Guhring Mill / Drill Huge Issues with Breakage and Tool Life - Page 4
Close
Login to Your Account
Page 4 of 4 FirstFirst ... 234
Results 61 to 78 of 78
  1. #61
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    Quote Originally Posted by Milland View Post
    The quick breakers may be the ones with high eccentricity, that would wreck smaller cutters.

    Did you discuss going to a spot drill rather than using an endmill?

    Thanks for keeping us updated!
    Nachi is testing a flat bottom drill on our parts in their lab to do everything in one operation.

  2. #62
    Join Date
    Dec 2004
    Location
    uk
    Posts
    11,560
    Post Thanks / Like
    Likes (Given)
    2985
    Likes (Received)
    5006

    Default

    No disrespect, but a carbide drill with run out plunging into a shallow depression made by that milling cutter is going to snap randomy, its a tooling 101 do not ever do that level event. Its just a straight up piss poor thing to do. Above all ditch gurhing and call sandvick, watch there youtube videos and learn how you should use a drill bit!

    Use a std spot drill and it MUST be a shallower angle than the drill point and you will stabilise your tool life massively.

    Its a 2mm drill bit you don't need mega buck hydraulic holders, you don't need shrink fit, and you don't need a big plus spindle for this job. A humble ER16 collet setup will sort it and theres more than a few good American suppliers that can have you a holder there some point Monday for less than a $100!!! Speak to Maritool on here.

    Me i would ditch the carbide for now, buy a pack of screw length coated HSS cobalt and get a steady 200+ holes a bit all be it a bit slower, but tool life will be rock solid reliable. That means production will go up. They woun't give a toss about 5 thou spindle run out either if you don't chioke em up too tight in the collet (you want some length to flex till you fix that problem.)

  3. #63
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    Quote Originally Posted by adama View Post
    No disrespect, but a carbide drill with run out plunging into a shallow depression made by that milling cutter is going to snap randomy, its a tooling 101 do not ever do that level event. Its just a straight up piss poor thing to do. Above all ditch gurhing and call sandvick, watch there youtube videos and learn how you should use a drill bit!

    Use a std spot drill and it MUST be a shallower angle than the drill point and you will stabilise your tool life massively.

    Its a 2mm drill bit you don't need mega buck hydraulic holders, you don't need shrink fit, and you don't need a big plus spindle for this job. A humble ER16 collet setup will sort it and theres more than a few good American suppliers that can have you a holder there some point Monday for less than a $100!!! Speak to Maritool on here.

    Me i would ditch the carbide for now, buy a pack of screw length coated HSS cobalt and get a steady 200+ holes a bit all be it a bit slower, but tool life will be rock solid reliable. That means production will go up. They woun't give a toss about 5 thou spindle run out either if you don't chioke em up too tight in the collet (you want some length to flex till you fix that problem.)
    I take no disrespect to that at all. I didnt develop the process, I inherited it. I'm also brand new to machining at the speed we are. We are using carbide because these 3 machines are integrated directly into a large line that does grind/heat treat after those operations. The spot mill isnt plunging straight down into a flat surface. The plunge goes into a spline thats on a 30 degree angle.

  4. #64
    Join Date
    Dec 2006
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    23

  5. Likes f40lm liked this post
  6. #65
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    441
    Post Thanks / Like
    Likes (Given)
    282
    Likes (Received)
    160

    Default

    Are you allowed to post a picture or sketch of the setup/part? Since it seems to be consistently-inconsistent across all your machines (even the one with .0005 runout) I doubt it's the machines (of course grinding your tapers won't hurt!). Can you post a pic of one that's been used but not broken yet if there seems to be anything worth sharing? Its just a hole....we should be able to figure this one out!

