Advice for drilling solid copper
Close
Login to Your Account
Results 1 to 19 of 19
  1. #1
    Join Date
    Oct 2021
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Advice for drilling solid copper

    Hello everyone. Needing some help with drilling a .062 hole into .130 diameter material on a lathe. My current program reads as follows
    G97 s1000 m13;
    M98p1;
    T4x0.;
    Z.2 s3000;
    G1 g99 z-.65 f.0005;
    M98p1;
    I'm running on an older hardinge lathe, with barely any stock protruding from the face of the spindle and it pulls out to part length after it drills to prevent the stock from bending. Chuck pressure is all the way down to 30psi to prevent crushing. Carbide through coolant drill.
    I've managed to make 1 part and the drill broke on the second. I've tried many different speed and feed combinations with no consistent luck. Does anyone have any ideas what to do to get this thing to run consistent? Thanks in advance

  2. #2
    Join Date
    Aug 2004
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    2,974
    Post Thanks / Like
    Likes (Given)
    248
    Likes (Received)
    1400

    Default

    It kind of depends on if you have the equipment to change the profile of your carbide bits. Copper is gummy and grabs pretty easily. That is probably the reason you broke your bit. It is a common practice to dub the bit when drilling copper to keep it from grabbing. If you don't have the equipment to change the profile of your carbide bits then I would go to a standard bit and dub it.

  3. #3
    Join Date
    Feb 2004
    Location
    peekskill, NY
    Posts
    27,598
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6488

    Default

    What is the top spindle speed on this machine?

  4. Likes Mtndew liked this post
  5. #4
    Join Date
    Oct 2021
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I am honestly not sure

  6. #5
    Join Date
    Oct 2021
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks! I'll give it a shot

  7. #6
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,308
    Post Thanks / Like
    Likes (Given)
    3187
    Likes (Received)
    1677

    Default

    Might be better off with a cobalt drill instead of carbide.

  8. #7
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,296
    Post Thanks / Like
    Likes (Given)
    5881
    Likes (Received)
    4025

    Default

    Quote Originally Posted by Emilyfinchum View Post
    G97 s1000 m13;
    That's 16 SFPM. WAY too slow.
    You need to spin at least 4,000rpm if your machine can go that fast.

  9. #8
    Join Date
    Feb 2004
    Location
    peekskill, NY
    Posts
    27,598
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6488

    Default

    Quote Originally Posted by Mtndew View Post
    That's 16 SFPM. WAY too slow.
    You need to spin at least 4,000rpm if your machine can go that fast.
    I think 100 SFPM is about right. For a 1/16 dia drill that's about 6000 rpm

    0.062 X 3.14 = .198 inch circumference = 0.0165 feet circumference

    100 ft/min / 0.0165 feet = 3030 rev/min

    What's the max speed on the lathe?

  10. #9
    Join Date
    Aug 2021
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    34

    Default

    I had a somewhat similar situation. Went to straight flute drills. That took care of it for me

  11. #10
    Join Date
    Aug 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    1,755
    Post Thanks / Like
    Likes (Given)
    1373
    Likes (Received)
    750

    Default

    Quote Originally Posted by Woodeye1 View Post
    I had a somewhat similar situation. Went to straight flute drills. That took care of it for me
    Are you referring to a half round drill?

  12. #11
    Join Date
    May 2021
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    346
    Post Thanks / Like
    Likes (Given)
    379
    Likes (Received)
    89

    Default

    Quote Originally Posted by Illinoyance View Post
    Are you referring to a half round drill?
    McMaster-Carr

    Maybe these.

  13. #12
    Join Date
    May 2021
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    346
    Post Thanks / Like
    Likes (Given)
    379
    Likes (Received)
    89

    Default

    Thought it was standard practice to "brass off" the edges on a twist drill if you're going to drill something soft like copper. Basically just dull the cutting edges a bit. I usually just drag the cutting edges over a fine stone or use a diamond file.

  14. #13
    Join Date
    Feb 2004
    Location
    peekskill, NY
    Posts
    27,598
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6488

    Default

    I advise against dubbing the edge on a 1/16 drill going into copper.

