Q: Drill diameter for reamed holes. - Page 2


Page 2 of 2 FirstFirst 12
Results 13 to 22 of 22

Thread: Q: Drill diameter for reamed holes.

  1. #13
    Registered
    Join Date
    Apr 2008
    Location
    us
    Posts
    3
    Downloads
    0
    Uploads
    0

    Default

    I use a drill that is .0156"-.0312" smaller than the reamer.
    The material being cut is also a large factor, as well a feeds and speeds.
    Make sure that your center drill leaves a slightly larger chamfer than the reamer size.
    In plain 1018 CRS steel I would use 300-400 rpm and a high feed .018" per. rev. for the larger drill size (.015") and a 4-6 flute carbide tip reamer, about 15-20 percent less feed for a HSS reamer. The higher feed insures a straighter, tighter hole size. Non-ferrous materials use abit faster RPM and about the same feed ratio.



  2. #14
    Registered
    Join Date
    Apr 2008
    Location
    us
    Posts
    3
    Downloads
    0
    Uploads
    0

    Default

    Also, I know this sounds crazy, but I have actually reamed a dead on hole size in non ferrous materials with a spiral flute bottom tap, in a rigid collet chuck feeding at a slow feed. The teeth on th tap act like a bunch of very precision cutting edges. Works great in aluminum. Nice finish to.



  3. #15
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by jefilomeno View Post
    Also, I know this sounds crazy, but I have actually reamed a dead on hole size in non ferrous materials with a spiral flute bottom tap, in a rigid collet chuck feeding at a slow feed. The teeth on th tap act like a bunch of very precision cutting edges. Works great in aluminum. Nice finish to.
    And when you discovered this little tidbit, were you intending to ream the hole or thread the hole?

    It does sound like a heck of an idea, better than using an endmill, because the upper body of a tap is not relieved, so it will burnish the hole, yet the contact is minimal, and coolant flow should be good.

    Plus, the rake angle of the spiral flute will give a nice positive cutting action compared to the dumb scraping of a straight flute machine reamer.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  4. #16
    Registered
    Join Date
    Apr 2008
    Location
    us
    Posts
    3
    Downloads
    0
    Uploads
    0

    Thumbs up Reaming with a spiral flute tap...

    I was actually tapping a pretty deep hole, so I wasn't using the tapping cycle. The problem was getting coolant to the bottom and so I wrote a peck-tap cycle to reciprocate in and out but not comming out of the hole completely as to keep the threads timed correctly. Well as most of you know FEED HOLD dosen't work in a tapping cycle until the tap comes out. Not the case in just a standard G01. So, the tap stopped mid cut and just turned while inside the hole. The spiral is on a tight helix so it was like dozens of little boring bar edges polishing the hole to .250" As I investigated my screw-up, it came to end happily with a new found, as you said tidbit. And there you have it...
    Quote Originally Posted by HuFlungDung View Post
    And when you discovered this little tidbit, were you intending to ream the hole or thread the hole?

    It does sound like a heck of an idea, better than using an endmill, because the upper body of a tap is not relieved, so it will burnish the hole, yet the contact is minimal, and coolant flow should be good.

    Plus, the rake angle of the spiral flute will give a nice positive cutting action compared to the dumb scraping of a straight flute machine reamer.




  5. #17
    Registered
    Join Date
    Nov 2011
    Location
    United States
    Posts
    25
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Deviant View Post
    Yea I figured the tip of the hole wouldn't get reamed.

    Normally I'd use a boring bar, but 6.5mm, is a tiny hole.

    Maybe I'll try grinding down a boring bar.