  7. Likes f40lm liked this post
  8. #66
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    Quote Originally Posted by Nerdlinger View Post
    Are you allowed to post a picture or sketch of the setup/part? Since it seems to be consistently-inconsistent across all your machines (even the one with .0005 runout) I doubt it's the machines (of course grinding your tapers won't hurt!). Can you post a pic of one that's been used but not broken yet if there seems to be anything worth sharing? Its just a hole....we should be able to figure this one out!
    I will PM you tomorrow.

  9. #67
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    Quote Originally Posted by Nerdlinger View Post
    Are you allowed to post a picture or sketch of the setup/part? Since it seems to be consistently-inconsistent across all your machines (even the one with .0005 runout) I doubt it's the machines (of course grinding your tapers won't hurt!). Can you post a pic of one that's been used but not broken yet if there seems to be anything worth sharing? Its just a hole....we should be able to figure this one out!
    PM'd with video of the operation.

  10. #68
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    441
    Post Thanks / Like
    Likes (Given)
    282
    Likes (Received)
    160

    Default

    Whatever happened with this??

  11. Likes Ox liked this post
  12. #69
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    Quote Originally Posted by Nerdlinger View Post
    Whatever happened with this??
    Tooling trials are next week. I have a Kennametal mill/drill setup. Nachi just came in today recommending a flat bottom drill for the pilot and then a deep hole drill to finish it off. They have 3 feeds on the deep hole drill because the issue they are seeing is due to the drill chipping. Since the entry and exit is at an angle the drill has been chipped prematurely. Slowing the entry, then speeding up, then slowing for exit has supposedly taken care of that. I'm very curious to see these results. They slowed down the deep hole drill to 50rpm during entry into the pilot so the runout doesnt break the tool instantly.

  13. #70
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    22,109
    Post Thanks / Like
    Likes (Given)
    2879
    Likes (Received)
    5796

    Default

    I'm guessing that the exiting out into the splines on the opposite side is the hardest on the drill.



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

    Think Snow Eh!
    Ox

  14. #71
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    Quote Originally Posted by Ox View Post
    I'm guessing that the exiting out into the splines on the opposite side is the hardest on the drill.



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

    Think Snow Eh!
    Ox
    I'm going to sample a program later this week. I ran the kennametals mill/drill set. Drill life was very low at 208 parts made (416 operations). The mill life appears to be great though. Before lunch I was sitting at 2,200 parts on one mill (4,400 operations). That is 300 parts off of our highest in the past few months and 500 parts over our best on that specific robodrill. We will see if it surpasses it. I am testing the remaining 4 mills/drill.

    I am going to sample a program recommended by Nachi which was pretty genius I thought. They are aware of our bad runout.

    Pilot mill Operation Untouched to Z-2.mm

    Drill Operation

    S50 F240. to Z-1. (Almost 0RPM to eliminate runout on drill entry)
    S15000 F711. to Z-11.5 (Once drill has entered part, increase RPM and feed)
    S5500 F51. to Z-14.0 (Slow RPM / Feed on exit last 2.5mm)

  15. #72
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    22,109
    Post Thanks / Like
    Likes (Given)
    2879
    Likes (Received)
    5796

    Default

    OH, so you are drilling to C/L and flipping it then.


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

    Think Snow Eh!
    Ox

  16. #73
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    3,676
    Post Thanks / Like
    Likes (Given)
    749
    Likes (Received)
    2405

    Default

    Quote Originally Posted by f40lm View Post

    I am going to sample a program recommended by Nachi which was pretty genius I thought. They are aware of our bad runout.
    I don't understand why you're not dealing with the runout first - that's the biggest reason for low tool life and unstable operation.

  17. #74
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    Quote Originally Posted by Milland View Post
    I don't understand why you're not dealing with the runout first - that's the biggest reason for low tool life and unstable operation.
    Agreed, but we need to prevent the runout from happening again first before investing in all new spindles. We are adding flood coolant and possibly changing the deburr brush material. The theory is the deburr brush sandpaper material is getting up into the spindle. It makes no sense to put in brand new spindles right now when in 6months they will just be wrecked again. We need to find the root cause of the runout, correct, then move forward with the spindle replacement.

