reaming holes on the cnc mill (can of worms open) - Page 3
Close
Login to Your Account
Page 3 of 3 FirstFirst 123
Results 41 to 57 of 57
  1. #41
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,436
    Post Thanks / Like
    Likes (Given)
    603
    Likes (Received)
    8472

    Default

    Like Greg White I never indicate a reamer (who has time for that?).
    Also I always leave it hanging out so long is good in my thinking.
    Bob

  2. Likes Tom Lg liked this post
  3. #42
    Join Date
    May 2006
    Country
    UNITED STATES
    State/Province
    California
    Posts
    339
    Post Thanks / Like
    Likes (Given)
    87
    Likes (Received)
    102

    Default

    1. Spot drill for location.
    2. Drill, appropriately undersized, deeper than finished depth
    3. Bore for location and straightness, undersized and to maybe 1/4 finished depth.
    4. To size and finished depth. Stop spindle to retract.

  4. #43
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,805
    Post Thanks / Like
    Likes (Given)
    2369
    Likes (Received)
    1207

    Default

    I just interpolated some +/- .0002" holes on the old Haas. They're as good as we can inspect them.

  5. #44
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,436
    Post Thanks / Like
    Likes (Given)
    603
    Likes (Received)
    8472

    Default

    Quote Originally Posted by mhajicek View Post
    ...... They're as good as we can inspect them.
    This sentence says it all when making holes.

  6. Likes mhajicek liked this post
  7. #45
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    414
    Post Thanks / Like
    Likes (Given)
    161
    Likes (Received)
    164

    Default

    It's a 1/4" hole, 1/2" deep in aluminum, you can stick a blank in the machine and run as many free test holes as you want. Interpolating is a free way to make precision holes if the degree of precision meets your needs. Measuring roundness is a difficulty no matter how we do it.

  8. #46
    Join Date
    Sep 2010
    Location
    Anchorage, Alaska, USA
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    348
    Likes (Received)
    150

    Default

    Hi guys!
    Let me ask the dumbest question of all...
    What are you talking about here... interpolate a hole?
    Honestly... no clue.
    Self-taught CNC machinist, and you guys are about the only buddies I can talk to...

  9. #47
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,436
    Post Thanks / Like
    Likes (Given)
    603
    Likes (Received)
    8472

    Default

    Quote Originally Posted by snowshooze View Post
    Hi guys!
    Let me ask the dumbest question of all...
    What are you talking about here... interpolate a hole?
    Honestly... no clue.
    Self-taught CNC machinist, and you guys are about the only buddies I can talk to...
    Scream and slap down.
    .256 or 2.070 hole. How to make it with a cnc.
    Manual and cnc done the world is so different.
    Bob

  10. #48
    Join Date
    Sep 2010
    Location
    Anchorage, Alaska, USA
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    348
    Likes (Received)
    150

    Default

    Quote Originally Posted by CarbideBob View Post
    Scream and slap down.
    .256 or 2.070 hole. How to make it with a cnc.
    Manual and cnc done the world is so different.
    Bob
    Bob, to interpolate it, you mean just run the end mill around it on the CNC?
    I do bearing fits regularly that way.
    The machines still amaze me. Started out manual.... made the change 10 or so years back...

  11. #49
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,805
    Post Thanks / Like
    Likes (Given)
    2369
    Likes (Received)
    1207

    Default

    Quote Originally Posted by snowshooze View Post
    Bob, to interpolate it, you mean just run the end mill around it on the CNC?
    I do bearing fits regularly that way.
    The machines still amaze me. Started out manual.... made the change 10 or so years back...
    Yes. G2 and G3 are called "circular interpolation", "interpolation" being when the machine closely approximates a curve via a series of closely spaced linear moves. Not to be confused with "point to point" where you tell the machine the series of linear moves. Some machines can interpolate a spline.

  12. Likes snowshooze liked this post
  13. #50
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,246
    Post Thanks / Like
    Likes (Given)
    1303
    Likes (Received)
    809

    Default

    Quote Originally Posted by mhajicek View Post
    ...Some machines can interpolate a spline.
    You mean like our Fadal when interpolating anything faster than 10IPM?

