Guide to Reaming Holes
Close
Login to Your Account
Page 1 of 4 123 ... LastLast
Results 1 to 20 of 63
  1. #1
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    108
    Post Thanks / Like
    Likes (Given)
    37
    Likes (Received)
    27

    Default Guide to Reaming Holes

    Hi!

    I have some holes to ream and every time I have ever reamed holes in the past (once or twice), they have always come out oversize. Does anyone know of a "guide to successful reaming"? I couldnt find one using the search.

    Or if anyone would be so helpful to write a quick step by step guide, do's and donts etc, I would massivley appreciate the help.

    Thanks in advance!

    P.S Im reaming a 6mm H7 hole in mild steel.

  2. Likes awalker25 liked this post
  3. #2
    Join Date
    May 2018
    Country
    ALAND ISLANDS
    Posts
    71
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    17

    Default

    Well it all depends on the purpose of the reamed hole. My preference has been drill under 1/32 depending on material and job maybe inturp with a endmill .1 dp. 100/150 sfm .0005/.0025 C. L. Depending on diameter. Also look into under/over reamers. If you're reaming in a drill press try light pressure with cutting oil. Heavier feed may increase hole size.

    Sent from my SM-G950U using Tapatalk

  4. #3
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    3,276
    Post Thanks / Like
    Likes (Given)
    1396
    Likes (Received)
    4259

    Default

    can't even figure out where to start. More details, please

  5. #4
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    108
    Post Thanks / Like
    Likes (Given)
    37
    Likes (Received)
    27

    Default

    Quote Originally Posted by Larry Dickman View Post
    can't even figure out where to start. More details, please
    Let me know what details you need and ill provide them

  6. #5
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,320
    Post Thanks / Like
    Likes (Given)
    1961
    Likes (Received)
    838

    Default

    Basic (read: minimum needed) steps to ream a +-.0005" hole

    1) spot the hole with the appropriate angle, spot drill
    2) follow that with a drill that is about 0.015" less than the desired reamer size.

    **(this is more a percentage of the drill size, but 0.015" is a good start)
    ***(there is probably someone who will chime in with "general rule of 6%", and another member who will regale us all with the stated use of spread sheets, notebooks, 100 Ton parts, and 8' long boring bars..... Please ignore him)***

    3) choose speeds / feeds (material dependent)
    4) feed into the hole
    5) stop the spindle, at the bottom
    6) G1 retract from the hole (G00/ rapiding out of the hole sill sometimes grab the lands, and pull the reamer out of the collet some.)

    The above is the basic (minimum) needed.
    If you want to be really accurate, you could include boring the hole in between the drill and the reamer, to assure location, and roundness.
    The better the preparation of the hole, the better the end result.

    Having said that, I HATE REAMING!
    It is a crapshoot at best. Especially when you only have 1 or 2 holes/ parts.....

  7. Likes jancollc, AARONT, NAST555, KristianSilva, Ox and 3 others liked this post
  8. #6
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    3,276
    Post Thanks / Like
    Likes (Given)
    1396
    Likes (Received)
    4259

    Default

    Quote Originally Posted by KristianSilva View Post
    Let me know what details you need and ill provide them
    what kind of reamer are you using? A good, sharp high quality reamer, or some piece of shit you found in a box?

    Did you indicate the reamer in? (Probably the most important step)

    What do you call o/s? .0001" or .0200"

    Coolant/ Oil?

    Speed, feed?

  9. Likes tteitgen liked this post
  10. #7
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    11,648
    Post Thanks / Like
    Likes (Given)
    3978
    Likes (Received)
    4145

    Default

    I like to chamfer the drill hole for a close size reamer need, leave about .010 to ,016 stock for the reamer, do it
    in a drill press, mill, lathe or mag base drill, blow out the hole, use some tap ease, spindle oil or coolant, feed slow so it does not heat up..be sure sharpening is done between centers or in a holding bushing so all flutes are in the cut..

    Reamers are hard to measure because flutes may not be exact apart from each other..they can ream a few millionths off the measure..and can go big with a long run from getting hot/warm.

    Grinding or lapping OD size it is good to turn the reamer from the heal side to go to the cutting side, that places the grinding crash/chatter on the heal so not causing a fail edge at the cutting edge of the flute.

  11. #8
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,343
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2681

    Default

    Quote Originally Posted by KristianSilva View Post
    Hi!

    I have some holes to ream and every time I have ever reamed holes in the past (once or twice), they have always come out oversize. Does anyone know of a "guide to successful reaming"? I couldnt find one using the search.

    Or if anyone would be so helpful to write a quick step by step guide, do's and donts etc, I would massivley appreciate the help.

    Thanks in advance!

