New to solid carbide drills
Close
Login to Your Account
Results 1 to 14 of 14
  1. #1
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Kentucky
    Posts
    66
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    11

    Default New to solid carbide drills

    Machine: haas sl30 lathe
    Material: 4140
    Drill size 6.7mm with through tool coolant

    I know not to peck with a carbide drill, but any other best practice i need to know? Any speed and feed recommendations? The manufacture is recommending 6500 RPM and a feed of 0.007 IPR, this machine won’t spin that fast.
    Thank You

  2. #2
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,893
    Post Thanks / Like
    Likes (Given)
    2531
    Likes (Received)
    1292

    Default

    I'd keep the chipload the same and run as fast as you can. If the drill is long, do a pilot with a stub drill first, put the long drill in at a low RPM, then speed up and drill.

  3. #3
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,271
    Post Thanks / Like
    Likes (Given)
    915
    Likes (Received)
    512

    Default

    If you spot the hole first make certain it is with a tool that has a GREATER tip angle than your carbide. So if, for instance, your carbide drill has 140 degree tip make sure to use something equal to or greater than that....142 is a common spot drill tip angle for this reason. Good luck!

  4. Likes mhajicek liked this post
  5. #4
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    2,281
    Post Thanks / Like
    Likes (Given)
    247
    Likes (Received)
    2205

    Default

    Who told you not to peck?! Nothing wrong with pecking. Even with coolant thru if your pressure isn't the greatest, or sometimes you let the filters get a little dirtier than it should adding a few pecks in your program will make it more reliable. If I am drilling 3.5" deep and my flute length is 3.8 or 3.9" long I will add a few packs starting at 2.75".

    .007ipr in 4140 for a 6mm drill sounds very high. Drilling on a lathe where the drill is stationary is always worse than when the drill is spinning !!! I would start out with .0045 ipr.

  6. Likes Gobo, Nerdlinger, PegroProX440, Red James liked this post
  7. #5
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    13,623
    Post Thanks / Like
    Likes (Given)
    2995
    Likes (Received)
    9122

    Default

    If a blind hole you might program in brief dwell (.1 second or so) before retract. Doing the same before a peck is good too, but you might have to hand program.

    If through you might slow feed a bit during breakout.

  8. Likes Nerdlinger liked this post
  9. #6
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    794
    Post Thanks / Like
    Likes (Given)
    348
    Likes (Received)
    872

    Default

    Quote Originally Posted by fmari --MariTool- View Post
    Who told you not to peck?! Nothing wrong with pecking. Even with coolant thru if your pressure isn't the greatest, or sometimes you let the filters get a little dirtier than it should adding a few pecks in your program will make it more reliable. If I am drilling 3.5" deep and my flute length is 3.8 or 3.9" long I will add a few packs starting at 2.75".

    .007ipr in 4140 for a 6mm drill sounds very high. Drilling on a lathe where the drill is stationary is always worse than when the drill is spinning !!! I would start out with .0045 ipr.
    The Mitsubishi MVS drills I use recommends between .0043-.0094 for 4340 with .0071 being right in the middle for that size range. I routinely drill with these drills in the 25-40xd range in various diameters from 5mm-10mm in a single shot, but the machine we use them with has 1000PSI coolant. The 10mm we feed at .012 per rev and it makes beautiful holes. They also say not to peck. The problem for him comes down to being limited by spindle speed. Spin it as fast as you safely can and from there you'll have to play with your IPR until you get the best results.


    Op does need to clarify how deep because that does affect things.
    What brand drill are you using?
    What coating?

  10. #7
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Kentucky
    Posts
    66
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    11

    Default

    The depth is 1.125 and brand is widin with TiAIN coating.

  11. #8
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Kentucky
    Posts
    66
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    11

    Default

    Hand coding isn’t a problem, i had code everything i do on this machine.

  12. #9
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,987
    Post Thanks / Like
    Likes (Given)
    5642
    Likes (Received)
    3813

    Default

    Quote Originally Posted by FrankieB View Post
    Machine: haas sl30 lathe
    Material: 4140
    Drill size 6.7mm with through tool coolant

    I know not to peck with a carbide drill, but any other best practice i need to know? Any speed and feed recommendations? The manufacture is recommending 6500 RPM and a feed of 0.007 IPR, this machine won’t spin that fast.
    Thank You
    In 4140 I typically go around 300sfpm for solid carbide drills. That comes out to around 4400rpm, and I agree with Frank, the .007 is a tad high... maybe kick it down to around .005ipr and send it.

  13. #10
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Kentucky
    Posts
    66
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    11

    Default

    I want to thank everyone for the recommendation, i went with 3000 rpm at 0.005 ipr.

  14. Likes mhajicek, Mtndew liked this post
  15. #11
    Join Date
    Dec 2017
    Country
    CANADA
    State/Province
    Alberta
    Posts
    70
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    15

    Default

    Quote Originally Posted by fmari --MariTool- View Post
    Who told you not to peck?! Nothing wrong with pecking. Even with coolant thru if your pressure isn't the greatest, or sometimes you let the filters get a little dirtier than it should adding a few pecks in your program will make it more reliable. If I am drilling 3.5" deep and my flute length is 3.8 or 3.9" long I will add a few packs starting at 2.75".

    .007ipr in 4140 for a 6mm drill sounds very high. Drilling on a lathe where the drill is stationary is always worse than when the drill is spinning !!! I would start out with .0045 ipr.
    Almost every manufacturer that I've seens technical guide tells you specifically not to peck. Heck even allied tells you not to on their spade drills.

  16. #12
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,578
    Post Thanks / Like
    Likes (Given)
    619
    Likes (Received)
    8546

    Default

    Quote Originally Posted by escapethewrmhole View Post
    Almost every manufacturer that I've seens technical guide tells you specifically not to peck. Heck even allied tells you not to on their spade drills.
    The process of the how and by whom these "technical guides" are often written is interesting and sometimes scary.
    Bob

  17. Likes Orange Vise liked this post
  18. #13
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,901
    Post Thanks / Like
    Likes (Given)
    604
    Likes (Received)
    346

    Default

    Quote Originally Posted by CarbideBob View Post
    The process of the how and by whom these "technical guides" are often written is interesting and sometimes scary.
    Bob
    Somebody tried something and it worked. It then becomes gospel.

    Look at the sfm values for diamond tools in Machinery's Handbook. They're all over the place! I figure that it's due to rpm limitations on whatever machine they were using at the time the data was compiled.

    So there you go.

  19. #14
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    2,281
    Post Thanks / Like
    Likes (Given)
    247
    Likes (Received)
    2205

    Default

    Quote Originally Posted by CarbideBob View Post
    The process of the how and by whom these "technical guides" are often written is interesting and sometimes scary.
    Bob
    Very hard to get and keep good technical cutting tool engineers. The good ones are making 6 figures in machines shops and not making technical guides.

  20. Likes Orange Vise 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
  •