Feeds and Speeds for 1/8" Parabolic Drill - I keep breaking them - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 36 of 36
  1. #21
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,337
    Post Thanks / Like
    Likes (Given)
    275
    Likes (Received)
    2187

    Default

    Tell us the exact process, center drill etc

    Occurs to me that I have had problems with chips running up into the grooves in the collet packing the chips in the hole.

    IF you changed the drill and put it in the collet deeper[perhaps thinking better support] it could cause this

    Carefully setting the drill sot he flutes are not lined up with the collet grooves and that they end before the drill enters the collet.

    I have a dim memory of putting a 1/2 diameter disk on a drill on slower spindle machine to stop the chip loading in the collet or maybe chuck.


    I just looked it up, I run cobalt stub drills .121 dia, .5 deep[really .25-.4 material] no peck in 6063 at 10500rpm 120 ipm, and 5000 rpm 50 ipm, no center drill.

    I really don't know how many tens of thousands of holes I get out of a drill.

    Not apples to apples, but similar.

    A long drill I would center drill and run slower

  2. #22
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,216
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2653

    Default

    Quote Originally Posted by crane550 View Post
    Hello,

    I hope someone can give me some advice.

    SPECS:
    Haas VF4-SS, 6061 Aluminum, Flood Cooling
    Chicago Latrobe 120DHT Parabolic drill, depth of 2.3 inches


    I bought a company that makes a product that has been in production for quite a while. I am a one man show at this point. Somewhere on the order of thousands of parts already made, 160 or so by me.

    We are drilling 8x holes per part at a depth of 2.3" deep, approximately. Accuracy only matters for the top 1" or so, and even then the tolerance is not all that important. We spot drill first and are using Chicago Latrobe 120DHT 1/8" parabolic end mills. Historically these have been drilled at 6112 RPM at 24IPM (200 SFM, .004 IPR) with a 0.75" peck drill. Since I have taken over the company (one man shop) I have cycled 160 or so units without changing out the bit, until recently when the installed bit broke. After the 1st breakI replaced it and the new one broke on the 1st hole. I replaced it again and got 5 holes out of it. Replaced again and broke on the 2nd hole. I have tried reducing my speeds and feeds to be as safe as possible with no luck.

    I have reduced my SFM to 150 which is 4584 RPM and and a IPR to .002 but still broke. I get a lot of squeaking on the plunge. Any ideas? Tired of making scraps! Those broken bits don't come out and my oops pile (wall of shame) is growing and more importantly I'm out of production at the moment.

    Thanks in advance!
    Alex
    .
    1) obviously some aluminum is more abrasive (dulls drill faster) and sticks to cutting edges more easily especially if coolant not reaching drill tip. different material can easily effect things. if drill packed with chips coolant not reaching tip in a deep hole and drill tip gets hot chips start sticking
    .
    2) chips sticking to flutes or still in hole. if rapids too fast coolant doesnt wash chips off drill and chips still in hole and drill rapid reentry crashing into chips still in hole can be hard on drill
    .
    3) drill lot or sometimes whole package of drill bits is brittle and break extra easy. sometimes drill tip not sharpened correctly (slightly off) and is giving problems
    .
    4) feeds and speeds. if sudden tool failure causing massive delays and extra costs often its faster and cheaper in the long run to back off feeds and speeds and peck depth and slow rapids. that is if going 50% slower is increasing reliability that often at end of year is the most important factor. like driving a car at 55mph rather than 100mph. might seem slower but avoiding a crash saves time in the long run
    .
    5) if metal has hardness variations the drill will drift towards softer material. a curved hole and or wavy hole can be hard on some drill bits. some start resonance vibrating which can easily break drill bit. often vibration can occur even when feeds and speeds are considered normal. easily have seen that many hundreds of times. and often its not every hole could easily be 1 out of 10 holes where drill starts resonance vibration til it breaks. usually its a rpm drill doesnt like and often it needs a big rpm change to stop the vibration. tool length to dia ratio or stickout amount can have a big effect.