    P.S Im reaming a 6mm H7 hole in mild steel.
    .
    1) most reamers have runout and you get a bellmouth or tapered hole til its in the hole enough to steady reamer to lower runout. usually let reamer stick out enough to allow it to flex
    .
    2) when dry the metal can form bue or built up edge of material causing false cutting edge a larger diameter. generally you can easily get different sizes depending on dry or if cutting oil or coolant used
    .
    3) at too high a rpm vibration can cause larger hole. hardness variations also with straight flute reamers can cause a lobed hole effect of hole not round. spiral flute reamers can help with some materials
    .
    4) reamers come in different sizes. you can easily get a reamer .001" smaller when you want a press fit and .001" oversize when you want a sliding fit

  12. Likes KristianSilva liked this post
  13. #9
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    11,648
    Post Thanks / Like
    Likes (Given)
    3978
    Likes (Received)
    4145

    Default

    We had some very high precision reamers that had no flutes exactly apart.. they came from vendor to our print with a wide stub at the heal of one flute for inspection..then we had to TC grinder or by hand grind off that stub to use them.

    Had reamers we would place in an adjustable lapping hole and back turn them with compound to make exact OD side.

  14. #10
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,196
    Post Thanks / Like
    Likes (Given)
    4770
    Likes (Received)
    3146

    Default

    Quote Originally Posted by KristianSilva View Post
    Hi!

    I have some holes to ream and every time I have ever reamed holes in the past (once or twice), they have always come out oversize. Does anyone know of a "guide to successful reaming"? I couldnt find one using the search.

    Or if anyone would be so helpful to write a quick step by step guide, do's and donts etc, I would massivley appreciate the help.

    Thanks in advance!

    P.S Im reaming a 6mm H7 hole in mild steel.
    Reaming is a fickle art. And the best teacher is experience to be honest.
    Runout is a big factor in holding size as well as rpm and feedrate.
    One thing to keep in mind is that on some reamers that are brand new, they might have an "edge" from the factory. Meaning that it could be too sharp. Sometimes we take a small stone and lightly hone the cutting edges before using a new reamer.

  15. Likes michiganbuck, Rewt, KFALCON954 liked this post
  16. #11
    Join Date
    Jan 2003
    Location
    Canada
    Posts
    11,401
    Post Thanks / Like
    Likes (Given)
    5771
    Likes (Received)
    3520

    Default

    Depends, but usually, drill, bore for straightness if its picky(not always necessary), chamfer the edge, then ream as final step.
    It's the best way to ensure a round straight hole that stays on location.
    I ream as a very last resort if I really can't just easily bore it on size/depth.

  17. #12
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,633
    Post Thanks / Like
    Likes (Given)
    1208
    Likes (Received)
    672

    Default

    If none of these posts have helped you, nice write up by the way Doug, then look up username litlerob1 here on the forum. He loves reaming and I am sure that he will tell you how efficient reaming is

  18. Likes Mtndew, doug925, yardbird, rjs44032 liked this post
  19. #13
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    11,648
    Post Thanks / Like
    Likes (Given)
    3978
    Likes (Received)
    4145

    Default

    Guess one might ask if the problem/difficulty is consistent in size for a job run using the same reamer..or from one reamer to another reamer.

    Often .0002" back taper of OD can make a resharpened reamer smaller diameter..also a good way to change the size as needed.

    One can ream a hole in a block..split the block with a 1/32" parting wheel.. add a closing drill and tap needed to provide adjusting the size..then with compound in the hole and turning the reamer backwords la the reamer to 6 to 12 millionths of size.

    What is H-7.. about .00045 I think...if so that is a wide tolerance for reaming.

    like mtndew said: {take a small stone and lightly hone the cutting edges before using a new reamer.]
    also with a lopp to see or just eyeball one can put a small corner bevel with a hone to make size hold better/often tighter..

    We used to lighty wire brush HSS lathe bits to break them in, I know you cant do that with a reamer with not messing up th OD.

  20. #14
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    10,238
    Post Thanks / Like
    Likes (Given)
    1396
    Likes (Received)
    3696

    Default

    Quote Originally Posted by KristianSilva View Post
    Hi!

    I have some holes to ream and every time I have ever reamed holes in the past (once or twice), they have always come out oversize. Does anyone know of a "guide to successful reaming"? I couldnt find one using the search.

    Or if anyone would be so helpful to write a quick step by step guide, do's and donts etc, I would massivley appreciate the help.

    Thanks in advance!

    P.S Im reaming a 6mm H7 hole in mild steel.
    Buy a few different reamers around the nominal diameter you need, like half a thou under, and half a thou over, and one right on nominal dimension. This will help ensure that the nominal reamer behaves and reams right on size. It knows if you bought the other reamers and won't behave if it is by itself, something to do with quantum mechanics and the way that you can't measure something and know where it is at the same time. So the reamer in the drawer that you know is undersize transposes itself into your toolholder of the one you think you know the size of, but can actually know it is in the spindle. But the one in the drawer....is it really there?

