Long reach 1/4 endmill in 6061
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Feb 2017
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default Long reach 1/4 endmill in 6061

    I've got a "very" deep feature to make in 6061 Al. The minimum corner radius is .125" and this thing is 3.8" or so down there. Machine is VMC and tool is held in er32 collet/ 40 taper. I purchased some 6" reduced neck 1/4" endmills for the job. 2 flute and for aluminum and all that. Having some problems with chatter. Stickout from the collet is 4". I test ran some slots and .003 DOC at 12k rpm and 154ipm seemed to be doing "ok" (still crappy for my taste) going in conventional. Climb cut started digging in the corners. Anyone have any pointers for running this long length/diameter ratio stuff? I'm roughing out with a larger endmill but I just need to get the smaller diameter one to run a bit better.

  2. #2
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    1,879
    Post Thanks / Like
    Likes (Given)
    539
    Likes (Received)
    943

    Default

    Recent thread, pretty good info;

    .125 ball end mill help

    16x diameter is long ways to go, plunging seems like a decent option. I would get my SFM down from 785, chatter is caused by NOT cutting, just bouncing around, so you need to make the cutter cut.

    R

  3. Likes wheelieking71 liked this post
  4. #3
    Join Date
    Jun 2015
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    983
    Post Thanks / Like
    Likes (Given)
    230
    Likes (Received)
    523

    Default

    Carbide cutters are more rigid. If those are not available in the full length, one could possibly braze a carbide extension to a shorter one.

  5. #4
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    556
    Post Thanks / Like
    Likes (Given)
    796
    Likes (Received)
    308

    Default

    lilerob1 hit it on the SFM issue. The other issue is you're banging into a corner thats the same radius as your cutter. Thats a lot of engagement. If you can find a cutter a little smaller on diameter, that would help as well.

  6. Likes ernieflash liked this post
  7. #5
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,117
    Post Thanks / Like
    Likes (Given)
    2855
    Likes (Received)
    2146

    Default

    154 ipm is way too fast
    I would see about getting some 6mmm tools so the part has a corner radius to swing in the corners.
    Drill close to the corner with a ~.244 drill

    Also I would use multiple tools to get down there first.
    first tool with 1" flute length
    second tool with short flutes necked 2.125
    third tool with 3.375
    fourth tool with your 4" reach

    How many parts to do?
    How wide is the overall pocket?

  8. Likes Hazzert, Limy Sami, wheelieking71, gkoenig liked this post
  9. #6
    Join Date
    Sep 2002
    Location
    gloucester ma
    Posts
    1,525
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    877

    Default

    I cannot say I have had success in this area, but the closest I have come is starting with a shorter end mill and going as far as I can with as small a remainder as possible, then only finishing with the longer end mill. I would probably also try drilling the corners. I think if there is a 7/32 end mill that long it is worth while trying, especially if the accel decel is making it seem to dwell in the corner

  10. #7
    Join Date
    Dec 2007
    Location
    Southeastern US
    Posts
    6,080
    Post Thanks / Like
    Likes (Given)
    652
    Likes (Received)
    2404

    Default

    Another option is to tilt the part 2-5° on a sine plate and use a ball end mill and a surfacing routine to get the engagement down to just a tiny fraction of a plunge or straight cut. Will be slower and you still may have some minor issues at the very corner of the floor depending on what radius is allowed there.

  11. Likes Limy Sami, alexhawker liked this post
  12. #8
    Join Date
    Nov 2001
    Location
    WAPELLO, IA USA
    Posts
    6,396
    Post Thanks / Like
    Likes (Given)
    29
    Likes (Received)
    1788

    Default

    all sfm and feed rules go right in the can on long reach. You have to figure out what your combo likes, and thats machine, holder, cutting tool, and part- yep the part can induce chatter too if its thin wall/ fragile.

    all I can say is try slower than you could ever imagine and see what it does. work up from there.

  13. Likes Bobw, Limy Sami liked this post
  14. #9
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,447
    Post Thanks / Like
    Likes (Given)
    2807
    Likes (Received)
    1993

    Default

    Drill the corners before pocketing?

  15. #10
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,464
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    1004

    Default

    Quote Originally Posted by Mtndew View Post
    Drill the corners before pocketing?
    Yes, this, and if you feel it would be OK with your customer, predrill at the nominal corner location but cheat a bit high on the drill size, maybe a 6.5mm or "F" drill.

    Now having said that, drilling 1/4" x 4" deep is no picnic either . Might need to do it in steps.

    Have you mentioned this to the customer? Sometimes they don't really care that much what the corner radius is and would be OK with either a larger radius or a dogbone corner that gives the same clearance but allows larger tools.

    Regards.

  16. Likes Mtndew liked this post
  17. #11
    Join Date
    Oct 2008
    Location
    north carolina,usa
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    6

    Default

    I use 3 or 4 flt.on the long endmills .They are a lot stiffer than a 2 flt.

  18. #12
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    1,879
    Post Thanks / Like
    Likes (Given)
    539
    Likes (Received)
    943

    Default

    Quote Originally Posted by harley88 View Post
    I use 3 or 4 flt.on the long endmills .They are a lot stiffer than a 2 flt.
    Sorry my friend, but no that is not true. The existing web of a 4 flute Endmill is smaller that the web of a 2 fluter.

    R

  19. Likes wheelieking71 liked this post
  20. #13
    Join Date
    Oct 2009
    Location
    near Seattle, Washington, USA
    Posts
    1,367
    Post Thanks / Like
    Likes (Given)
    283
    Likes (Received)
    734

    Default

    Drill slightly under size in the corners, maybe a "A" or "B" drill. Then finish drill the corner with your long 1/4" end mill with a slow feed rate. They'll look marvelous.

