3/8 hole ~9D deep in 6061
Close
Login to Your Account
Results 1 to 15 of 15
  1. #1
    Join Date
    Oct 2014
    Country
    UNITED STATES
    State/Province
    Maine
    Posts
    1,353
    Post Thanks / Like
    Likes (Given)
    268
    Likes (Received)
    646

    Default 3/8 hole ~9D deep in 6061

    I need a thru hole in 6061, about 3.25" deep, to be .378 -0/+.003 after anodizing. My anodizer says I'll have about .0006 per side, half of that being buildup, so I was going to go for a .3795 hole before anodizing. My current plan is to spot drill, then drill 23/64 thru from one side with a good taper length drill, then ream with a .3795 reamer with plenty of cutting fluid. I can do the reaming in the machine (should I have a special holder for this?) or with a hand drill or drill press.

    I did think about drilling from both ends and then reaming through, but my concern is that they won't be perfectly concentric and the reamer will follow a wandering path.

    For the drill, a Guhring 535 series is readily available. It looks like a good drill and says it's good for non-ferrous and steel, just not stainless. It doesn't, however, give speeds and feeds for regular aluminum, just for cast aluminum. That seems pretty common and confusing. For example, the 5536 says on it's page that it's good for non-ferrous, but then the non-ferrous section is blank on the speeds and feeds document.

    It looks like the best drill for aluminum might be the 501, but it's just for non-ferrous. I'm only doing two of these parts, so if I can buy a more versatile tool and use it again on another project, that would be great.

  2. #2
    Join Date
    Oct 2014
    Country
    UNITED STATES
    State/Province
    Maine
    Posts
    1,353
    Post Thanks / Like
    Likes (Given)
    268
    Likes (Received)
    646

    Default

    I should add, it's a Prototrak FHM7 bed mill. 40 taper, 5k rpm

  3. #3
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,380
    Post Thanks / Like
    Likes (Given)
    2552
    Likes (Received)
    3158

    Default

    Might not be much help, but Sandvik sells tooling with geometries that are supposed to be good for stainless and aluminum. Drills, endmills, etc

  4. #4
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    6,598
    Post Thanks / Like
    Likes (Given)
    779
    Likes (Received)
    3919

    Default

    How many do you have to do

    I guess I would center drill then drill, to keep the wander down. might be tempted to go most of the way with a stub drill to keep it straight, but it is another tool change, which is time

  5. #5
    Join Date
    Oct 2014
    Country
    UNITED STATES
    State/Province
    Maine
    Posts
    1,353
    Post Thanks / Like
    Likes (Given)
    268
    Likes (Received)
    646

    Default

    Quote Originally Posted by gustafson View Post
    How many do you have to do

    I guess I would center drill then drill, to keep the wander down. might be tempted to go most of the way with a stub drill to keep it straight, but it is another tool change, which is time
    I'm only doing two of them. Unfortunately though, this hole is drilled fairly late in the process, so if the hole is bad, a lot of work is wasted. So I don't really care how long it takes to drill the hole, just that it's right.

  6. #6
    Join Date
    Sep 2011
    Location
    Posts
    2,273
    Post Thanks / Like
    Likes (Given)
    547
    Likes (Received)
    558

    Default

    Quote Originally Posted by DanielG View Post
    I'm only doing two of them. Unfortunately though, this hole is drilled fairly late in the process, so if the hole is bad, a lot of work is wasted. So I don't really care how long it takes to drill the hole, just that it's right.
    Have you considered a "D" bit?

  7. #7
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,750
    Post Thanks / Like
    Likes (Given)
    1133
    Likes (Received)
    2529

    Default

    Ball sizing might be an option if its thru

    Sent from my SM-G981V using Tapatalk

  8. #8
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    6,598
    Post Thanks / Like
    Likes (Given)
    779
    Likes (Received)
    3919

    Default

    Quote Originally Posted by DanielG View Post
    I'm only doing two of them. Unfortunately though, this hole is drilled fairly late in the process, so if the hole is bad, a lot of work is wasted. So I don't really care how long it takes to drill the hole, just that it's right.
    So I guess if I were doing them:

    center drill
    stub drill
    long drill to finish depth
    ream

    Boy would I be happier if the customer did not want the hole anodized and the finish size is just up to me

    I don't know what it is doing, but I would worry the anodize would vary with depth enough to cause a problem

    Over spec'ed for a bolt not right for a press so dunno, could be a pin they want a slip, who knows

  9. #9
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,825
    Post Thanks / Like
    Likes (Given)
    16888
    Likes (Received)
    12045

    Default

    You are way overthinking this...

    First. You have a tolerance after anodize of 378-381.. Why are you reaming it
    right in the middle when there is going to be buildup.. Go for the high side.
    Then you don't have to worry about it.

    As for drilling it.. Just drill it. I do a ton of expensive castings, and I just
    take it easy.. Where I could punch a hole at .010 a rev if it was just a piece of
    cheap ass bar stock.. On something that has some money it in already.. Take it easy,
    make sure that sucker comes out straight. I'm not going to run max surface speed,
    and max feed to save 30 seconds, when I could take 2 minutes to do it and make 100%
    sure I don't toss $750 casting in the trash.

    I would definitely use a split point. A jobber is almost long enough to get you through,
    Grind a little relief at the top of the flutes, and you'll have enough length. I'd keep
    the surface speed conservative. Maybe 120-150, and the feed at about .003 or .004 a rev,
    depending on how I felt that day.

    To start the hole, a stubby drill, split point of course.. You could even use the jobber,
    just feed her in about .100" at .001 or .0015 a rev or so..