  21. Likes mhajicek, Bobw, Hazzert, imc188222, mountie and 3 others liked this post
  22. #15
    Join Date
    Dec 2004
    Location
    uk
    Posts
    14,053
    Post Thanks / Like
    Likes (Given)
    4552
    Likes (Received)
    6711

    Default

    IMHO run out should not overly matter on a HSS reamer of these sizes, secret is you want as much stick out as you can so its some what floppy. Then don't baby it, feed it at least 2x as fast as a drill bit but at only half or less of the spindle speed.

    Ream like you don't care at the above speeds and feeds is how i get the best out of them, before then i babied em and they just chattered and made a mess. There self guiding with lots of flutes, so they want feed and to self guide they need to get in the work and get to there job, slow hole entry is tomb DMF's true cause for the bell mouthed holes. Again chucked up tight and fed slow and they start to cut over sized, stuck out further so they can flex a little and fed hard enough they are doing there job and suddenly reaming becomes easy!

  23. Likes Mtndew, doug925, Ox, david n, imc188222 and 1 others liked this post
  24. #16
    Join Date
    May 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    207
    Post Thanks / Like
    Likes (Given)
    135
    Likes (Received)
    81

    Default

    The key for our shop is to keep runout minimal and make sure the reamer is hitting a good hole. We use precision carbide drills (YG Inox) and Morse carbide reamers, held in Schunk hydraulic holders. This keeps runout absolutely minimal.

    With this setup you generally do not need a spot drill, although it never hurts - just make sure the tip angle is the same or broader than your drill angle (hence why a lot of spot drills are 142 degrees).

    Our drills are .2mm under the reamer size (.008).

    We have good results reaming H7 tolerances for the most part, although it can still be tricky at times.

    And the last thing, feed rates can get ridiculous. I think I have a 3mm reamer set to feed at like... .012 IPR for steel. A lighter feed rate seems to cause the holes to taper more, and be bigger at the top.

    Although it was a hard battle to fight, we were able to demonstrate successful reaming to the company's owner, who insisted on jig-grinding any H7 hole. We get a lot more work now without that extra 30 minutes per hole, hahaha...

  25. Likes imc188222 liked this post
  26. #17
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    11,648
    Post Thanks / Like
    Likes (Given)
    3978
    Likes (Received)
    4145

    Default

    If using that same size often and could order perhaps 12 reamers then order to the size that fits the part.
    Perhaps .00017 to .0002 smaller than you want the hole.
    Here one top shop for making reamers to your specs. Special drill and reamer Corp.

    Tell them Buck recomended their shop (agree they may not rember me)

    307 Temporary Redirect

    *Oh, You are from the UK..so find a good tool and cutter manufacturing shop in the UK..catalog cutteres are all over the map fpr size.

  27. #18
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,320
    Post Thanks / Like
    Likes (Given)
    1961
    Likes (Received)
    838

    Default

    Quote Originally Posted by NAST555 View Post
    If none of these posts have helped you, nice write up by the way Doug,
    Thanks!
    Quote Originally Posted by NAST555 View Post
    Then look up username litlerob1 here on the forum. He loves reaming and I am sure that he will tell you how efficient reaming is
    HAHAHAHA!!!!

  28. #19
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,419
    Post Thanks / Like
    Likes (Given)
    897
    Likes (Received)
    1540

    Default

    Oversized holes often means you're spinning too fast and feeding too slow. It could also mean the predrilled hole is too big.

    I like to predrill undersized and interpolate with an endmill before reaming. Interpolated holes are more likely to be on-location, on-size, and round than a merely drilled hole. Tweaking the interpolated hole size via wear offset can affect the reamed dimension. Of course this only works on relatively shallow holes.

  29. Likes kevin66, KFALCON954 liked this post
  30. #20
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    108
    Post Thanks / Like
    Likes (Given)
    37
    Likes (Received)
    27

    Default

    Quote Originally Posted by Larry Dickman View Post
    what kind of reamer are you using? A good, sharp high quality reamer, or some piece of shit you found in a box?

    Did you indicate the reamer in? (Probably the most important step)

    What do you call o/s? .0001" or .0200"

    Coolant/ Oil?

    Speed, feed?

    Thanks for all the advice!

    I am using a high quality WNT 6mm HSS machine reamer, they recomend running at 630 RPM and feeding at 190mm/min, also before reaming I will be drilling to 5.8mm dia, so 0.2mm reaming allowance on dia.

    I will be using a precision holder and collet that are rated to 2 microns runout and I will be using coolant.

    I dont know what you mean when you say "What do you call o/s? .0001" or .0200"?

    Does this sound like a reasonable setup??

    In this case positional tolerance isnt critical, the dowel is a single dowel to stop something moving, if there was a tight position tolerance I would interpolate for better accuracy.


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
  •