Help: What is the proper manufacturing method for machining a reamerd hole?!
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Feb 2020
    Country
    UNITED KINGDOM
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Question Help: What is the proper manufacturing method for machining a reamerd hole?!

    Hi fellow machinists!

    I know that the rule of thumb for a reamed hole is to drill out prier to the reamer i.e. drill size ~2% less than the reamer size.

    My question is! Can you use an end mill to machine out this hole instead of a drill?


    Kind Regards,
    Taylor

  2. #2
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    20,695
    Post Thanks / Like
    Likes (Given)
    16117
    Likes (Received)
    16551

    Default

    Yawot? .....I'm a bit lost here.

    A hole is a hole - as long as it's within tolerance and spec - how you machine (as opposed to laser etc etc) it prior to reaming doesn't matter.

  3. #3
    Join Date
    Nov 2003
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5,607
    Post Thanks / Like
    Likes (Given)
    194
    Likes (Received)
    1900

    Default

    I don't see why you couldn't. Or wire EDM it. Or bore it. Or whatever.

    Heck, you could pull an Elmer Fudd and boast the hole with a shotgun and then ream it. Or a Clint Eastwood and use a 44 magnum. Or .....

    That 2% is not real cut and dry. In many hole sizes you will be hard put to find a drill bit that is 2% smaller. You want to remove at least a few thousandths so that the imperfections of the drilling process do not remain, more for larger holes. But 5% smaller or even more may be dictated by the exact numbers involved.

    Most reamers have cutting edges on their nose, just like drill bits do. They are usually at about a 45 degree angle and they extend only a small percentage of the radius of the reamer. So, the drilled hole should be large enough so that these cutting edges are doing the actual enlargement and you are not just forcing the core of the reamer into the material.

    Also the amount of chips created should be kept to a minimum so that they do not build up in the flutes and start digging into the walls of the hole as happens with drill bits. There is where that 2% probably comes from.



    Quote Originally Posted by Taylor96 View Post
    Hi fellow machinists!

    I know that the rule of thumb for a reamed hole is to drill out prier to the reamer i.e. drill size ~2% less than the reamer size.

    My question is! Can you use an end mill to machine out this hole instead of a drill?


    Kind Regards,
    Taylor

  4. Likes Taylor96 liked this post
  5. #4
    Join Date
    Feb 2020
    Country
    UNITED KINGDOM
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Hi Limy,

    Thanks for your responce. I have an order that has came in that requires multiple H7 holes. I was just enquiring about a good working practice for machining out reamed holes i.e. one hole required a 50mm reamed hole and this tool is very expensive, approx £300. So to ensure that the machining is done correct to prevent tool failure. Tool material is HSS

    Regards,
    Taylor

  6. #5
    Join Date
    Feb 2020
    Country
    UNITED KINGDOM
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thanks EPAIII that was a very helpful responce! Very detailed and well explained. I will taking your advise into consideration when programming for these H7 tolernace holes!


    Kind Regards,
    Taylor

  7. #6
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    20,695
    Post Thanks / Like
    Likes (Given)
    16117
    Likes (Received)
    16551

    Default

    Quote Originally Posted by Taylor96 View Post
    Hi Limy,

    Thanks for your responce. I have an order that has came in that requires multiple H7 holes. I was just enquiring about a good working practice for machining out reamed holes i.e. one hole required a 50mm reamed hole and this tool is very expensive, approx £300. So to ensure that the machining is done correct to prevent tool failure. Tool material is HSS

    Regards,
    Taylor
    For a 50mm hole (as in a 1 odd or few) I'd bore it, ..a 50mm reamer takes a lot of driving.

  8. #7
    Join Date
    Oct 2005
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    19,554
    Post Thanks / Like

    Default

    Your profile says "CNC programming" I would suggest circular interpolating the hole with an endmill (center cutting)
    Last edited by digger doug; 02-24-2020 at 08:28 AM. Reason: "er" to "ing"

  9. Likes jrmach liked this post
  10. #8
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,679
    Post Thanks / Like
    Likes (Given)
    2251
    Likes (Received)
    2827

    Default

    Quote Originally Posted by Limy Sami View Post
    Yawot? .....I'm a bit lost here.

    A hole is a hole - as long as it's within tolerance and spec - how you machine (as opposed to laser etc etc) it prior to reaming doesn't matter.
    Yes it does if you need to hold position and size...

    OP, you need to bore or interpolate the top portion of the hole (how deep depends on size IMO) to get your position correct. A 'regular'* reamer follows the undersize hole, so if the drill walks a bit the reamer will too.

  11. Likes Limy Sami liked this post
  12. #9
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    20,695
    Post Thanks / Like
    Likes (Given)
    16117
    Likes (Received)
    16551

    Default

    Quote Originally Posted by Mike1974 View Post
    Yes it does if you need to hold position and size...

    OP, you need to bore or interpolate the top portion of the hole (how deep depends on size IMO) to get your position correct. A 'regular'* reamer follows the undersize hole, so if the drill walks a bit the reamer will too.
    I gave you a like, but in my reply I did state as long as it's within tolerance and spec .....................and in my book that includes both position and size.

