Threading burr problem
Close
Login to Your Account
Results 1 to 14 of 14
  1. #1
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    527
    Likes (Received)
    505

    Post

    Good morning all,
    I have a problem with the last thread of a part being rolled over, creating a burr. Bad, Bad. This is a conical shaped thread, starting at 6.60 mm and cutting down at a 10 degree angle. It is a double lead thread. The last thread rolls over creating a rather heavy burr. Part of the process uses a rotating wire brush to help de-burr, but it does not really work well. These parts cannot be touched by hand, it is a completely automated process. This is 316L medical grade stainless steel. I am using a G92 threading cycle on a Fanuc 21i-T control.
    Here is a sample of code.
    G92X5.50Z-5.R1.058F1.
    X5.45
    X5.35
    X5.25
    X5.15
    X5.05
    X5.00
    X4.95
    X4.92
    X4.90
    X4.90
    G0X10.Z1.5
    G92X5.50Z-5.R1.146F1.
    X5.45
    X5.35
    X5.25
    X5.15
    X5.05
    X5.00
    X4.95
    X4.92
    X4.90
    X4.90
    G0Z20.M9
    G28U0W0M5
    These parts need to fit a transparency after threading and the burr causes them to not fit. Will a G76 cycle help eliminate this burr? Can this burr be eliminated sufficiently without hand work (not possible). I need to find a way to eliminate or reduce the amount of rollover on the last thread. These are bone screws and any hanging material as such can come off in the body. Really not a good thing. I really appreciate the help I might get from all of you capable and experienced pro's out there

    Thanks, Paul

  2. #2
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,922
    Post Thanks / Like
    Likes (Given)
    342
    Likes (Received)
    1941

    Post

    Paul

    Burrs on threads are one of the facts of life. With special threads with no thread form inserts it's even more common.
    What I do is finish the OD, thread to depth in one G92 cycle. Then do another pass on the complete OD again and then another G92 cycle, but this time a few tenths above the finished thread dia.
    It still doesn't completely remove the burrs, but thins them out to a point where a simple scotchbrite takes them off.
    Sure, it adds machining time, but that's just another fact of life. Consider the time it takes to hand-deburr and compare it to the added cycle time.

    If this is on a Fanuc then you must use G92 as Fanucs do not follow the same pattern for G76 and G92. HAAS does, so you can do the initial threading with G76 and then use G92 with different X dia. passes. The reason you want to use G92 as the springpass is that you have exact control of each X diameter, which you will have to experiment with to get things tweaked just right.

  3. #3
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    527
    Likes (Received)
    505

    Post

    SeymourDumore,
    Thanks bunches for your input. We are at the moment doing what you suggest, turn-thread-turn-thread again. Cycle time really isn't the issue. This is an automated process. Pallet that holds 250 parts, 2 lathes and a Denso robot to load and unload. No manual intervention alowwed as far as deburring is concerned. We make over 3 million of these a year so you might understand why. I thought a G76 cycle would at least minimize the burr problem. Thanks a lot again.

    Paul

  4. #4
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Post

    Paul,

    Is there any kind of undercut behind the threads? If so, recut the undercut after threadding. If not, try passing your turn tool across the thread about .00005 under the diameter. Still in 316, that burr my still be there, just tiny. Can you tumble the screws?

  5. #5
    Join Date
    May 2006
    Location
    Illinois
    Posts
    964
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Post

    Paul,

    If the burr is really more of the last thread rolling over then cutting the double lead by alternating passes between the first and second lead will help.

    I haven't worked on a 21i in a while but I think you can use a "Q" value to simplify programming. I'm sure you can on the 30/31/32i and I'm pretty sure you can on the 21i.

    Q is the shift amount for the start angle. So it would look like this:

    G92X5.50Z-5.R1.058 Q0 F1.
    X5.5 Q180.
    X5.45 Q0
    X5.45 Q180.
    X5.35 Q0
    X5.35 Q180.
    X5.25 Q0
    X5.25 Q180.
    X5.15 Q0
    X5.15 Q180.
    X5.05 Q0
    X5.05 Q180.
    X5.00 Q0
    X5.00 Q180.
    X4.95 Q0
    X4.95 Q180.
    X4.92 Q0
    X4.92 Q180.
    X4.90 Q0
    X4.90 Q180.

