Q: Drill diameter for reamed holes.


Page 1 of 2 12 LastLast
Results 1 to 12 of 22

Thread: Q: Drill diameter for reamed holes.

  1. #1
    Registered
    Join Date
    Sep 2004
    Location
    USA
    Posts
    412
    Downloads
    0
    Uploads
    0

    Default Q: Drill diameter for reamed holes.

    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.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Nov 2006
    Location
    USA
    Posts
    382
    Downloads
    0
    Uploads
    0

    Default How I was taught

    If you are over 1/4 inch in diameter (or 5mm). Drill the hole .020 to .030 inches undersize (.5 to .75 mm).
    If you are under 1/4 inch in diameter (or 5 mm). Drill the hole .010 to .015 undersize (.25 to .30 mm).
    The closer the drill to the reemed size the tighter the hole will be. Do not run the reemer in and out of the hole only in and flood it. 1/2 the speed and 2 x the feed for highspeed. flood the coolant.



  3. #3
    Gold Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12176
    Downloads
    0
    Uploads
    0

    Default

    A rule of thumb is that a reamer can remove about 0.5% to about 1.5% of its diameter; for your 6.5mm hole this means the drilled hole will be between 6.48mm and 6.40mm. Stay closer to the larger drill size for small holes because small reamers are not as strong.

    It is possible to force a reamer to remove much more than this but not good practice. Also if you are working with an adjustable blade reamer take even less per pass.

    With blind holes an adjustable reamer cannot be used but even a regular reamer will not ream a blind hole to size the entire depth. The leading end of a reamer has a slight taper and does not cut full size until about 60% of the diameter back from the end.

    A final note with reamers is never, never ever rotate them backwards. If they are intended to cut in a clockwise direction turn them clockwise both going in and out. And don't turn fast and go in slow; run a reamer at maybe 10% of the speed you would drill a hole, use plenty of cutting fluid and feed at up to 10% of the diameter per revolution.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  4. #4
    Registered
    Join Date
    Sep 2004
    Location
    USA
    Posts
    412
    Downloads
    0
    Uploads
    0

    Default

    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.



  5. #5
    Gold Member
    Join Date
    Mar 2006
    Location
    USA
    Posts
    2712
    Downloads
    0
    Uploads
    0

    Default

    For those holes where you can get the correct size end mill, you might grind relief on all but one flute for full depth. Then grind relief above a short portion of the OD "ribbon" on the remaining flute. In effect, you have a single point boring tool for the end mill's diameter. I had a whole drawer full of those in my tool box. They are easy to mount in end mill holders or collets.

    DZASTR


  6. #6
    Registered
    Join Date
    Sep 2004
    Location
    USA
    Posts
    412
    Downloads
    0
    Uploads
    0

    Default

    What about just center drilling with the correct size endmill.

    Do they wander to much, or is there a problem with chips?

    I was looking on mcmaster and they have most of the sizes I need in a center drilling end mill. Rated at +.001"/-.000". Where I think they reamer is rated at +.00019".

    Obviously the reamer would be more accurate, but I can I actually expect to get a 6.5mm +.001" hole with an endmill.

    Sorry if that is a newbish question. Traveling in uncharted waters here.

    Thanks



  7. #7
    Gold Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12176
    Downloads
    0
    Uploads
    0

    Default

    You say "center drilling end mill". Does this mean the cutting end has an end like a spot drill? In other words it would tend to be self-centering when entering the material?

    If this is the case it may be worth trying.

    If it really says "center cutting" chances are it will not work. A center cutting end mill can make a hole from scratch but it will tend to wander around and the hole will not be accurate.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  8. #8
    Registered
    Join Date
    Sep 2004
    Location
    USA
    Posts
    412
    Downloads
    0
    Uploads
    0

    Default

    Center cutting is what I meant.

    I've seen drilling_mills. But that wouldn't help me in this case.



  9. #9
    Gold Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12176
    Downloads
    0
    Uploads
    0

    Default

    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.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  10. #10
    Gold Member
    Join Date
    Mar 2006
    Location
    USA
    Posts
    2712
    Downloads
    0
    Uploads
    0

    Default

    What I was referring to in #5 above was substituting the modified end mill for the reamer or boring tool. Boring feeds/speeds. End mills are not usually ground flat at the tip but have a slight concave angle. That results in a slight convex shape at the bottom of the hole if bored full depth in a blind hole.

    DZASTR


  11. #11
    Registered
    Join Date
    Apr 2008
    Location
    us
    Posts
    3
    Downloads
    0
    Uploads
    0

    Wink reamer

    Hey guys. I was reading this post and though fairly inexperienced, I would like to offer my oppinion, and let you all tell me if I am wrong. lol.
    I would use a fractional drill size smaller than the finall reamed hole. I would convert the metric to standard by multiplying the number by .0394. If the material was hard such as a2 or d2 I would go with the letter size smaller to take it more easy on the reamer. I don't know if I would use an enmill though I mean yes it would work but depending on speed and heat, your hole could still wind up being bigger. Depends on the tollerence, but if there was that much you propably wouldn't be reaming it anyway right. Besides why dullen your end mills when you don't have to. Drill bitts are much cheaper.



  12. #12
    Registered
    Join Date
    Mar 2008
    Location
    USA
    Posts
    240
    Downloads
    0
    Uploads
    0

    Default

    Metric - 0.3 mm under, Inch - 1/64 under.If you want a 6.5 mm reamed hole, drill 6.2, if you drill 6.48 ??- 6.4 you will most likely loose it. Don't forget to cut your speed way down and lubricate. This is gen. shop practice for use in drill press or vertical mill. In a belt driven Bridgebort for reaming speed just switch to "low speed" without changing the belt from the speed you used for drilling
    Blind holes, flat bottom can not be done with a regular reamer. You need an End-reamer like for jigbore use. You will still have a small radius on the bottom. If you cut off a standard reamer you will have to stone a radius on the bottom. Do it in a vise using a triangular oilstone and tooth after tooth stone a light radius with a back up. Do not try to stone a radius on the end while the reamer is turning in a chuck.



Page 1 of 2 12 LastLast

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.