  13. #10
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    12,298
    Post Thanks / Like
    Likes (Given)
    4153
    Likes (Received)
    4400

    Default

    A drill with a pre-drill (smaller) hole will cut to the micrometer check size of the last drill ( + a few tenths).. just drilling a hole with not a pre-drill it may cut oversize. A drill with a point .020 off center point would likely cut to your reamer diameter size. A drill hole may also cut a tad off spindle center.
    A center cut gash end mill would cut at the spindle center line of your spindle but would/may cut oversize to the amount of run out, so one would need consider run-out spotting the location..
    A reamer most often will follow the drill (hole) spot location.
    Careful bore or interpolate would allow adjusting the location and size.

  14. #11
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,679
    Post Thanks / Like
    Likes (Given)
    2251
    Likes (Received)
    2827

    Default

    Quote Originally Posted by Limy Sami View Post
    I gave you a like, but in my reply I did state as long as it's within tolerance and spec .....................and in my book that includes both position and size.
    Yes, you did. I made an assumption about the OP simply because he asked for the 'proper' method to ream a hole.... I am trying to imagine a scenario where the hole size is critical (at least enough to ream, but that's another conversation), but position is not - ie good enough to just drill and ream without some operation to ensure the hole is on position.

    I tried searching for jig reamers, maybe that is not the correct term? Anywho, they can be used directly after a drill because they are end cutting, eliminates an operation.

  15. #12
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    12,298
    Post Thanks / Like
    Likes (Given)
    4153
    Likes (Received)
    4400

    Default

    A jig bore reamer has a very stout shank so the spindle bore is better followed. They need a stout machine to provide location/spot and a little dewell at the entering is good. IMHO

  16. #13
    Join Date
    Sep 2004
    Location
    Rugeley UK
    Posts
    1,031
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    114

    Default

    When you are dealing with a small but deep hole that must be reamed, a boring bar may be apt to follow a drilled hole rather than bore true. My solution is to drill a small hole, follow with a 4flute endmill under reaming size, drill reaming size and ream.
    The endmill will true up the deviation in the hole from the initial drill wandering off centre,you are not concerned about it being slightly off centre as it will 'mill' the bore back on centre.
    The whole process is faster than using a boring tool because the feed rate is higher because the boring bar in these very small diameters will flex.
    This has worked well for me for years.
    Peter

  17. #14
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    9,474
    Post Thanks / Like
    Likes (Given)
    520
    Likes (Received)
    7871

    Default

    Quote Originally Posted by EPAIII View Post
    .....
    Most reamers have cutting edges on their nose, just like drill bits do. They are usually at about a 45 degree angle and they extend only a small percentage of the radius of the reamer. So, the drilled hole should be large enough so that these cutting edges are doing the actual enlargement and you are not just forcing the core of the reamer into the material.
    Ever measure the heel clear on that 45 leadin on the nose?
    May look like it but these are not drill tips.
    Bob

  18. #15
    Join Date
    Nov 2003
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5,607
    Post Thanks / Like
    Likes (Given)
    194
    Likes (Received)
    1900

    Default

    Really? I have a collection of dozens and every one has clearance on those cutting edges.

    Just two examples, first a 0.4000", factory sharpened:



    The clearance is mostly radial, not along the length of the reamer. But it IS THERE. Those are cutting edges.
    Another, smaller one (0.1868"):



    Again, the clearance is mostly radial and it is a bit harder to see here due to the smaller size. But, again those are cutting edges. Just like drill's cutting edges.

    If you look at these two reamers or most of the others in my collection from the side you will not easily see any clearance. It is a radial clearance and that is not like a drill bit. But it is real clearance and those edges can bite and cut into the material surrounding the hole.

    Taper reamers, as sold in hardware stores, with a range from 1/8" to 1/2" and that are intended to enlarge holes in sheet metal, are intended to cut on the outer edges of the flutes. But machine reamers, like these, which are intended to cut a hole to an exact size will have the exact same diameter all the way down to the tip. They are intended to cut on these 45 degree edges.

    Oh, BTW if you look close at the first photo, you can see the same lands that drill bits have on the outer edges of the flutes. These lands are there to prevent any cutting action there. They really are intended to cut ONLY on those small, 45 degree edges at the nose. They probably exist on the smaller one also but are harder to see. OK, I just checked with my pocket magnifier and yes, they are there on the small one too.



    Quote Originally Posted by CarbideBob View Post
    Ever measure the heel clear on that 45 leadin on the nose?
    May look like it but these are not drill tips.
    Bob

  19. #16
    Join Date
    Nov 2003
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5,607
    Post Thanks / Like
    Likes (Given)
    194
    Likes (Received)
    1900

    Default

    BESIDES, reamers are fed DOWN, like drill bits. Not sideways like milling cutters. You don't even want them to cut sideways as that would enlarge the hole.

  20. #17
    Join Date
    Aug 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    140
    Post Thanks / Like
    Likes (Given)
    137
    Likes (Received)
    52

    Default

    Taylor, for what it's worth, the guys in the Tesla shop I used to work with would pretty much interpolate everything. We would spec h7 all the time, it was probably the most common tolerance our team used. The shop would interpolate the holes and check fit on the machine with plug gauges. Never had a problem.

    The only times it ever presented an issue is when that tolerance would be called out on deep, small diameter holes (e.g. 5mm x 20mm). Tool deflection would result in an ever-so-slight taper towards the bottom of the hole that would be noticable when installing pins. This was pretty much always done just because it was faster to throw a tolerance on a thru-hole without considering the manufacturing side. In almost all of the cases drawings were revised to only specify the tolerance on maybe a 1xD portion. Deeper than that was rarely necessary.


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
  •