Boring Issues
Close
Login to Your Account
Results 1 to 19 of 19

Thread: Boring Issues

  1. #1
    Join Date
    Jun 2020
    Country
    CANADA
    State/Province
    Ontario
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    2

    Angry Boring Issues

    Hey folks. I'm pretty new to machining in general so go easy on me, but I have an issue with chatter/lousy finish on these parts that I'm trying to bore, figured maybe you guys might see something that I'm missing.

    I'm running a Mori Seiki NLX2500, trying to bore a 42mm hole about 9 1/2" deep into M2, and the finish has to be good enough for a slip fit to go with another part I already finished. I'm using a 14" indexable boring bar, choked up as tight as I can get, with a 1 1/4" diameter. Currently set to a feed of 0.003ipr, 80CSS, and cut depth is about 0.005".

    The problem I'm having is that aside from being as loud as all hell, my finish is like sandpaper. I also can't get a consistent cut. I'll measure it, see that I need to take off another 0.010", adjust for that with tool wear, take a cut and measure again only to find out that I only took off 0.002".

    I've tried rubber bands on the part, masking tape on the boring bar, electrical tape on the boring bar, electrical tape and a shim, and I even tried swearing at it, but nothing I do seems to affect it. Any ideas of what I'm missing?

  2. #2
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,668
    Post Thanks / Like
    Likes (Given)
    690
    Likes (Received)
    1038

    Default

    What kind of insert and geometry?

  3. #3
    Join Date
    Jun 2020
    Country
    CANADA
    State/Province
    Ontario
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    2

    Default

    CCMT3251HQ inserts.

  4. #4
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,668
    Post Thanks / Like
    Likes (Given)
    690
    Likes (Received)
    1038

    Default

    CCMT3251HQ inserts.
    Kyocera makes a PCD insert in CCMT but they run about $150 each. Your bars out there almost 8 times diameter and M2 is like machining sandpaper in the first place. The speed and feed look fine for the insert you have now it's just the rigidity on the bar,, IMO. I would bet the only way you're really gonna get a good finish is to go with a ceramic insert and get a load off of the bar. 6% tungsten and 4% chrome would be hell on tools.

  5. Likes NeedForFeed liked this post
  6. #5
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    23
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    14

    Default

    With steel boring bars a 3 to 1 length to diameter ratio is basically the end of trouble free boring, in your case 3.75"

    Options beyond 3 to 1 are heavy metal, carbide bars, and de-vibe bars. Your length to diameter ratio is 7.6 which puts you into the expensive boring bar range.
    If you want to bore that deep consistently and often, de-vibe bars are awesome, especially with interchangeable heads for different deep hole applications.

    Some other points to consider are tool nose radius and depth of cut. You want to use the smallest tool nose radius possible boring to limit tool pressure, also taking less than the tool nose radius for depth of cut will often result in poor surface finish especially in steel. If the part tolerance/finish allows it could you bore from each end halfway? Boring is fickle and depends on so many factors that an image of the application would make suggestions easier.

  7. Likes ChipSplitter, NeedForFeed, Bobw liked this post
  8. #6
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,668
    Post Thanks / Like
    Likes (Given)
    690
    Likes (Received)
    1038

    Default

    Not sure how big your shop is and how much deep boring you do but as Octane said, the Tunable De vibe bars are the best for length to diameter ratios. And the fact you can have a multitude of heads for different geometries and rakes is a plus.

    This vid is pretty slick going 14Xd with a nickel balanced on the bar.

    YouTube

  9. Likes OCTANE WORKHOLD, NeedForFeed liked this post
  10. #7
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,404
    Post Thanks / Like
    Likes (Given)
    387
    Likes (Received)
    629

    Default

    Quote Originally Posted by OCTANE WORKHOLD View Post
    With steel boring bars a 3 to 1 length to diameter ratio is basically the end of trouble free boring, in your case 3.75"

    Options beyond 3 to 1 are heavy metal, carbide bars, and de-vibe bars. Your length to diameter ratio is 7.6 which puts you into the expensive boring bar range.
    If you want to bore that deep consistently and often, de-vibe bars are awesome, especially with interchangeable heads for different deep hole applications.