    Anyway, by alternating leads you reduce the pressure on the second lead which reduces the chance of the last thread rolling over due to tool pressure.

  6. #6
    Join Date
    May 2006
    Location
    Illinois
    Posts
    964
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Post

    If this is on a Fanuc then you must use G92 as Fanucs do not follow the same pattern for G76 and G92.
    Sure it does. Just set your included tool tip angle to 0, then G92 and G76 will cut in the same pattern.

    But why not just use G76 for the deburring pass? On the second go-round just set the depth of the first pass to the depth of the thread or set the min DOC to the whole depth of the thread. Oh and set the number of finishing passes to zero. Then G76 will take just one deburring pass.

    In any case I prefer to take alternate passes on double lead threads, unless it's a really stout Acme thread.

  7. #7
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    26,060
    Post Thanks / Like
    Likes (Given)
    6355
    Likes (Received)
    8521

    Post

    I am also assuming that your burr that your talking aboot is a departure burr heading into an [aleady made] undercut at the bottom of the thread?

    Hows aboot making the thread, cut your undercut, and then run your deburr threading sequence?

    OR - another option being - can you infeed the other direction? Instead of feeding in towards the part each time (compound here) can a feller infeed the other way so that you are only pushing on the blowout side the first pass? This is likely something in another routine other than G76? Or maybe a perameter that could be switched?

    One thing tho - are 3,000,000 bone screws used in a yrs time in the whole werld? And to think that there are plenty of others making them too....

    That said - if you make 3,000,000 of these a yr - I would like to think that you've gott'r fingered out by now eh?


    Sweatin' to the Oldies!
    Ox

  8. #8
    Join Date
    May 2006
    Location
    Illinois
    Posts
    964
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Post

    Heh, I missed the bone screw part.

    Why not thread whirl them on a Swiss? I've done double start bone screws by whirling before. Although without seeing the print, it's hard to say for sure.

  9. Likes TeachMePlease liked this post
  10. #9
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,878
    Post Thanks / Like
    Likes (Given)
    3640
    Likes (Received)
    3035

    Post

    What's the going price for a bone screw at the manufacturer level? Not that I'm interested in making any, BTW. A few years back my son had knee surgery to repair a torn ACL. The surgeon used a staple that looked about the size of a standard romex staple, but with a bunch of barbs on it. Probably worth about the same at the shop level as a bone screw, but at the hospital level it sold for 190 bucks over 10yrs ago.

    When it was removed once the ligament was reattached, my son told the surgeon he'd like to have it as a souvenir. He finishes up and comes out into the waiting area to tell me and my wife everything's okay. He slips a little pill bottle containing the staple to Karen and tells her to put it in her purse discreetly. Seems hospital policy dictates that anything removed from a human body is to be sent to pathology for identification. So, as the Doc said, no only do they charge you damn near $200 for the staple, but when it goes back to path after removal they'll charge you another $150 to tell you it was a staple. What a racket !!

  11. #10
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,922
    Post Thanks / Like
    Likes (Given)
    342
    Likes (Received)
    1941

    Post

    Swiss

    Have never tried that as I always use the A word during threading. Will check it out though.

    And the reason for the G92 during the spring passes is that you can explicitly define the diameters for each pass. For nasty stuff like Inco, or thin walled parts with threads I sometimes get chatter caused not by high SFM but rather the nature of the part. What I do is do spring passes at alternating depths, and the very last or even last two passes are done at .0002-.0005 above the minor/major. It really works nice and can be tweaked until just perfect. That is not possible with G76.

    Here is an example of a 1 1/1-12 UNJ thread on one of those parts:

    (THREADING)
    G54
    G50 S900
    G00 G97 T404 S500 M03
    G00 X1.066 Z0.05 M08
    G76 D0.011 A60 F0.0833 X0.9616 K0.0476 Z-0.57
    G80
    T404
    G00 X1.066 Z0.05 M08
    G97 S500 M03
    G92 X0.9616 Z-0.57 F0.0833
    X0.9616
    X0.9612
    X0.9612
    G80
    M09
    M05
    G28

    Again, this runs just dandy on the HAAS while the Fanuc plows right through the middle of the thread.
    Will check it without the A60 in the G76 line though.