    Thanks for the tips.
    Deviant
    6.5mm converts to .256 (English) of course you can ream it. I don't see the problem.
    Flat bottom the hole using a 4 flute center cutting 1/4" carbide end mill (rough the hole with a 15/64 if needed though I doubt it), go as deep as the tolerance allows. Don't use a 2 flute, use a 4 fluted end mill, it will not distort due to torque and most end mills are designed .001/.002 smaller to allow for deflection, but with a straight cut down deflection is not a problem. with the right speed and feed I doubt you could get a .2500 pin gauge into the hole.
    Now, take the reamer, .2559 (.256) and grind off all but .010 of it's lead, that's plenty to guide the reamer, and if your at the top of your tolerance with the milled hole your reamed hole can be within .005 of the required depth.
    It takes some finesse since reamers can cut both over and under their stated size, so practice on scrap of similar material, low RPM and as aggressive a rate of feed as the tool allows.
    Now it's up to you, adjust from there.



  6. #18
    Registered
    Join Date
    Nov 2011
    Location
    United States
    Posts
    25
    Downloads
    0
    Uploads
    0

    Default

    Deviant
    You mean center cutting not center drilling.
    See my last reply to your question ^_^



  7. #19
    Registered
    Join Date
    Nov 2011
    Location
    United States
    Posts
    25
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Geof View Post
    Here is a really crude suggestion...that does work.

    Get a used 2 flute end mill the correct size, but not too used, all you want is the initial really razor sharp edge taken off.

    Take it to an oilstone or if you don't have this some fine emery paper held flat on something solid and hone a tiny radius on the corners of the cutting edges; tiny means a few thousands of an inch, .010 to .015.

    Drill your hole undersize like you would for reaming, you should be spotting it with a spot drill and you can take this deep enough to leave a small chamfer.

    Now go in with your modified end mill almost like you would with a reamer, slowish rpm and fastish feed. The dulled and rounded cutting edges hold the end mill centered in the hole. There will be a little radius at the bottom of the hole from the dulled corners but that is unavoidable.
    That's good Geof
    If my comments were not six years behind yours, we could have taught each other a thing or two.



  8. #20
    Registered
    Join Date
    May 2010
    Location
    Australia
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default Re: Q: Drill diameter for reamed holes.

    Quote Originally Posted by Deviant View Post
    I have a few blind holes that I'm looking to drill out with flat bottoms.

    Can anyone tell me what the rule of thumb is for determining the drill size prior to reaming.

    I.e.

    6.5mm hole reamed.

    What drill bit should I use?

    Additionally, I'm looking to ream 12.5 and 14.5 mm.

    Thanks for any help.
    Use Percentage rule IE 98% of drill size, or if bigger 96%



  9. #21
    Registered gmenzies's Avatar
    Join Date
    Nov 2015
    Posts
    20
    Downloads
    0
    Uploads
    0

    Default Re: Q: Drill diameter for reamed holes.

    Quote Originally Posted by Deviant View Post
    I have a few blind holes that I'm looking to drill out with flat bottoms.

    Can anyone tell me what the rule of thumb is for determining the drill size prior to reaming.

    I.e.

    6.5mm hole reamed.

    What drill bit should I use?

    Additionally, I'm looking to ream 12.5 and 14.5 mm.

    Thanks for any help.
    Here is what I do.


    If I am using a manual mill or radial arm drill. I never move the table or head until I finish spot drill/drill/ream each hole
    On the cnc we have a hard coded all drill operations to feed to the hole position from the same direction. eliminates any backlash issue

    spot drill first ( new tool) use dwell three revs
    Drill hole peck with dwell ( 2 to 4 % smaller ) always use a new drill. -- no hand sharpened tools allowed
    Ream Peck feed depth at least 2 to 4 X diameter ( coolant only)

    stick to the feeds and speeds of the material.
    carbide reamers follow same rules

    if a hole requires a extremely tight tolerance we will usually hand lap or wire EDM

    If your really concerned. test on a scrap piece.

    when reaming 1/32 and 1/16 we order coated reamers and drills from vendor

    one last thing -- use collets-- No drill chuck

    Cheers Gord



  10. #22
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    2743
    Downloads
    0
    Uploads
    0

    Default Re: Q: Drill diameter for reamed holes.

    hmmm... not bad... back to life after 11.5 years after 1st post.



Page 2 of 2 FirstFirst 12

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Q: Drill diameter for reamed holes.

Q: Drill diameter for reamed holes.