  15. #14
    Join Date
    May 2021
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    346
    Post Thanks / Like
    Likes (Given)
    379
    Likes (Received)
    89

    Default

    Quote Originally Posted by jim rozen View Post
    I advise against dubbing the edge on a 1/16 drill going into copper.
    Ehhhhh... I think it's worth a shot. Especially since they're doing this on a CNC machine. More torque on the drill bit, but it aught to be less "grabby".

    Could also try peck drilling.

    Maybe use a sharp drill and go at a more conservative feed rate?

  16. #15
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    60
    Post Thanks / Like
    Likes (Given)
    120
    Likes (Received)
    16

    Default

    My grandfather turned a good amount of copper and he used straight flute drills. At first I thought they were reamers. He also used milk instead of a cutting oil.
    Not sure if these drills are available today. I dub the cutting edge and also the flutes on one set of drills. I mark these drills with blue dykom on the shaft so I do not mix them up with other drills.

  17. Likes 52 Ford, boslab, MilGunsmith liked this post
  18. #16
    Join Date
    Sep 2007
    Location
    Maryland near DC
    Posts
    420
    Post Thanks / Like
    Likes (Given)
    90
    Likes (Received)
    88

    Default

    Back in the day we machined a lot of OHFC copper. Holes were typically much smaller, ~0.020”. No attempt was made to dub them. Drilling was always done by hand with a sensitive drill chuck. The only lubricant used for copper was lard oil.

  19. Likes MilGunsmith liked this post
  20. #17
    Join Date
    Feb 2004
    Location
    peekskill, NY
    Posts
    27,598
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6488

    Default

    Quote Originally Posted by mnl View Post
    Back in the day we machined a lot of OHFC copper. Holes were typically much smaller, ~0.020”. No attempt was made to dub them. Drilling was always done by hand with a sensitive drill chuck. The only lubricant used for copper was lard oil.
    Our standard lube for copper is 50/50 kerosene/lard oil. Dead sharp drills. The drill breakage mentioned is probably because of low spindle speed and excess feed rate per turn.

  21. #18
    Join Date
    Jan 2007
    Location
    wales.uk
    Posts
    1,918
    Post Thanks / Like
    Likes (Given)
    438
    Likes (Received)
    455

    Default

    We used tallow in work, came in big sticks for Ali saws
    Had a funny thought, we used a big pacemaker lathe to machine copper Lance tips, like 25’ centres, I was imagining cleaning the drip dray from swarf flavoured yogurt, not nice
    Electrical copper was a pig, beryllium copper was fairly tolerable
    Mark

  22. #19
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,414
    Post Thanks / Like
    Likes (Given)
    2131
    Likes (Received)
    899

    Default

    Quote Originally Posted by Emilyfinchum View Post
    Hello everyone. Needing some help with drilling a .062 hole into .130 diameter material on a lathe. My current program reads as follows
    G97 s1000 m13;
    M98p1;
    T4x0.;
    Z.2 s3000;
    G1 g99 z-.65 f.0005;
    M98p1;
    I'm running on an older hardinge lathe, with barely any stock protruding from the face of the spindle and it pulls out to part length after it drills to prevent the stock from bending. Chuck pressure is all the way down to 30psi to prevent crushing. Carbide through coolant drill.
    I've managed to make 1 part and the drill broke on the second. I've tried many different speed and feed combinations with no consistent luck. Does anyone have any ideas what to do to get this thing to run consistent? Thanks in advance

    I just finished drilling 0.039" holes through 1" of 99% pure copper.
    The drill was a standard, jobbers drill. Nothing specialized for copper or anything.
    I broke the first drill trying to do it manually.
    Then I changed to the cnc mill, flooded the drill with coolant, & pecked it out.

    S8000M3
    M8
    G00 G43 Hhh
    X.xx Y.yy
    Z.zz
    G83 X.xx Y.yy Z.zz F0.0008 Q0.01
    G80

    It worked beautifully, and ran with no problems.

    Doug.

  23. Likes 52 Ford 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
  •