  14. Likes mhajicek liked this post
  15. #51
    Join Date
    Sep 2010
    Location
    Anchorage, Alaska, USA
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    348
    Likes (Received)
    150

    Default

    Quote Originally Posted by mhajicek View Post
    Yes. G2 and G3 are called "circular interpolation", "interpolation" being when the machine closely approximates a curve via a series of closely spaced linear moves. Not to be confused with "point to point" where you tell the machine the series of linear moves. Some machines can interpolate a spline.
    Ah, as I suspected. Something I have been doing a long time, just I wasn't familiar with the nomenclature.
    Thanks!
    Mark

  16. #52
    Join Date
    Sep 2010
    Location
    Anchorage, Alaska, USA
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    348
    Likes (Received)
    150

    Default

    Quote Originally Posted by AARONT View Post
    You mean like our Fadal when interpolating anything faster than 10IPM?
    Are you having problems with your Fadal?
    I have done this regularly on mine with great success, and I learned the speeds and feeds I wanted after a while as when I first started, that 20x40 table was zipping around so fast it worried me I was being brutal to the machine.

  17. #53
    Join Date
    Sep 2010
    Location
    Anchorage, Alaska, USA
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    348
    Likes (Received)
    150

    Default

    Quote Originally Posted by mhajicek View Post
    I just interpolated some +/- .0002" holes on the old Haas. They're as good as we can inspect them.
    Same here with every mill I have tried it on.
    All back-lashes are kept up with... all bearings good. Seems to me to be the only things that could screw it up.

  18. Likes mhajicek liked this post
  19. #54
    Join Date
    Nov 2012
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    2,329
    Post Thanks / Like
    Likes (Given)
    3844
    Likes (Received)
    2876

    Default

    I am sure many will disagree....oh well.
    You and many others dont like to ream (I am assuming) because you have had it fail I get it. There are some cases where you arent gonna be able to reach a .2496" hole with an endmill. (next to a shoulder, bottom of a bore etc). There is obviously a difference when needing 1 or 2 holes vs. needing 1500 holes. There is also a cycle time difference. There again....1 part...who cares....1500???? you are eating into the profit. In my head....reaming is a bit of black art along with a ratio sort of thing. I dont machine alot of aluminum. Mostly toolsteel. In toolsteel....carbide reamer, water soluble coolant, spot drill, drill leaving .01" or so....ream...40SFM .004" to .01" / rev. I dont shut off my spindle and I rapid out of the hole. Could shutting off and / or feeding out make a difference?....I am sure it could but I havent had a need to since the holes are good for a press fit pin. If the hole is o/s....try less RPM, try less feed...try more feed....sometimes a smaller drilled hole will make a bigger reamed hole....sometimes not. If the hole is u/s....well...depends how undersize..try a bigger drill, try a slower feed..Try a higher feed to make it cut more aggressively ..try a higher rpm and slower feed.....
    I have had all these things work....and not.
    Best way to get experience reaming is on a Bridgeport mill.....you can feel whats happening and try to simulate what works.....30+ years of screwing around with reamers and the best I can tell you is you have to do it...and figure it out.
    No substitute for experience
    Yes I know aluminum will ream differently than toolsteel....but the idea is similar.
    Make it work....the day will come when you have no other legit option.
    Good luck

  20. #55
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,805
    Post Thanks / Like
    Likes (Given)
    2369
    Likes (Received)
    1207

    Default

    Yes, very true. If you're making 1500+ of something, it pays to get your process dialed in. For me 30 parts is a long run, so I'd rather use a method that lets me get it right the first time every time at the cost of a little cycle time.

  21. #56
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,246
    Post Thanks / Like
    Likes (Given)
    1303
    Likes (Received)
    809

    Default

    Quote Originally Posted by snowshooze View Post
    Are you having problems with your Fadal?
    I have done this regularly on mine with great success, and I learned the speeds and feeds I wanted after a while as when I first started, that 20x40 table was zipping around so fast it worried me I was being brutal to the machine.
    Aside from the fact it dropped a tool mid cut and trashed the spindle, and it doesn't interpolate for squat? No, everything's gravy.

    Sarcasm aside. Before the spindle got jacked up, it was ok. It's just never been good at interpolating with speed. I just don't like Fadal's. They work fine, but are just too slow and I don't have the patience for it.

  22. #57
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    473
    Post Thanks / Like
    Likes (Given)
    235
    Likes (Received)
    395

    Default

    I don't know much, but I have reamed a few 1/4" holes in aluminum. Spot drill, drill it to .242 with as stubby a drill as you can. Drill it 1/4" deeper than you need to ream. It eliminates chip packing as a concern.

    Ream it at about 50-70 sfm and .006-.008 IPR.

    You can also use A-9 cutting fluid and it will make your hole go under size.

    Then start reaming holes and adjust your speeds and feed to be consistent with your tooling.
    reaming sucks, but it is awesome when it works right.


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
  •