  18. #75
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    22,109
    Post Thanks / Like
    Likes (Given)
    2879
    Likes (Received)
    5796

    Default

    Doo you have a (series of) sock filter(s) on your coolant line?

    What feature of the part are you "deburring" with abrasives?


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

    Think Snow Eh!
    Ox

  19. #76
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    We are still working out these issues, but I have done quite a few trials and Kennametal products have way better tool life for this line its just unbelievable. The pricing is better and we have seen a tool life increase by 70% on our end mills (currently running a 50 mill trial). We have only consumed 20 mills over 2.6 weeks and our usual consumption rate is 30 end mills per week.

    I trialed 5 of there drills, getting a lot of 50 in after the 1st. Tool life seems significantly better on these as well. It looks like we are on the way to a $100k+/yr cost savings with this option without even getting the process stabilized yet. That is the next step.

  20. Likes Ox, Blazemaster, doug925, Motorsports-X liked this post
  21. #77
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    2,934
    Post Thanks / Like
    Likes (Given)
    1118
    Likes (Received)
    590

    Default

    Quote Originally Posted by f40lm View Post
    We are still working out these issues, but I have done quite a few trials and Kennametal products have way better tool life for this line its just unbelievable. The pricing is better and we have seen a tool life increase by 70% on our end mills (currently running a 50 mill trial). We have only consumed 20 mills over 2.6 weeks and our usual consumption rate is 30 end mills per week.

    I trialed 5 of there drills, getting a lot of 50 in after the 1st. Tool life seems significantly better on these as well. It looks like we are on the way to a $100k+/yr cost savings with this option without even getting the process stabilized yet. That is the next step.
    That is excellent news! (it never hurts to have that in your pocket when you go for your annual review. LOL)
    Please keep this thread updated. We all love hearing success stories.

    Doug.

  22. #78
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    7,236
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1933

    Default

    Quote Originally Posted by f40lm View Post
    Tooling trials are next week. I have a Kennametal mill/drill setup. Nachi just came in today recommending a flat bottom drill for the pilot and then a deep hole drill to finish it off. They have 3 feeds on the deep hole drill because the issue they are seeing is due to the drill chipping. Since the entry and exit is at an angle the drill has been chipped prematurely. Slowing the entry, then speeding up, then slowing for exit has supposedly taken care of that. I'm very curious to see these results. They slowed down the deep hole drill to 50rpm during entry into the pilot so the runout doesnt break the tool instantly.
    .
    .
    1) as a operator i inherit all cutting conditions that is normal for me to figure out how to improve. i calculate sfpm and ipt although you might need to keep in metric
    .
    2) i often seen differences in part material and differences in cutting tools from batch to batch. sure sometimes part metal and heat treatment is consistent for a long time but that dont mean there are no differences ever
    .
    3) i use a optical presetter. on a screen at 20x magnification i can see runout. sometimes it is a cracked or damaged tool holder sometimes it is just a collet is dirty. without the magnified image of actual tool runut can vary with each tool change and needs to be checked on each tool setup . notice picture showing drill not resharpened enough. often cannot see cutting tool small defects without magnification
    .
    4) tool length usually it is better to keep tool stickout short and to a consistent length
    .
    5) feeds and speeds. often lowering rpm will lower vibration and vibration can resonate. that is at certain rpm vibration can increase 10x when vibration gets just right. often slowing rpm 50% does help
    .
    6) like a lot of things i write all parameters down and change things one at a time. when you change multiple items it is hard to tell what is doing what. but you also have to maintain repeatably. if you got random large runout amounts it can give random problems. large runout should never have made it to the spindle.
    .
    7) reasonable expectations. often somebody gets 1000 parts machined per cutting tool and does not realize they are already doing very good. sure cutting costs everybody wants to reduce. just saying often limits are reached and you do not get things much better as you have reached a practical limit
    Attached Thumbnails Attached Thumbnails parlecscreen.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
  •