machine and tool?
    The same run problem occurs when making center holes. Bing bang, done and then.....downstream.
    .006 per rev with a instant machine pullout should leave you out of round a lot as in .006. Think about it.
    Bob

  16. #14
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    166
    Post Thanks / Like
    Likes (Given)
    179
    Likes (Received)
    88

    Default

    I would check a finished part with a test indicator before removing it from the jaws.If its too short of a dwell it will show up pretty easy.

  17. #15
    Join Date
    Feb 2021
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Quote Originally Posted by digger doug View Post
    I'm wondering if you work hardened it on the roughing pass.
    I forgot that I was testing grooves on a piece of steel before trying the 420ss. I went and checked those grooves for roundness and measured .001"-.002" out just like I'm getting on this stainless. I think it's more than a work hardening issue.

  18. Likes digger doug liked this post
  19. #16
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    1,285
    Post Thanks / Like
    Likes (Given)
    112
    Likes (Received)
    519

    Default

    Quote Originally Posted by tsabo View Post
    Hey everyone.

    I'm machining 420SS on my 1994 mazak qt15n. The part OD is 1.5" and groove OD is 1.257" (+-.001). The groove is about .8" in front of my jaws.

    The groove is measuring 1.256 one way and 1.258 measuring 90 degrees from the previous.

    I'm using a kennametal top notch NG3189-K 5010 tool. The groove width is .189", so I'm going full width and depth no peck. I'm running 500 sfm at .008" feed/rev. Reducing to .006" feed/rev didn't seem to help. I'm using those feeds and speeds because the finish is good with no chatter.

    Every once in a while it seems like i get a part that is within .001" round. I'm not sure where to go from here.

    Any thoughts?

    -Tyler
    A host of things could be causing this. these are the obvious, and most often over looked.
    1st jaw pressure and are your jaws Cut round? if you dont use a round spinder your jaws wont cut round did you check the jaws with an indicator.

  20. #17
    Join Date
    Feb 2021
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Quote Originally Posted by Delw View Post
    A host of things could be causing this. these are the obvious, and most often over looked.
    1st jaw pressure and are your jaws Cut round? if you dont use a round spinder your jaws wont cut round did you check the jaws with an indicator.
    I am using hard jaws. I'm feeding a 1 ft bar through the spindle. The bar fits the liner good. I've tried 175-300 psi on the chuck pressure. This is a 1st op.

    The OD of the part is measuring round and so is the stepped feature at the front of the part.

  21. #18
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,869
    Post Thanks / Like
    Likes (Given)
    689
    Likes (Received)
    1147

    Default

    Mazatrol program?

  22. #19
    Join Date
    Feb 2021
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    11
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    2

    Default

    Quote Originally Posted by Gobo View Post
    Mazatrol program?
    Yes mazatrol program.

  23. #20
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,869
    Post Thanks / Like
    Likes (Given)
    689
    Likes (Received)
    1147

    Default

    Are you using a "0" grooving cycle? I am not sure if it dwells with a 0 cycle. Put a really crazy number in your dwell parameter and see if it does dwell. If not, you will have to use a "1" cycle or write a Mazatrol manual unit.

  24. Likes tsabo liked this post

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
  •