Making a deep hole with good finish and accuracy
Close
Login to Your Account
Results 1 to 19 of 19
  1. #1
    Join Date
    Mar 2005
    Location
    India
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Making a deep hole with good finish and accuracy

    I have to make a hole of Dia 13.5mm and 68mm deep in Aluminium 6082. The finish required is 0.8 Ra max.

    I am doing bigger holes on CNC lathe with carbide boring bars. But this one seems to be challenge as I will have to use a 8mm Carbide boring Bar would mean L/D ratio of 8.5 Times. This results in chattering.

    I am thinking of doing this hole on a VMC. But I am not sure about the tools to use! Maybe a Drill of 13.25mm followed with a boring bar. Or maybe a PCD drill?

    Wohlhaupter sales person is not confident that it is possible on their holders even with carbide boring bar and not not seem to have a solution.

    So I guess it may have to be PCD Drill.

  2. #2
    Join Date
    May 2005
    Location
    CA
    Posts
    846
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    127

    Default

    Use a larger boring bar or reduce the tip radius on the cutting edge to near nothing. Preferably both.

  3. #3
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,443
    Post Thanks / Like
    Likes (Given)
    2802
    Likes (Received)
    1990

    Default

    Is it a blind hole? Might want to try feeding left to right for the finish.
    Do you have the budget to buy a carbide dampened bar?

  4. #4
    Join Date
    Nov 2011
    Location
    UK
    Posts
    103
    Post Thanks / Like
    Likes (Given)
    37
    Likes (Received)
    16

    Default

    Slow the spindle speed down.


    Sent from my iPhone using Tapatalk

  5. #5
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    919
    Post Thanks / Like
    Likes (Given)
    219
    Likes (Received)
    513

    Default

    Positive rake insert = less cutting pressure.

  6. #6
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    5,553
    Post Thanks / Like
    Likes (Given)
    115
    Likes (Received)
    2120

    Default

    I am lost here, it isn't even 10x diameter deep. Why not just drill and ream for the finish requirement?

  7. Likes yardbird, Limy Sami, apestate, Steveo liked this post
  8. #7
    Join Date
    Nov 2011
    Location
    UK
    Posts
    103
    Post Thanks / Like
    Likes (Given)
    37
    Likes (Received)
    16

    Default

    Use a 10mm boring bar. That needs a minimum bore size of 12mm so you have plenty of clearance.


    Sent from my iPhone using Tapatalk

  9. #8
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    16,364
    Post Thanks / Like
    Likes (Given)
    11935
    Likes (Received)
    11307

    Default

    Quote Originally Posted by Dualkit View Post
    I am lost here, it isn't even 10x diameter deep. Why not just drill and ream for the finish requirement?
    That was my reaction, ......but I didn't post as the R word seems kinda dirty on the CNC forum.

  10. #9
    Join Date
    Jun 2015
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    978
    Post Thanks / Like
    Likes (Given)
    229
    Likes (Received)
    512

    Default

    Very light cut on the finishing pass(es)?

  11. #10
    Join Date
    Aug 2003
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    47
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    4

    Default

    +1 for Gobo & precisionmetal

  12. #11
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    5,553
    Post Thanks / Like
    Likes (Given)
    115
    Likes (Received)
    2120

    Default

    Quote Originally Posted by Limy Sami View Post
    That was my reaction, ......but I didn't post as the R word seems kinda dirty on the CNC forum.
    You can ream faster than boring and you don't have to worry about galling in soft aluminum from chips getting packed around a boring bar. No brainer to me unless you are making a one off and you don't have a reamer in stock, but plenty of boring bars.

  13. Likes Limy Sami liked this post
  14. #12
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,065
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1343

    Default

    Hi matoind:
    I've seen some amazing results from bog-standard coolant through carbide drills...better for size control and finish than I would have believed to be possible.
    I'd talk to a Guhring technical sales rep and see if they can make a recommendation for you.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    www.vancouverwireedm.com

  15. #13
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    919
    Post Thanks / Like
    Likes (Given)
    219
    Likes (Received)
    513

    Default

    Quote Originally Posted by Limy Sami View Post
    That was my reaction, ......but I didn't post as the R word seems kinda dirty on the CNC forum.
    I gotta agree. It just seemed like such an obvious answer, I suspected a trap.

