Large Insert Drill in Aluminum Issues - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 36 of 36
  1. #21
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,363
    Post Thanks / Like
    Likes (Given)
    358
    Likes (Received)
    846

    Default

    Quote Originally Posted by Mud View Post
    I'm wondering if you have steel inserts with edge prep instead of aluminum inserts, and the material is building up on the edge of the drill or insert which catches on the retract. The description of rough finish, oversize hole and limited feed rate supports that suspicion.
    Can you post pictures of the drill and the workpiece?
    I will grab some pics on Monday. I'm actually taking a weekend off to get house stuff and maybe some brewing or race car stuff done! Haven't done that in a year.

  2. #22
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,410
    Post Thanks / Like
    Likes (Given)
    224
    Likes (Received)
    915

    Default

    We switched to allied drills we drill thru 7 inches of 7075 about 100 inches per minute 1 inch diameter no problem at all
    Don


    Sent from my iPhone using Tapatalk Pro

  3. Likes empwoer liked this post
  4. #23
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,436
    Post Thanks / Like
    Likes (Given)
    603
    Likes (Received)
    8473

    Default

    Why did you go to high pressure coolant?
    Yes this changes the breaking of the chips and can lead to fix or new chatter problems as it changes resonance of the system.
    Chatter is chip formation and break/twist cycle vs tool and spindle. You may have changed this cycle or frequency.
    May need to change feed to find a new sweet spot.
    Al and steel or cast iron cutting inserts very different so if a change here at the same time as pressure.......If somewhat working bad to change two things.
    Bob

  5. #24
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,357
    Post Thanks / Like
    Likes (Given)
    7761
    Likes (Received)
    9550

    Default

    Quote Originally Posted by Rick Finsta View Post
    I did this for the last hole on the part that was giving me issues yesterday but I also had the paper shim in the vise. I may just run this lot with shim and see what happens, but I don't like the idea of experimenting with a $20k+ spindle on the line. LOL
    Quote Originally Posted by Rick Finsta View Post
    It is 1000psig. I've got some relays laying here to get the low pressure hooked up (basically uses the feed pump through the filters into the spindle and bypasses the high pressure pump) but I need to do some electrical voodoo because of how Okuma spare M code keep relays work. The coolant ports face down the Z axis so upon breakthrough they are pointed towards the table. Maybe chips are blasting back upwards or dislodging from the T Slots and getting in the way?

    I don't have a square but the machine cuts square (I check parts on my CMM) and I did just check tram by sweeping the vise bases at the one year mark and everything looked good.


    I tried feeds of 0.006-0.010" and it wouldn't break a chip.

    When the tool rep gets in I want to try feeding in and out and lowering the breakthrough amount. I may also try a boring cycle and just stop the drill at the bottom and feed it out.

    Then again I might find out the last guy had the wrong inserts in there and that's been a problem the whole time LOL.

    You said somewhere else that your rec feed was up to .016, so why not drop your SFM and up the feed?

    Seems safer for your spindle concerns eh?


    BTW - what on Earth fer spindle doo you have that's 20 Large?
    I take it that _ that machine has an integrally wound motor/spindle like the neighbor shops Okuma lathe?




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

    Think Snow Eh!
    Ox

  6. #25
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,085
    Post Thanks / Like
    Likes (Given)
    1893
    Likes (Received)
    603

    Default

    Quote Originally Posted by D Nelson View Post
    We switched to allied drills we drill thru 7 inches of 7075 about 100 inches per minute 1 inch diameter no problem at all
    Don


    Sent from my iPhone using Tapatalk Pro
    the allied drills are no joke! we're doing the same thing, just a tad slower. working really good for us.

  7. #26
    Join Date
    Jan 2003
    Location
    Posts
    605
    Post Thanks / Like
    Likes (Given)
    130
    Likes (Received)
    194

    Default

    Which series allied drills are you guys using? I've been amazed at how fast you can go with their old style HSS spade drills, and how long they last. Not quite up to carbide performance but still impressive. Havent tried their new styles

  8. #27
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,085
    Post Thanks / Like
    Likes (Given)
    1893
    Likes (Received)
    603

    Default

    Quote Originally Posted by mmurray70 View Post
    Which series allied drills are you guys using? I've been amazed at how fast you can go with their old style HSS spade drills, and how long they last. Not quite up to carbide performance but still impressive. Havent tried their new styles
    this is the one i'm using
    Allied - Artikel-Detail

  9. Likes mmurray70, Silent_Man liked this post
  10. #28
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,363
    Post Thanks / Like
    Likes (Given)
    358
    Likes (Received)
    846

    Default

    Ox, it is an Okuma. LOL.

  11. #29
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,410
    Post Thanks / Like
    Likes (Given)
    224
    Likes (Received)
    915

    Default

    We are using the TA pro drill
    Allied
    Don


    Sent from my iPhone using Tapatalk Pro

  12. #30
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,563
    Post Thanks / Like
    Likes (Given)
    1662
    Likes (Received)
    2133

    Default

    My experience using insert drills in aluminium is that you have to either massively exceed the "correct" chipload, or massively reduce it. I run a 50-80mm drills quite frequently on parts we make out of 7075. It works great if you can push up to around 0.5mm/r, but if the machine can't manage that, then it also chips pretty nicely at .05-07mm/r. Anything in between is just strings and chip congestion.

    I use Sandvik (880) and Tungaloy (TDS) drills mainly.

