Need pointers for drilling ETD150
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 42
  1. #1
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,934
    Post Thanks / Like
    Likes (Given)
    883
    Likes (Received)
    2064

    Default Need pointers for drilling ETD150

    Hello all.

    I make an extra deep-well socket as an application tool for an OEM. I was using Stressproof but the OEM has requested a stronger material so I selected ETD150...and it's kicking my ass.

    The hole is .75" diameter and 7" deep, drilling in a Fadal VMC4020 with a PTD HSS drill. 75SFM, .008ipr, 0.188" pecks, no dwell. Rapid set to 25% (225IPM) to increase cooling during the peck feed moves. Coolant is Trim 690xt, ~8%.

    It goes very well until about 4" deep, then squeals and spindle load goes through the roof.

    I called Allied about a spade drill but without TTC they figured it was a fool's errand, and I think I agree.

    Does anyone see any glaring errors here? I have 25 of these to do.


    Thanks!

  2. #2
    Join Date
    Jan 2003
    Location
    Canada
    Posts
    11,401
    Post Thanks / Like
    Likes (Given)
    5771
    Likes (Received)
    3520

    Default

    Probably chips clogging up the flutes when you're past about 4". I'd try shallower pecks past that point, maybe .100" and see if that changes anything.
    That's assuming the hole is going in fairly straight too and drill has a good split point tip. Might be getting lots of chips falling back down the hole too eh?

  3. Likes Limy Sami liked this post
  4. #3
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,453
    Post Thanks / Like
    Likes (Given)
    410
    Likes (Received)
    654

    Default

    IMHO, Allied drills are good for banging out quick & dirty ops on the Bport or lathe; mediocre on a VMC.
    The flutes aren't shaped for optimal chip evacuation and their geometry isn't spectacular.
    Tooling costs are cheap, though. That's the good part.
    If this is something you are doing a lot, I would look at Iscar or Kennametal for a better solution.
    Otherwise, full retract peck drilling will be your ace-in-the-hole.

  5. #4
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,453
    Post Thanks / Like
    Likes (Given)
    410
    Likes (Received)
    654

    Default

    If you have the choice of material, would 41L40 work?
    Strong (it's chrome-moly after all ), heat-treatable, and not hard to machine.

  6. #5
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    3,617
    Post Thanks / Like
    Likes (Given)
    764
    Likes (Received)
    2505

    Default

    I don't know about Fadal canned cycles- on a Fanuc I would be using a G83 deep hole cycle. That's a full retract to clear the chip on each peck. G73 is the high speed peck cycle, and it only breaks the chip. So when you get deep in the hole, the chips still pack up on the G73 cycle, the G83 cycle will take them all the way out of the hole.

    I do some deep holes that I break up into 2 or 3 cycles, with parameters appropriate to the depth. I'll take a large G73 peck when the drill is shallow, then switch it over to a shallower peck and G83 cycle when the hole gets deeper. I usually separate the cycles with a fast G1 move to the new start point.

    It's a little more work to program, but I don't sell programs- I sell parts...

  7. Likes Cole2534, Garwood liked this post
  8. #6
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    19,871
    Post Thanks / Like
    Likes (Given)
    15322
    Likes (Received)
    15593

    Default

    Quote Originally Posted by Cole2534 View Post
    Hello all.

    I make an extra deep-well socket as an application tool for an OEM. I was using Stressproof but the OEM has requested a stronger material so I selected ETD150...and it's kicking my ass.

    The hole is .75" diameter and 7" deep, drilling in a Fadal VMC4020 with a PTD HSS drill. 75SFM, .008ipr, 0.188" pecks, no dwell. Rapid set to 25% (225IPM) to increase cooling during the peck feed moves. Coolant is Trim 690xt, ~8%.

    It goes very well until about 4" deep, then squeals and spindle load goes through the roof.


    I called Allied about a spade drill but without TTC they figured it was a fool's errand, and I think I agree.

    Does anyone see any glaring errors here? I have 25 of these to do.


    Thanks!
    Are you sure the drill's not worn on diameter etc etc - they should have a back taper - which often disappears with use, .and that makes them jamb like
    Last edited by Limy Sami; 05-22-2020 at 02:24 AM. Reason: typo

  9. #7
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    9,267
    Post Thanks / Like
    Likes (Given)
    2192
    Likes (Received)
    6426

    Default

    That the process works well until a certain depth makes it likely it's a drill geometry issue, not anything to do with the material.

    Drill to the best depth, then switch to a longer fluted drill for the remainder, perhaps cutting the SFM but upping the peck a bit. When deep drilling without TSC on a VMC I like to minimize drill retraction to lower the risk of chips falling back into the hole and causing trouble when the drill comes back down.

    Similarly, I'd use a return distance above the last drill depth, then feed in to allow chips to be swept away by the drill point, rather than hammered into. I know you can do this with G83 options on a Haas, not sure if a Fadal has the same capability. At worst you could program a sequence of G1/G0 to clear and return moves to achieve the same effect.

  10. #8
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,934
    Post Thanks / Like
    Likes (Given)
    883
    Likes (Received)
    2064

    Default

    Forgot to mention earlier, this is a G83 cycle.

    I'm contemplating adding a short dwell prior to retract, 1-2revs to ensure the hole's bottom doesn't have some abnormality the drill point is slamming back into. At .008ipr there wouldn't be a huge ledge, but maybe that will help?