    Some other points to consider are tool nose radius and depth of cut. You want to use the smallest tool nose radius possible boring to limit tool pressure, also taking less than the tool nose radius for depth of cut will often result in poor surface finish especially in steel. If the part tolerance/finish allows it could you bore from each end halfway? Boring is fickle and depends on so many factors that an image of the application would make suggestions easier.
    Big deal, right there.

    You're running a .015 radius and going .005 deep.
    You will get chatter with that combination.

    Go with a CCMT3250.5 insert which has an .008 rad.
    Also get a super-finishing chipbreaker to eliminate as much defection as possible.
    I would start at .01" DOC and .0025 IPR and see what it does.

    And as mentioned, you are in de-vibe bar territory.

  11. Likes NeedForFeed liked this post
  12. #8
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,270
    Post Thanks / Like
    Likes (Given)
    963
    Likes (Received)
    4036

    Default

    Recommended feeds and speeds are just a starting point, when I see chatter on a bore first thing I try is increasing the feed and lowering the RPM. If I have a taper I will also program a taper in the opposite direction to straighten it out.

  13. Likes NeedForFeed liked this post
  14. #9
    Join Date
    Sep 2006
    Location
    SW Wisconsin
    Posts
    567
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    152

    Default

    I have had better luck using D or even T series inserts. More back clearance seems to help. It looks like a reamer job to me.

    Ed.

  15. Likes NeedForFeed liked this post
  16. #10
    Join Date
    Jun 2020
    Country
    CANADA
    State/Province
    Ontario
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    2

    Default

    Quote Originally Posted by OCTANE WORKHOLD View Post
    With steel boring bars a 3 to 1 length to diameter ratio is basically the end of trouble free boring, in your case 3.75"

    Options beyond 3 to 1 are heavy metal, carbide bars, and de-vibe bars. Your length to diameter ratio is 7.6 which puts you into the expensive boring bar range.
    If you want to bore that deep consistently and often, de-vibe bars are awesome, especially with interchangeable heads for different deep hole applications.

    Some other points to consider are tool nose radius and depth of cut. You want to use the smallest tool nose radius possible boring to limit tool pressure, also taking less than the tool nose radius for depth of cut will often result in poor surface finish especially in steel. If the part tolerance/finish allows it could you bore from each end halfway? Boring is fickle and depends on so many factors that an image of the application would make suggestions easier.
    I wish I had a devibe bar, but I doubt my boss will spring for a $4000 bar considering we just bought this one for this job. I just switched inserts to one with a smaller rad and am running it again, so fingers crossed that might help. Unfortunately due to the design of the workpiece, I cannot bore from both sides. Also unfortunately I have no immediate way to post a picture for you guys to see the setup. I might be able to figure something out in that regard tomorrow.

  17. #11
    Join Date
    Jun 2020
    Country
    CANADA
    State/Province
    Ontario
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    2

    Default

    Quote Originally Posted by atex57 View Post
    I have had better luck using D or even T series inserts. More back clearance seems to help. It looks like a reamer job to me.

    Ed.
    I only have 2 bars long enough for this bore and they both take the same inserts. I did try a reamer, but it dulled so quickly that each successive part I made had a smaller hole than the last and then on part #9 it actually snapped the reamer right in half and we had to use a press to extract it.

  18. #12
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    23
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    14

    Default

    Some applications like this, such as trying to bore 9.500 deep with a steel bar is akin to trying to write with one hand using a 3 foot pencil. You have a job to finish though so small insert radius, try spindle speed variation if your machine can do that, if not ride the speed control up and down to pulse and break the harmonic wave. Try taking a large DOC for the finish pass instead of small. Make sure you are using a split block holder gripping at least 4 x d of the shank with circular full contact. There is no silver bullet for boring other then building the cost of a de-vibe bar into your quote, or not accepting deep boring jobs.

  19. #13
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    11,622
    Post Thanks / Like
    Likes (Given)
    3968
    Likes (Received)
    4132

    Default

    Some times there is not proper clearance and the bar has to twist a bit to get the edge to touch the part.
    A look at the heal with a loop can sometimes tell if this is a problem.

    Holding the boring bar insert to a 1 5/8 hole and eyeball look might tell if clearance is good.

  20. #14
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,260
    Post Thanks / Like
    Likes (Given)
    14977
    Likes (Received)
    11097

    Default

    Some other points to consider are tool nose radius and depth of cut.

    Quote Originally Posted by ChipSplitter View Post
    Big deal, right there.