  13. #31
    Join Date
    Nov 2019
    Country
    CANADA
    State/Province
    Ontario
    Posts
    589
    Post Thanks / Like
    Likes (Given)
    917
    Likes (Received)
    139

    Default

    i wonder if the work piece is relieving stress on breakthrough and bending the bore slightly allowing the drill to drag. have you stopped short and retracted and got the same thing?

  14. #32
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,506
    Post Thanks / Like
    Likes (Given)
    801
    Likes (Received)
    654

    Default

    Quote Originally Posted by Rick Finsta View Post


    Then again I might find out the last guy had the wrong inserts in there and that's been a problem the whole time LOL.
    That's what I'm starting to think. That drill shouldn't give issues, regardless of coolant flow.

  15. #33
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,363
    Post Thanks / Like
    Likes (Given)
    358
    Likes (Received)
    846

    Default

    So I did look this morning and the inserts are the correct ones. The insert grade is still visible on one of them and they are visually very different than the Sumitomos that the old owner used (and I still do)for the face mill.

    I spoke to me neighbor who does a ton of swiss stuff and he said they did occasionally see issues with harmonics developing when using high pressure coolant and needing to change speeds and feeds.

    Ingersoll rep will be in soon and wants me to look at another design. I really don't want to go to a smaller drill size and it looks like those Allied units only go up to 35mm. Realistically it would only cost me a few seconds of cycle time per part to have extra material there for roughing. Maybe not even. The rougher drops down in 0.375" depth increments and spirals out from the center of the drilled hole so no matter what I think it would traverse the same distance but obviously would be cutting more.

    If I can get a deal where I buy a few packs of inserts and get a drill body I might do that. I also need a few smaller drills (29/64" and 17/32" for the bolt clearance holes on these parts so I might see about those as well. I was going to pick up some Sandvik 870s or Sumitomo SMDs since I've had good luck with those and a local place can resharpen the insert tips on either. I think they also do the Ingersolls. I would of course prefer to just get this drill going for now.

    If I can avoid spending money I will. Material prices are going up and the pre-race-season rush seems to be dying off a bit...

  16. Likes empwoer liked this post
  17. #34
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    14,591
    Post Thanks / Like
    Likes (Given)
    2829
    Likes (Received)
    4327

    Default

    I think your feed/speed is good. We use the same drills in Iscar brand, we use a 2" in a lathe at 1500rpm/ .010 ipr which is very conservative because the operator doesn't want the slug flying out, he feeds slowly and stops just shy of the bottom. We use a 1.5" in a VMC at 3000 rpm/ 40ipm (.013 ipr) penetrating through the bottom with no issue, but no through coolant is being used.

  18. #35
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,363
    Post Thanks / Like
    Likes (Given)
    358
    Likes (Received)
    846

    Default

    So the tool rep stopped in and took a look at everything, and was on the same page as everyone here. Something changed in the harmonics that now I've got something going on at the bottom of the bore with a rapid retract where it is catching and chattering. The pulsing of the high pressure has to be hitting a natural harmonic of the drill/holder setup or something like that. Feed and Speed were about what he's seen before and he said he usually does see a need to increase feed above the "maximum" recommended to break a chip in some materials. He looked at the chips and thought they looked perfect.

    I tried using a reaming cycle and barely punching through the bottom and everything seems good to go. I did it without the paper shim just to remove that as a variable, but technically I did change two things (breakthrough depth and feed out versus rapid out).

    The cycle takes a little bit longer but I can still punch four holes in around a minute of cycle time (up from about 45 seconds).

    He did recommend that if I go to a shorter drill I also transition to their Quad-twist series, since it has a modern chip breaker geometry that help to break chips at lower feed per rev. I'll keep an eye out (I eventually need to get a shorter tool that will go through the tool changer to get this process more hands-off) on eBay and honestly will likely end up with whatever tool brand I can find for a decent price. I may even go to something smaller.

    I have heard a lot of people using Allied and have never seen someone going back to something else once they switch. That is what Pat Rogers (PBUH) called a "clue."

    I really appreciate everyone throwing ideas around with me.

  19. #36
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,357
    Post Thanks / Like
    Likes (Given)
    7761
    Likes (Received)
    9550

    Default

    Quote Originally Posted by Rick Finsta View Post
    So the tool rep stopped in and took a look at everything, and was on the same page as everyone here. Something changed in the harmonics that now I've got something going on at the bottom of the bore with a rapid retract where it is catching and chattering. The pulsing of the high pressure has to be hitting a natural harmonic of the drill/holder setup or something like that. Feed and Speed were about what he's seen before and he said he usually does see a need to increase feed above the "maximum" recommended to break a chip in some materials. He looked at the chips and thought they looked perfect.

    I tried using a reaming cycle and barely punching through the bottom and everything seems good to go. I did it without the paper shim just to remove that as a variable, but technically I did change two things (breakthrough depth and feed out versus rapid out).

    The cycle takes a little bit longer but I can still punch four holes in around a minute of cycle time (up from about 45 seconds).

    He did recommend that if I go to a shorter drill I also transition to their Quad-twist series, since it has a modern chip breaker geometry that help to break chips at lower feed per rev. I'll keep an eye out (I eventually need to get a shorter tool that will go through the tool changer to get this process more hands-off) on eBay and honestly will likely end up with whatever tool brand I can find for a decent price. I may even go to something smaller.

    I have heard a lot of people using Allied and have never seen someone going back to something else once they switch. That is what Pat Rogers (PBUH) called a "clue."

    I really appreciate everyone throwing ideas around with me.


    I thought that was "black"?


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

    Think Snow Eh!
    Ox


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
  •