    Sent from my SM-G930R4 using Tapatalk

  11. #9
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,934
    Post Thanks / Like
    Likes (Given)
    883
    Likes (Received)
    2064

    Default

    Quote Originally Posted by ChipSplitter View Post
    If you have the choice of material, would 41L40 work?
    Strong (it's chrome-moly after all ), heat-treatable, and not hard to machine.
    Fatigueproof would be my next choice.

    Short-chip steels are amazing.

    Sent from my SM-G930R4 using Tapatalk

  12. #10
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,518
    Post Thanks / Like
    Likes (Given)
    1737
    Likes (Received)
    2166

    Default

    Do you have a cnc lathe? Drilling horizontal would help with chips somewhat, and it is pretty easy to get "coolant thru" the way most cnc lathes are plumbed. Just modify a back plate, or add a fitting, etc.

  13. #11
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,453
    Post Thanks / Like
    Likes (Given)
    410
    Likes (Received)
    654

    Default

    Quote Originally Posted by Cole2534 View Post
    Fatigueproof would be my next choice.

    Short-chip steels are amazing.

    Sent from my SM-G930R4 using Tapatalk
    Fatigueproof is similar to ETD150 OTOH.

    Both are "Elevated Temperature Drawn".

    41L40 would be my choice because the lead will make amazingly short chips, better than ETD150.

  14. #12
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    73
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    29

  15. #13
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    109
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    20

    Default

    I like the idea of 41L40 but of course HT runs up the price. :-(
    However, being of good cheer and possessing a fertile imagination ... this sounds like gun drill territory. Emulate a gun drill on your lathe.
    So much depends on the cost margin you have to work with. Short ... .75 x 16" gun drills seems to cost about the same as smaller gun drills. But screwing around for a day does also. If this were easy you'd have it done by now. :-)
    I hope something works well for you.

  16. #14
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,453
    Post Thanks / Like
    Likes (Given)
    410
    Likes (Received)
    654

    Default

    This is REALLY off the wall but.....

    1) Clamp part in lathe turret.
    2) Put parabolic flute drill in chuck.
    3) Drill hole. The revolving drill will pull the chips out better than a revolving part.

    ?? IDK....

  17. #15
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,419
    Post Thanks / Like
    Likes (Given)
    897
    Likes (Received)
    1543

    Default

    Quote Originally Posted by Cole2534 View Post
    I have 25 of these to do.
    Not that many, so I'd just baby it for the last half.

    Reduce the peck, slow down rapids, and keep your R plane high enough to so you can maybe rig up an air blast.

  18. #16
    Join Date
    Aug 2017
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    7

    Default

    I'd second 41L40. I used to do a lot of long shaft work in 4140 and we were always fighting chatter issues in mid-cut when approaching the center of the shaft. Switched to 41L40 and it was light night and day. Much easier going, no compromise on strength.

  19. #17
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    9,267
    Post Thanks / Like
    Likes (Given)
    2192
    Likes (Received)
    6426

    Default

    Quote Originally Posted by ChipSplitter View Post
    This is REALLY off the wall but.....

    1) Clamp part in lathe turret.
    2) Put parabolic flute drill in chuck.
    3) Drill hole. The revolving drill will pull the chips out better than a revolving part.

    ?? IDK....
    No, clamp bar in spindle of mill, drill in vise - BOOM! Instant hole maker.

    [I've actually done this with some parts, and it works really well. Just fiddle with coolant delivery to have a fixed nozzle or two aiming up where the drill is clamped]

  20. Likes ChipSplitter, gbent liked this post
  21. #18
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,453
    Post Thanks / Like
    Likes (Given)
    410
    Likes (Received)
    654

    Default

    Quote Originally Posted by Milland View Post
    No, clamp bar in spindle of mill, drill in vise - BOOM! Instant hole maker.

    [I've actually done this with some parts, and it works really well. Just fiddle with coolant delivery to have a fixed nozzle or two aiming up where the drill is clamped]
    Ahhh....

    And use a straight flute coolant fed drill so the chips just fall out.
    Doesn't take much coolant pressure, just 5-10 psi.

    Brilliant, Milland!!

  22. #19
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,934
    Post Thanks / Like
    Likes (Given)
    883
    Likes (Received)
    2064

    Default

    Quote Originally Posted by Orange Vise View Post
    Not that many, so I'd just baby it for the last half.

    Reduce the peck, slow down rapids, and keep your R plane high enough to so you can maybe rig up an air blast.
    I think that's the answer.

    I do not have a cnc lathe yet, need a damn Mazak or Okuma to show up juuuussstt right.

    Thanks for the help gentlemen.

    Sent from my SM-G930R4 using Tapatalk

  23. #20
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,884
    Post Thanks / Like
    Likes (Given)
    1291
    Likes (Received)
    2760

    Default

    Quote Originally Posted by Milland View Post
    No, clamp bar in spindle of mill, drill in vise - BOOM! Instant hole maker.

    [I've actually done this with some parts, and it works really well. Just fiddle with coolant delivery to have a fixed nozzle or two aiming up where the drill is clamped]
    Worst idea of 2020!! Why not just put it under your pillow at night and hope a hole gets in there?!

    R


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
  •