Pulling my hair out trying to helical ramp into 6061 - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 39 of 39
  1. #21
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,509
    Post Thanks / Like
    Likes (Given)
    4108
    Likes (Received)
    2669

    Default

    1) ramp angle is too steep for your end mill
    2) not getting enough coolant

    If you can't turn up the koolmist, get a can of WD-40 and douse the shit out of it while it's entering the pocket. Or a large water bottle filled with coolant and keep it flooded.

  2. #22
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    2,924
    Post Thanks / Like
    Likes (Given)
    212
    Likes (Received)
    2039

    Default

    I do this all day long in 6061, with flood coolant, 3/4 3 flute carbide. Coated, uncoated, no welding ever

    I don't think in terms of angle, but depth per rev, and I think I do 3 or 4 revolutions in 1/2 plate. Not at the machine now...

    [edit]
    39 CC IX+0 IY+0
    40 L IX+0.64 RL FMAX
    41 CP IPA-1080 IZ-0.58 DR+ F600

    7200 rpm, 3/4 inch carbide 3 fl 60 ipm

    That's 3 revolutions in .58. full flood, billion horsepower[for all practical purposes, or Haas rating if you will]
    Last edited by gustafson; 07-24-2019 at 10:32 AM.

  3. #23
    Join Date
    Dec 2012
    Location
    Croatia
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    20

    Default

    Only YG-1 polished carbide endmills - AluPower series. Their HSS for aluminum I have tried, and they were a bit hit n miss at best of times. On the other side, polished carbide without coating is the best. Cant calculate what it is in SFM, but in m/min, I would run insane high surface speed - somewhere around 380 to 550 m/min. Way over catalogue recommendations. And the endmill would work wonderfull at these settings. Also life of the endmill was excellent. Rapming down in holes with helix no problem. The formula for entry is as follows: if the hole is 8 mm, use at maximum 6 mm endmill. So that the center goes well around and doesnt have to cut much itself - no matter that it is center cutting - because actual pressure on the center gives that screeching sound due to instability. Ramp down at 2 degrees in helix, and speed it up, lots of speed. Light chipload, insane high feed and high high high rpm. Like for an 6 mm endmill somewhere around 13000 to 15000 rpm. And a lot of flood coolant. Nothing beats flood on alu.

  4. #24
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    5,723
    Post Thanks / Like
    Likes (Given)
    7122
    Likes (Received)
    7234

    Default

    I have mountains of helix boring experience. My favorite strategy to make odd sized holes.
    I do it every day. Two things:
    You need more coolant. Flood is pretty much mandatory (if you don't have TSC).
    Stick with 5 degrees. That is the sweet spot with YG1's.
    Also, quit trying to avoid the pre-drill. In your situation, you are stepping on your own dick.

  5. Likes Perry Harrington, Delw liked this post
  6. #25
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    533
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    186

    Default

    Quote Originally Posted by wheelieking71 View Post
    Also, quit trying to avoid the pre-drill. In your situation, you are stepping on your own dick.
    What he said

  7. #26
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    158
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    9

    Default

    Wow. And I'm still below 3k rpm capability.

  8. #27
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    146
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    83

    Default

    Maybe I’m off base, and if so I hope I’m corrected promptly, but 10k seems way fast. Chip weld is often indicative of excess spindle speed, and/or too slow of feed. That, and lack of flood.


    Toss your end mills with chip weld in some lye (outside with PPE!!!) for a few minutes and the aluminum will dissolve leaving the cutters looking new.

  9. Likes Bobw liked this post
  10. #28
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,343
    Post Thanks / Like
    Likes (Given)
    1463
    Likes (Received)
    1583

    Default

    Quote Originally Posted by wheelieking71 View Post
    I have mountains of helix boring experience. My favorite strategy to make odd sized holes.
    I do it every day. Two things:
    You need more coolant. Flood is pretty much mandatory (if you don't have TSC).
    Stick with 5 degrees. That is the sweet spot with YG1's.
    Also, quit trying to avoid the pre-drill. In your situation, you are stepping on your own dick.
    I would strongly disagree with this normally. BUT it seems the op has probably wasted 10x more time trying to get it right so ya, just drill a hole... OTOH, I would personally want to get it figured out not having a tool changer...