  3. #23
    Join Date
    Sep 2011
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    27,630
    Post Thanks / Like
    Likes (Given)
    7561
    Likes (Received)
    8603

    Default

    Quote Originally Posted by gustafson View Post

    Occurs to me that I have had problems with chips running up into the grooves in the collet packing the chips in the hole.

    IF you changed the drill and put it in the collet deeper[perhaps thinking better support] it could cause this

    Carefully setting the drill sot he flutes are not lined up with the collet grooves and that they end before the drill enters the collet.

    I have a dim memory of putting a 1/2 diameter disk on a drill on slower spindle machine to stop the chip loading in the collet or maybe chuck.


    I just looked it up, I run cobalt stub drills .121 dia, .5 deep[really .25-.4 material] no peck in 6063 at 10500rpm 120 ipm, and 5000 rpm 50 ipm, no center drill.

    I really don't know how many tens of thousands of holes I get out of a drill.
    Thee yah go. Sub 2K holes per drill is no big deal.

    The drop to 1, 2, or 5 OTOH?

    That's like the fat lady who got too close to the train tracks.

    Dis-ASSED-her.

  4. #24
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,216
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2653

    Default

    drill depth to dia ratio has a big effect.
    .
    can drill a million shallow holes with no problems and can easily have massive sudden tool failure with deeper drill depths. you should try drilling .25 dia at over 12" depths with 24" long drill bit, its a lot different than 1" depths with a 4" long drill bit

  5. #25
    Join Date
    May 2017
    Country
    FINLAND
    Posts
    1,775
    Post Thanks / Like
    Likes (Given)
    496
    Likes (Received)
    812

    Default

    Quote Originally Posted by crane550 View Post
    Interesting, can you explain why? I am trying to learn this.
    Aluminium sticks to (PVD) TIN coating more easily than bare metal.
    Aluminum Machining, Machining Aluminum, High Speed Machining | Radical Departures
    TiN: The titanium-nitride coating | RUKO
    "When machining aluminium only suitable with stationary machine tools using forced liquid cooling"


    PVD(physical vapor deposition) TIN coating is dull matt and slighly rough surface.
    Some drills also come with very shiny TIN coating and those seem to perform somewhat OK with aluminium.

  6. #26
    Join Date
    Mar 2005
    Location
    Northwest Indiana
    Posts
    4,217
    Post Thanks / Like
    Likes (Given)
    845
    Likes (Received)
    848

    Default

    He's doing lower receivers. That's one hole per workpiece. If the drill is the same and coolant is good I'd be looking awfully hard in the material's direction. Gummy aluminum is a right bastard to drill.

  7. #27
    Join Date
    May 2017
    Country
    FINLAND
    Posts
    1,775
    Post Thanks / Like
    Likes (Given)
    496
    Likes (Received)
    812

    Default

    Quote Originally Posted by eKretz View Post
    He's doing lower receivers. That's one hole per workpiece. If the drill is the same and coolant is good I'd be looking awfully hard in the material's direction. Gummy aluminum is a right bastard to drill.
    Same drill except the TIN coating..
    Material would be another good suspect even still.

  8. #28
    Join Date
    Sep 2011
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    27,630
    Post Thanks / Like
    Likes (Given)
    7561
    Likes (Received)
    8603

    Default

    Quote Originally Posted by eKretz View Post
    He's doing lower receivers. That's one hole per workpiece. If the drill is the same and coolant is good I'd be looking awfully hard in the material's direction. Gummy aluminum is a right bastard to drill.
    "Drill" not-only..

    Have to admit so much so, my first reaction to facing that challenge is to see whether to make "whatever" in steel or bronze instead!

    A man has got to know his limitations. Lack of bleedin' PATIENCE on the list..

    Some OTHER Pilgrim deals with shiney-wood.

    Not as if there was only the ONE guy better at it than I care to bother to become, nor that folks get medals for doin' it. World is full of 'em. Their stuff mostly just works.

    Happy to JF buy the product of THEIR skills and experience, stick to the more predictable PITA-gnarlies like Mangalloys and Nickel-Aluminium-Bronze, thanks!