    As for the reaming.. Again.. I play conservative. On something that is going to cost me money
    if it goes oversize, I run 'em slow, and I get very consistent results. My go to on things I can't
    screw up is about 240 rpms.. Regardless of size of reamer, or material.. I'd probably be feeding
    at about .005 or .006 a rev.. And yeah, that's slow.. But it will be consistent..

    I know that all sounds SLOW.. It is.. If its a $4 piece of bar stock, and I have 100 of 'em to do,
    wind it up and punch it. But when the part already has a ton of work into it, or the material/casting
    is going to cost an arm and a leg to replace.. Those are my GoTo #'s.

    I'm also a huge fan of taking a test cut on a separate piece of material that is similar.. Make sure
    your hole making technique is going to give you the results you want.. Even if you just punch a 1x2"
    aluminum soft jaw the 2" direction as a test.. You'll know its going to work, and you're out 5 minutes.

  10. Likes MaxPrairie, AARONT, gustafson liked this post
  11. #10
    Join Date
    Oct 2021
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Have you looked at Iscars line of cham drills? I believe they go that small. Then you would just buy the inserts for whatever material you are cutting. They usually drill a pretty good straight and true hole.

  12. #11
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,287
    Post Thanks / Like
    Likes (Given)
    5880
    Likes (Received)
    4025

    Default

    Quote Originally Posted by DanielG View Post
    It doesn't, however, give speeds and feeds for regular aluminum, just for cast aluminum.
    I'd call or email them, Guhring has pretty good support.

  13. #12
    Join Date
    Jul 2015
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    317
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    114

    Default

    Quote Originally Posted by Bobw View Post
    You are way overthinking this...

    First. You have a tolerance after anodize of 378-381.. Why are you reaming it
    right in the middle when there is going to be buildup.. Go for the high side.
    Then you don't have to worry about it.

    As for drilling it.. Just drill it. I do a ton of expensive castings, and I just
    take it easy.. Where I could punch a hole at .010 a rev if it was just a piece of
    cheap ass bar stock.. On something that has some money it in already.. Take it easy,
    make sure that sucker comes out straight. I'm not going to run max surface speed,
    and max feed to save 30 seconds, when I could take 2 minutes to do it and make 100%
    sure I don't toss $750 casting in the trash.

    I would definitely use a split point. A jobber is almost long enough to get you through,
    Grind a little relief at the top of the flutes, and you'll have enough length. I'd keep
    the surface speed conservative. Maybe 120-150, and the feed at about .003 or .004 a rev,
    depending on how I felt that day.

    To start the hole, a stubby drill, split point of course.. You could even use the jobber,
    just feed her in about .100" at .001 or .0015 a rev or so..

    As for the reaming.. Again.. I play conservative. On something that is going to cost me money
    if it goes oversize, I run 'em slow, and I get very consistent results. My go to on things I can't
    screw up is about 240 rpms.. Regardless of size of reamer, or material.. I'd probably be feeding
    at about .005 or .006 a rev.. And yeah, that's slow.. But it will be consistent..

    I know that all sounds SLOW.. It is.. If its a $4 piece of bar stock, and I have 100 of 'em to do,
    wind it up and punch it. But when the part already has a ton of work into it, or the material/casting
    is going to cost an arm and a leg to replace.. Those are my GoTo #'s.

    I'm also a huge fan of taking a test cut on a separate piece of material that is similar.. Make sure
    your hole making technique is going to give you the results you want.. Even if you just punch a 1x2"
    aluminum soft jaw the 2" direction as a test.. You'll know its going to work, and you're out 5 minutes.
    Agreed. This isn't a big deal to do. Split point cobalts and start with a stubby. Drill 0.368 ream 0.381. Sounds like you are getting hardcoat ano so the 0.381 leaves some room there in case your anodizer falls asleep and leaves them in the tank too long. Just spec a 0.0005/0.0005 hard ano.

  14. #13
    Join Date
    Oct 2014
    Country
    UNITED STATES
    State/Province
    Maine
    Posts
    1,353
    Post Thanks / Like
    Likes (Given)
    268
    Likes (Received)
    646

    Default

    Thanks everyone for the advice. We finished these parts up today.

  15. #14
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    353
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    96

    Default

    Quote Originally Posted by DanielG View Post
    I need a thru hole in 6061, about 3.25" deep, to be .378 -0/+.003 after anodizing. My anodizer says I'll have about .0006 per side, half of that being buildup, so I was going to go for a .3795 hole before anodizing. My current plan is to spot drill, then drill 23/64 thru from one side with a good taper length drill, then ream with a .3795 reamer with plenty of cutting fluid. I can do the reaming in the machine (should I have a special holder for this?) or with a hand drill or drill press.

    I did think about drilling from both ends and then reaming through, but my concern is that they won't be perfectly concentric and the reamer will follow a wandering path.

    For the drill, a Guhring 535 series is readily available. It looks like a good drill and says it's good for non-ferrous and steel, just not stainless. It doesn't, however, give speeds and feeds for regular aluminum, just for cast aluminum. That seems pretty common and confusing. For example, the 5536 says on it's page that it's good for non-ferrous, but then the non-ferrous section is blank on the speeds and feeds document.

    It looks like the best drill for aluminum might be the 501, but it's just for non-ferrous. I'm only doing two of these parts, so if I can buy a more versatile tool and use it again on another project, that would be great.
    One thing I noticed is the grade of aluminum. 6061 is used for extrusion is mealy and it will tend to stick to the drill. A better choice for machining would be an Aluminum in the 2000 series; 2024-T4.

    Roger

  16. #15
    Join Date
    Oct 2021
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    If you have spindle through coolant you could probably use something like this https://www.kennametal.com/us/en/pro...c.6389587.html to just drill the whole length in one pass.

    This insert has a diameter of .374 https://www.kennametal.com/us/en/pro...5.6371039.html


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
  •