    I go the other way most of the time, screw spotting and drilling and just ramp/helix pockets, except maybe large LxD small rad corners, then drill if it makes more sense. Of course now most of the pockets I do are with 1/8" endmills so I am not removing much volume...

  11. #29
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,343
    Post Thanks / Like
    Likes (Given)
    1463
    Likes (Received)
    1583

    Default

    Quote Originally Posted by 9finger View Post
    Maybe I’m off base, and if so I hope I’m corrected promptly, but 10k seems way fast. Chip weld is often indicative of excess spindle speed, and/or too slow of feed. That, and lack of flood.


    Toss your end mills with chip weld in some lye (outside with PPE!!!) for a few minutes and the aluminum will dissolve leaving the cutters looking new.
    It is only about 650sfm. Actually probably a little slow (for carbide tools and alum), depending on how rigid your machine and setup are....

  12. #30
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    146
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    83

    Default

    Quote Originally Posted by Mike1974 View Post
    It is only about 650sfm. Actually probably a little slow (for carbide tools and alum), depending on how rigid your machine and setup are....
    I should have worded it better....If 10k seems fast for 40IPM....I only have one 10k spindle, but even on the lower RPM machines, given rigidity is there, my feed in his case would have likely started at 70 and crept up.

  13. Likes Mike1974 liked this post
  14. #31
    Join Date
    May 2006
    Location
    Burlington, North Carolina
    Posts
    370
    Post Thanks / Like
    Likes (Given)
    401
    Likes (Received)
    138

    Default

    Quote Originally Posted by Finegrain View Post
    Just because an endmill is center-cutting (your HSS endmills are center-cutting, right?!?)
    I'm glad someone brought that up. I was thinking the same thing.

  15. #32
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,000
    Post Thanks / Like
    Likes (Given)
    13600
    Likes (Received)
    10613

    Default

    Quote Originally Posted by Mike1974 View Post
    It is only about 650sfm. Actually probably a little slow (for carbide tools and alum), depending on how rigid your machine and setup are....
    The material doesn't care or know what the tool is made out of.. Would the material know if it was the exact same tool made from HSS, or even ground out of piece of hardened bubble gum that you put under your desk in 3rd grade.

    Its all about geometry.

    Of course coatings come into play, but it really is based on how the tool was ground.. Just because its
    carbide does not mean it *HAS* to run fast. Especially if its a nice sharp new tool

  16. Likes WA-CNC liked this post
  17. #33
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    211
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    60

    Default 6061 Aluminum

    Quote Originally Posted by ItsFlipp View Post
    Hey all

    I'm at my wits' end trying to avoid chip welding while helical ramping into 6061. No other issues roughing or finishing, just ramping into pockets. I'm using 1/4" 3 flute at 10k RPM with a 5 degree helix and ramp diameter of .2375" (~95% tool width according to the CAM). I've tried both HSS and ZrN coated end mills, and feed rates of 20 and 40 IPM. Using air blast + koolmist for cooling, but it's clearly rubbing/melting the aluminum and getting welded onto every end mil I try Lowering the helix angle to 2 gives an ear-searing squeal which can't be good...

    Again, works perfectly for other operations; can side mill all day long without issue or heat. Any ideas on what to try next?

    6061 Aluminum is not the best for milling. Its used for extrusion, is mealy and tends to stick to the cutter regardless how the cutter is sharpened. Try reducing the RPM of the cutter while ramping. 3200 rpm. This is not the answer with 6061. Aluminum in the 2000 series would be a better choice for milling.