  21. #14
    Join Date
    Feb 2017
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Let me begin by describing the part. It's basically a box with an angled lid from front to back. On the inside of the front face there's some reliefs about .125"ish deep with .125 corners. The only way I've seen to reach this is by setting the box on the front face and coming in from the back. The clearance there is 4.6" or so. (I misspoke in my first post, it's deeper than I remembered)

    So the actual feature I need to do is a profile cut with some .125 corners at a .125 depth 4.6" down inside. Corner drilling won't help me as much because the point on the drill will go to deep and not give me enough clearance in the corners, there's only about .08 wall thickness to the outside face. What I came up with this morning is using a 4 flute on my finish pass at 385sfm and .015 chip load, .01 DOC and only finishing in the corners using trochoidal pocketing. I'm using a larger endmill for the main passes. It gives me a decent finish, not the best but acceptable. I may play with some other options that were suggested to try out something a little faster. I tried all different feeds and speeds this morning and a few different DOC and WOC. 2 flutes were giving me a pretty rough finish no matter what speed I ran it at. The 4 flute seemed to do decent enough. I should be ok with the 4 flute cause it's just a finish pass and shouldn't have to worry about chips clogging it up. I'll just have to get a green wheel and relieve the shank a little cause it was just a regular extra long length one that was laying around.

    There's only 3 of these I have to make so no large production runs. I only work on prototypes so I'm always doing these one off things.

  22. #15
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,117
    Post Thanks / Like
    Likes (Given)
    2855
    Likes (Received)
    2146

    Default

    I do shit like this all the time in prototypes and usually cheat by using a 5 axis machine and a tiny ball em to 3d the corners with it tilted over using a long tool extension.


    Glad to hear your 4 flute is working...

  23. Likes rlockwood liked this post
  24. #16
    Join Date
    Feb 2017
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    5 axis would be pretty sweet to cheat with, but I don't have to do to many parts that would need something like that. Never programmed one either, it'd be fun to learn though.

    Thanks for all the help everyone! Lots of excellent ideas! That's what I love about this line of work, always about 100 ways to skin the cat!

  25. Likes Mtndew liked this post
  26. #17
    Join Date
    Dec 2008
    Location
    LANGLEY, WA
    Posts
    13
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Quote Originally Posted by litlerob1 View Post
    Sorry my friend, but no that is not true. The existing web of a 4 flute Endmill is smaller that the web of a 2 fluter.

    R
    Not necessarily true that web dimensions solely determine stiffness.

  27. Likes sticks liked this post
  28. #18
    Join Date
    Sep 2010
    Location
    Vancouver Canada
    Posts
    613
    Post Thanks / Like
    Likes (Given)
    391
    Likes (Received)
    187

    Default

    This also might be a case where you go back to the designer and point out if they made the corners 1/2" radius it would be much easier/cheaper. If it's a box, chances are that radius dimension is pretty arbitrary and the designer just doesn't know. There's that CAD thing where you radius the vertical corners and the bottom of the edges at the same time with the same number, not realizing that you should design for a bullnose end mill which has a different bottom corner radius than the diameter.

  29. Likes 706jim liked this post
  30. #19
    Join Date
    Jun 2013
    Location
    england-newcastle upon tyne
    Posts
    686
    Post Thanks / Like
    Likes (Given)
    120
    Likes (Received)
    149

    Default

    Drill and ream the corners.Drill then flat bottom and ream.Or phone up and ask the planner if he will allow a concession on the corners can only say no

  31. #20
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,154
    Post Thanks / Like
    Likes (Given)
    1036
    Likes (Received)
    2946

    Default

    Quote Originally Posted by Clonekid54 View Post
    Let me begin by describing the part. It's basically a box with an angled lid from front to back. On the inside of the front face there's some reliefs about .125"ish deep with .125 corners. The only way I've seen to reach this is by setting the box on the front face and coming in from the back. The clearance there is 4.6" or so. (I misspoke in my first post, it's deeper than I remembered)

    So the actual feature I need to do is a profile cut with some .125 corners at a .125 depth 4.6" down inside. Corner drilling won't help me as much because the point on the drill will go to deep and not give me enough clearance in the corners, there's only about .08 wall thickness to the outside face. What I came up with this morning is using a 4 flute on my finish pass at 385sfm and .015 chip load, .01 DOC and only finishing in the corners using trochoidal pocketing. I'm using a larger endmill for the main passes. It gives me a decent finish, not the best but acceptable. I may play with some other options that were suggested to try out something a little faster. I tried all different feeds and speeds this morning and a few different DOC and WOC. 2 flutes were giving me a pretty rough finish no matter what speed I ran it at. The 4 flute seemed to do decent enough. I should be ok with the 4 flute cause it's just a finish pass and shouldn't have to worry about chips clogging it up. I'll just have to get a green wheel and relieve the shank a little cause it was just a regular extra long length one that was laying around.

    There's only 3 of these I have to make so no large production runs. I only work on prototypes so I'm always doing these one off things.
    Even high speed toolpaths don't help much if the endmill radius matches the corner radius. The instant the tool hits the corner, the chipload skyrockets from .015" to .196 per flute (1/4 of the tool circumference) and the rpm doesn't even come into consideration at that instant. So it is essential to use a slightly smaller diameter tool, probably a 6mm would be good, but anything to prevent the tool radius matching the feature radius.

    I'd probably cheat if I had to use the 1/4" tool by creating a mask surface to put in that corner with a .275" radius and see if anybody noticed.


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
  •