  9. #29
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    7,432
    Post Thanks / Like
    Likes (Given)
    698
    Likes (Received)
    3510

    Default

    Quote Originally Posted by eKretz View Post
    He's doing lower receivers. That's one hole per workpiece. If the drill is the same and coolant is good I'd be looking awfully hard in the material's direction. Gummy aluminum is a right bastard to drill.
    When stuck using crappy aluminum like Chinese 6061 or Service Center (Domestic reclaim, quality varies)I have found I have to up to triple cycle times over good domestic or European to keep from gumming up tools, breaking them and not getting a laminated finish.

  10. Likes eKretz liked this post
  11. #30
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    7,432
    Post Thanks / Like
    Likes (Given)
    698
    Likes (Received)
    3510

    Default

    Quote Originally Posted by MattiJ View Post
    Same drill except the TIN coating..
    Material would be another good suspect even still.
    With drills and taps I use bright finish only on aluminum. They also are usually the cheapest to boot.

  12. Likes MattiJ liked this post
  13. #31
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thanks for the replies, everyone. We seem to be up and going again, although I watch that OP very carefully. If a bit breaks then you ruin a brand spankin new end mill...don't ask me how I know.

    I have changed to the following strategy and it seems to be working well:

    6070 RPM (200 f/min)
    30 IPM Feed (.0025 in/tooth)
    .375 first peck, .25 second, and .125 the rest.

    I think my issue was the peck depth. .750 was just way too much, even if it worked for a lot of holes. Might get more aggressive again in the future, we will see.

    Small squeak every once in a while but not bad. Also my coolant mixture was on the lean side so I added more. Pressure has always been good. Cut ~60 holes so far and no break. Still monitoring closely.

    Thanks a ton for the help.

  14. #32
    Join Date
    Sep 2011
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    27,630
    Post Thanks / Like
    Likes (Given)
    7561
    Likes (Received)
    8603

    Default

    Quote Originally Posted by crane550 View Post
    I have changed to the following strategy and it seems to be working well:

    6070 RPM (200 f/min)
    30 IPM Feed (.0025 in/tooth)
    .375 first peck, .25 second, and .125 the rest.
    Suggestion: Take out the first .375", start with .250", then to .125"
    Personally, I'd start with .125" and stay there.

    Either way, it's trivially more pecks, but your now-and-then squeak might cease?
    Last edited by thermite; 10-24-2019 at 08:18 AM.

  15. #33
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,337
    Post Thanks / Like
    Likes (Given)
    275
    Likes (Received)
    2187

    Default

    Quote Originally Posted by DMF_TomB View Post
    drill depth to dia ratio has a big effect.
    .
    can drill a million shallow holes with no problems and can easily have massive sudden tool failure with deeper drill depths. you should try drilling .25 dia at over 12" depths with 24" long drill bit, its a lot different than 1" depths with a 4" long drill bit
    I think we all understand the difficulty and difference drilling deep holes

    The example I gave while significantly shallower, was twice as fast, with inferior setup[no center drill], inferior tool[standard cylindrical drill] and gummier material[6063]

    I have done enough holes that I think he should be able to get near infinite tool life if set up correctly

  16. #34
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,706
    Post Thanks / Like
    Likes (Given)
    1138
    Likes (Received)
    985

    Default

    Maybe go as deep as you can with a short length cobalt drill, then switch to the parabolic, not too time consuming if you have an ATC.

    Something sounds wrong though, there's likely a simple explanation, why it worked well, then doesn't, I suspect the drill.

  17. #35
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    535
    Post Thanks / Like
    Likes (Given)
    257
    Likes (Received)
    421

    Default

    Guhring 619 series, cobalt, uncoated, extra length 1/8" diameter, good for 20xD

    Quit using shit tools.

  18. #36
    Join Date
    Sep 2006
    Location
    Middletown, PA
    Posts
    482
    Post Thanks / Like
    Likes (Given)
    160
    Likes (Received)
    59

    Default

    Quote Originally Posted by crane550 View Post
    .... Also my coolant mixture was on the lean side so I added more...
    How lean is lean?
    If this part ran with the original parameters, it would have needed alot of lubrication to keep the flutes from packing.
    Drill the same hole on a drill press to get an idea how much material has to come out per peck.

    None of my business, but have you had any machining experience?


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
  •