    Roger

  18. #34
    Join Date
    Oct 2013
    Location
    New Jersey
    Posts
    1,046
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    880

    Default

    So this weekend I spiral milled about 200 13/16” holes in 6105 aluminum and quite few 0.300” holes as well in 6061. Two flute carbide end mill, nothing special. Used my homemade fog buster coolant dispenser and a fairly high air flow to clear chips. Ran all day at about 45 ipm at 16k rpm on my homebuilt weany mill. No chip welding at all. No fog either and the table and chips just slightly damp.

    For some reason 3 flute end mills just seem to like to weld for me. I suspect the chips just pack before they get out.

  19. #35
    Join Date
    Aug 2014
    Location
    California, USA
    Posts
    59
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    47

    Default

    I do 6061 every day. For a 1/4 tool ramp by depth (1x dia) at 9k rpm and 35ipm with flood coolant. Even that is conservative. Consider a roughing tool if you don't mind lines or leave .01 for cleanup. Organize your ops accordingly for minimal toolchanges.

  20. #36
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,509
    Post Thanks / Like
    Likes (Given)
    4108
    Likes (Received)
    2669

    Default

    Quote Originally Posted by rogertoolmaker View Post
    6061 Aluminum is not the best for milling. Its used for extrusion, is mealy and tends to stick to the cutter regardless how the cutter is sharpened. Try reducing the RPM of the cutter while ramping. 3200 rpm. This is not the answer with 6061. Aluminum in the 2000 series would be a better choice for milling.

    Roger
    I dislike when people spout that 6061 isn't the best for milling, I've been cutting it for 30 years.
    It's not bad either. Sure it sticks to the cutter.... if you don't use coolant, cut it with a mister on a bridgeport or any of the other ways that you're not supposed to cut 6061.

    Using that logic people could say that delrin isn't the best for milling.. it tends to melt when using a dowel pin to drill a hole.

  21. Likes Mike1974, wheelieking71, WA-CNC, Vancbiker liked this post
  22. #37
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,343
    Post Thanks / Like
    Likes (Given)
    1463
    Likes (Received)
    1583

    Default

    Quote Originally Posted by Bobw View Post
    The material doesn't care or know what the tool is made out of.. Would the material know if it was the exact same tool made from HSS, or even ground out of piece of hardened bubble gum that you put under your desk in 3rd grade.

    Its all about geometry.

    Of course coatings come into play, but it really is based on how the tool was ground.. Just because its
    carbide does not mean it *HAS* to run fast. Especially if its a nice sharp new tool
    I am confused. I guess *it* doesn't know, but I know. I wouldn't use hss tooling on hardened D2, no matter what grind/geometry it has.

    True carbide does not have to run fast, but it sure can run fast in aluminum. Why not use it and make the chips as fast as possible?

  23. #38
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    I looked and if I were programming this ramp, I'd be at 10k rpm 20.5 ipm about 650 sfm .0007ipt for the ramp diameter. I generally don't go much over 4 deg but as long as your endmill is center cutting you theoretically can plunge straight in. I don't generally like to ramp much deeper than 1.5xD because clearing out chips much deeper than that becomes an issue. Do you see the chips being evacuated and is there a change when you hit a certain depth?

  24. #39
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    5,723
    Post Thanks / Like
    Likes (Given)
    7122
    Likes (Received)
    7234

    Default

    Quote Originally Posted by rogertoolmaker View Post
    6061 Aluminum is not the best for milling. Its used for extrusion, is mealy and tends to stick to the cutter regardless how the cutter is sharpened. Try reducing the RPM of the cutter while ramping. 3200 rpm. This is not the answer with 6061. Aluminum in the 2000 series would be a better choice for milling.

    Roger
    HUH?! "Aluminum is not the best for milling" WTF you talking about?
    6061 is about the easiest material there is to deal with when it comes to "milling".

  25. Likes WA-CNC, Perry Harrington, Mtndew liked this post

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
  •