  12. #11
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    527
    Likes (Received)
    505

    Post

    Hello All,
    Thanks for everyones input. Most of these ideas have been tried and I appreciate everyones help. The real problem is that there is no manual deburring allowed after machining. If the part does not fit between the lines on the transparency, it is scrap. We have had this problem on and off since we started these parts. Quality says that if it is a thick enough burr that it will not come off, then it is not a burr. But, we have inspectors that create their own opinions of what is good or bad. Hence, a lot of paper work. So, we constantly revisit this. I was hoping a different pattern of cutting such as a G76, which we haven't tried yet, would make it thin enough that a wire brush would remove it.

    Yes, there is an undercut, but it is made in a previous operation, I can't revisit it.

    3 million bone screws is not a lot for us, this is just this one family. We make over 6 million a year of diferent varieties, even big ones for large animals. The shaft thread is whirled on a whirling machine. This thread is on a conical shaped head that locks into a plate after insertion, pulls the bone fragments together better for better healing. As for price, we make them for about $3 a pop. How's that for markup? [img]smile.gif[/img]
    I will try a couple of these other ideas and thanks again for all your ideas.

    Paul

  13. #12
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,922
    Post Thanks / Like
    Likes (Given)
    342
    Likes (Received)
    1941

    Post

    Locknut

    That sucks.
    How'bout a really stupid sounding, but possibly workable idea.
    Take a toolholder, or make one and use a piece of a soft deburring wheel to mount in it.
    Take it and do a couple of threading passes over the OD. Maybe that'll take the little boogers off.

    Before anyone else thinks I'm dumb ass, I have seen it done. Not with threads but with radial bearing balls that had an oil groove plunged into it. They finished the OD, plunged the groove with a profile tool and then plunged a piece of 3M deburring wheel mounted into an SNMG holder. A tiny wiggle of .05 back and forth on the Z and the thing came out cat's ass.

  14. #13
    Join Date
    Oct 2018
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Best thread burr fix

    Quote Originally Posted by LockNut View Post
    Good morning all,
    I have a problem with the last thread of a part being rolled over, creating a burr. Bad, Bad. This is a conical shaped thread, starting at 6.60 mm and cutting down at a 10 degree angle. It is a double lead thread. The last thread rolls over creating a rather heavy burr. Part of the process uses a rotating wire brush to help de-burr, but it does not really work well. These parts cannot be touched by hand, it is a completely automated process. This is 316L medical grade stainless steel. I am using a G92 threading cycle on a Fanuc 21i-T control.
    Here is a sample of code.
    G92X5.50Z-5.R1.058F1.
    X5.45
    X5.35
    X5.25
    X5.15
    X5.05
    X5.00
    X4.95
    X4.92
    X4.90
    X4.90
    G0X10.Z1.5
    G92X5.50Z-5.R1.146F1.
    X5.45
    X5.35
    X5.25
    X5.15
    X5.05
    X5.00
    X4.95
    X4.92
    X4.90
    X4.90
    G0Z20.M9
    G28U0W0M5
    These parts need to fit a transparency after threading and the burr causes them to not fit. Will a G76 cycle help eliminate this burr? Can this burr be eliminated sufficiently without hand work (not possible). I need to find a way to eliminate or reduce the amount of rollover on the last thread. These are bone screws and any hanging material as such can come off in the body. Really not a good thing. I really appreciate the help I might get from all of you capable and experienced pro's out there

    Thanks, Paul
    Old thread but figured I would post what I do. I use the threading insert to make the thread relief. Feeding it in at a 30 degree angle to turn the back side relief. Then I will take one final finish pass on the thread profile -.0005" from the last pass. The goal is to not cut anymore threads after the relief is cut rather fix any damaged threads from the cutting of the thread relief. One thing I forgot to mention is that I will also use a alternating threading cycle that cuts with the front side then switches to the backside of the insert per pass. Then after the relief is cut I go in with a grooving tool to square up the back of the relief.

    Thanks,
    EJ

  15. #14
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    3,315
    Post Thanks / Like
    Likes (Given)
    11430
    Likes (Received)
    3713

    Default

    Quote Originally Posted by LockNut View Post
    Quality says that if it is a thick enough burr that it will not come off, then it is not a burr.

    As someone who does the same type of products:

    JFC NO.


    Edit: Didn't realize this was a 13 year old necro thread.

    The sentiment remains the same.


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
  •