  16. #14
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    5,553
    Post Thanks / Like
    Likes (Given)
    115
    Likes (Received)
    2120

    Default

    Quote Originally Posted by Gobo View Post
    I gotta agree. It just seemed like such an obvious answer, I suspected a trap.
    Maybe the metric numbers have baffled some of the USA contingent here. It amazes me how many machinists can't convert metric numbers to inches in their head. The last place I worked for the man almost everybody but me had either a small calculator (most people didn't have cell phones then)or a decimal equivalent chart in their pocket.

  17. #15
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,125
    Post Thanks / Like
    Likes (Given)
    8658
    Likes (Received)
    2489

    Default

    Quote Originally Posted by Dualkit View Post
    Maybe the metric numbers have baffled some of the USA contingent here. It amazes me how many machinists can't convert metric numbers to inches in their head. The last place I worked for the man almost everybody but me had either a small calculator (most people didn't have cell phones then)or a decimal equivalent chart in their pocket.

    .03937

    For rough conversions on the fly, I just use .040.

  18. #16
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    795
    Likes (Received)
    307

    Default

    Quote Originally Posted by TeachMePlease View Post
    .03937

    For rough conversions on the fly, I just use .040.
    I prefer 25.4 myself. To each his own.

  19. #17
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    2,970
    Post Thanks / Like
    Likes (Given)
    1206
    Likes (Received)
    625

    Default

    I would be leery of reaming the hole, IF you only have 1 shot at the part.
    Reaming is a crap shoot, at best, if you have no experience with the exact same part/material/tooling/ machining strategy, etc....

    Without notes or previous experience, I can foresee any/ all of the following:
    Bell mouthed hole
    Over/undersize issues
    retract lines (scratches) from the reamer
    wondering hole

    I love reamers, but when I NEED absolute control over a NEW process; always the boring bar.....

    To the OP, if you have some setup parts, and or some extra material, DEFINITELY try a reamer.
    Drill a 33/64" and follow it up with a LH sprial, RH cut reamer. If you can get coolant through the reamer, it will be a snap!

    Doug.

  20. #18
    Join Date
    Mar 2003
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    1,054
    Post Thanks / Like
    Likes (Given)
    49
    Likes (Received)
    12

    Default

    hole is .5315" depth is 2.677", microfinish 125 ra.

    Buy a 13.1 drill if you're getting oversize holes. if not 13.2mm (.520) then ream it 13.5.

    buy a brand new chucking reamer and lovingly dull the corner at the chamfer with a "reamer stone" or equivalent

    Make sure drilled hole looks like 13.2mm

    Throw some of that green tapping fluid for aluminum on the reamer with an air gun

    ream it at 50 rpm and 15.25 mm/min (.012" / rev) feed

    increase feed rate & speed for a little bigger hole

    bore in - bore out, don't rapid out or you'll yank the part out of the vise

    and if the finish comes out ugly, have a 13.5mm ball bearing ready and press it through ...

    wait, is this a blind hole or thru hole?

  21. #19
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    22,528
    Post Thanks / Like
    Likes (Given)
    3091
    Likes (Received)
    6045

    Default

    Finish is 32


    Is there a reason that you can't use a reamer? (BTW - that is 17/32 inche in Western civilization)

    Is it blind?

    Does it need to have sqr bottom?


    I for one would NOT go with a LH spiral reamer unless it's a through hole. (we are in the "CNC" forum, so I'm expecting that this is not a Manuel opperation that needs the LH twist)

    I also would NOT stand it up and bore it in a mill if it is blind.

    If a reamer is possible, I would use a floating holder to help it stay on size and negate those nasty pull-out marks that you were warned about prior.

    If you need a sqr bottom in a blind hole, I have had endmills altered with through coolant (apparently a "hole popper" is the ticket for this. Many folks with wire EDM's will have this.) The coolant through will help to flush the chips out. I have had good luck with this in 6061.


    disclaimer
    I have no experience (knowingly anyhow) with this flavour or alum.


    ------------------------

    Think Snow Eh!
    Ox


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
  •