    You're running a .015 radius and going .005 deep.
    You will get chatter with that combination.

    Go with a CCMT3250.5 insert which has an .008 rad.
    Also get a super-finishing chipbreaker to eliminate as much defection as possible.
    I would start at .01" DOC and .0025 IPR and see what it does.

    And as mentioned, you are in de-vibe bar territory.

    My theory on deep-ish boring is to take a fairly large cut. Low feed,
    noseR * 1.5 or 2 depth. Then a lot of your cutting force is being
    directed back up the length of your boring bar, a direction that it
    is fairly stiff. Like a column at the parthenon.

    Kind of like "high feed" milling cutters.

    With a low DOC, you are effectively only pushing your bar sideways.
    Effectively turning it into a giant tuning fork.

    A smaller nose rad never hurts either, then you can run an even smaller
    DOC. And/Or get more of the total forces going straight down the bar
    instead of sideways.


    I don't know if my theory is correct or not, but its kept me out
    of too much trouble so far.

  21. Likes ChipSplitter, Bill in PA liked this post
  22. #15
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,404
    Post Thanks / Like
    Likes (Given)
    387
    Likes (Received)
    629

    Default

    Quote Originally Posted by Bobw View Post
    My theory on deep-ish boring is to take a fairly large cut. Low feed,
    noseR * 1.5 or 2 depth. Then a lot of your cutting force is being
    directed back up the length of your boring bar, a direction that it
    is fairly stiff. Like a column at the parthenon.

    Kind of like "high feed" milling cutters.

    With a low DOC, you are effectively only pushing your bar sideways.
    Effectively turning it into a giant tuning fork.

    A smaller nose rad never hurts either, then you can run an even smaller
    DOC. And/Or get more of the total forces going straight down the bar
    instead of sideways.


    I don't know if my theory is correct or not, but its kept me out
    of too much trouble so far.

    Yep, I agree 100% Bob.

    I will also say that tweaking the DOC as well as the bar stickout can make a big difference in harmonics.

    (Sliding the bar out 1/4" or changing the DOC by .003".)

  23. Likes Bobw liked this post
  24. #16
    Join Date
    Jun 2020
    Country
    CANADA
    State/Province
    Ontario
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    2

    Default

    Thanks for all the replies guys. I'll keep these suggestions in mind the next time my machine is making whale-calls. I changed the insert and adjusted the DOC, and that seems to have taken care of like 90% of the noise, and though my finish isn't as perfect as I would like, it's a world of difference from what I WAS getting, and it'll be enough to get the job done. I've got another part to slip-fit in there, so it won't be visible anyway, it just has to get in.

    Unfortunately due to the size of our shop, we don't have all the fancy tools and sometimes have to make do with what we have, so no de-vibes or split-block holders, and like I said: I'm pretty new to machining in general, even more so CNC lathe programming, so I really do appreciate all the advice.

    -Jordan

  25. Likes Mtndew, Bobw liked this post
  26. #17
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,196
    Post Thanks / Like
    Likes (Given)
    4770
    Likes (Received)
    3145

    Default

    Quote Originally Posted by NeedForFeed View Post
    Unfortunately due to the size of our shop, we don't have all the fancy tools and sometimes have to make do with what we have, so no de-vibes
    Yeah this makes it tough when you're unable to use the right tool for the job.
    But challenges also give experience and make you better.

  27. Likes Bobw, NeedForFeed liked this post
  28. #18
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,404
    Post Thanks / Like
    Likes (Given)
    387
    Likes (Received)
    629

    Default

    I get a kick out of this thread title.

    Yeah, I have mundane problems too................

  29. Likes NeedForFeed, Bobw liked this post
  30. #19
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,633
    Post Thanks / Like
    Likes (Given)
    1208
    Likes (Received)
    672

    Default

    Quote Originally Posted by NeedForFeed View Post
    and I even tried swearing at it, but nothing I do seems to affect it. Any ideas of what I'm missing?
    Did your boss maybe buy foreign material? Sometimes I find that swearing does work as long as the material speaks the same language

    Great suggestions here already from all. I will just add that for something like that you can try to rough out material with a shorter bar to get some it out. And then go to the longer one to rough the rest and finish it up. Could help to get it a bit more consistent.

  31. Likes g-coder05 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
  •