Pulling my hair out trying to helical ramp into 6061
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 39
  1. #1
    Join Date
    Feb 2019
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default Pulling my hair out trying to helical ramp into 6061

    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?

  2. #2
    Join Date
    Apr 2004
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,290
    Post Thanks / Like
    Likes (Given)
    6756
    Likes (Received)
    1003

    Default

    Drill an entry hole.

  3. Likes aj liked this post
  4. #3
    Join Date
    Feb 2019
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Sure, that's what I'm doing as a band-aid patch now but that requires at least one tool change for every pocket (no ATC on my machine, just power drawbar). I gotta imagine it's possible; I'm probably just overlooking something or using a bad setting...?

  5. #4
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,962
    Post Thanks / Like
    Likes (Given)
    1591
    Likes (Received)
    1847

    Default

    At 10k rpm I would be feeding more like 70-90. BUT I doubt that is really the problem, I would bet it is because it is 6061 without flood coolant. Can you 'turn up' the koolmist so you are getting a nice watery blast of air/coolant? Also, make sure it is adjusted so it is reaching the tool at final depth (which you should specify for us to help). The 5deg might be a bit aggressive depending on endmill grind, I normally default to 2-3deg, which might be a little sissy, but no problems.

  6. Likes Pete Deal, primeholy, Ox liked this post
  7. #5
    Join Date
    Feb 2019
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Huh. I normally side cut at ~78-ish, but had read that you typically slow down during ramping since it's essentially a full width cut (?). I can try even more coolant, but last night I was at the point where calling it "minimum quantity lubricant" might be a bit of a misnomer The pocket is .7" in total, but I take little steps of .2" each time. I can try turning it down to 2 degrees, but I've noticed some pretty significant squealing when entering last time I tried that which I assumed was the end burnishing instead of cutting. I've confirmed that the end mills I've tried are center cutting, but is there some other type of geometry I should be looking for in the grind that would make certain end mills unsuitable for ramping?

  8. #6
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,254
    Post Thanks / Like
    Likes (Given)
    200
    Likes (Received)
    1590

    Default

    Use an AL-specific endmill like Destiny Diamondback/Viper or YG-1 Alu Power. Just because an endmill is center-cutting (your HSS endmills are center-cutting, right?!?) doesn't mean the center cutting action will be "good".

    In 6061, I helix in @ 16,000 RPM x .001" - .006" chipload depending on endmill size (1/8" - 1/2"), 3-flute endmills. Never saw any chip welding unless I forgot to turn on the (flood) coolant, then the endmill clogs up when helixing in once it is well and truly into the bore.

    I suspect your relatively light chipload is making powdery wispy swarf that is packing in.

    Regards.

    Mike

  9. #7
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,962
    Post Thanks / Like
    Likes (Given)
    1591
    Likes (Received)
    1847

    Default

    Quote Originally Posted by ItsFlipp View Post
    Huh. I normally side cut at ~78-ish, but had read that you typically slow down during ramping since it's essentially a full width cut (?). I can try even more coolant, but last night I was at the point where calling it "minimum quantity lubricant" might be a bit of a misnomer The pocket is .7" in total, but I take little steps of .2" each time. I can try turning it down to 2 degrees, but I've noticed some pretty significant squealing when entering last time I tried that which I assumed was the end burnishing instead of cutting. I've confirmed that the end mills I've tried are center cutting, but is there some other type of geometry I should be looking for in the grind that would make certain end mills unsuitable for ramping?
    I don't ever slow down ramping. I don't think the "full width cut" really applies since you are only moving axially .xxx per rev (I'm not going to figure the math LoL)... And to be clear, you said you tried HSS and Zrn, is the Zrn coating on a carbide tool? 10k rpm is way too fast IMO for HSS....

    .70 deep, what is your flute length? What is the ext/projection from holder? What is the holder (er collet, solid, R8... since you mentioned power drawbar)? This will have an effect too.

    edit: for the record, I regularly use 1/4" 3 flute Zrn coated carbide endmills, .75-1.00 LOC, in aluminum using .003" ipt and 500'ish sfm (around 8k rpm). So I don't think my params are off, although they might be a little light.....

  10. #8
    Join Date
    Jul 2011
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    34
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    32

    Default

    I usually drop the RPMs when helical ramping to up the chipload. 4K RPM seems to be the happy zone for a 1/4" standard lg EM on my machine at a ~3deg ramp, but it feels like it could definitely be pushed steeper than that. The reason it screams is because only a short segment of the EM is engaged in the cut, so the upper portion of the flutes isn't stabilized - same reason people have issues with long reach EMs. Since it's effectively slotting with such a short LOC, it's gonna get mad at you unless you give it a bigger bite so the vibrations don't have a chance to develop in the first place. Try 40 IPM at 4K RPM instead of 10K and you'll probably have a better time, especially if you reduce the ramp angle.

  11. Likes Bobw liked this post
  12. #9
    Join Date
    Feb 2019
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Funny you mention the YG Alu... just wrecked one last night via chip welding (were you referring to this one?).

    You might be onto something with the wispy swarf... when I used the 2 degree helixes I almost never see chips; just looks like the metal disappears (albeit with the gnarly squealing), which I assume is the super tiny chips being blown away immediately. I've been hesitant to use much higher than a .0015-.002 chip load as it seems most manufacturers suggest ~.0017" IPT. Do higher chip loads affect the chances of chipping/breaking a flute tip?

  13. #10
    Join Date
    Feb 2019
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Quote Originally Posted by Mike1974 View Post
    I don't ever slow down ramping. I don't think the "full width cut" really applies since you are only moving axially .xxx per rev (I'm not going to figure the math LoL)... And to be clear, you said you tried HSS and Zrn, is the Zrn coating on a carbide tool? 10k rpm is way too fast IMO for HSS....

    .70 deep, what is your flute length? What is the ext/projection from holder? What is the holder (er collet, solid, R8... since you mentioned power drawbar)? This will have an effect too.

    edit: for the record, I regularly use 1/4" 3 flute Zrn coated carbide endmills, .75-1.00 LOC, in aluminum using .003" ipt and 500'ish sfm (around 8k rpm). So I don't think my params are off, although they might be a little light.....
    Interesting... well, maybe I'll try a full speed ramp, as terrifying as that is to me.

    Ya, the ZrN ones are carbine, and the HSS was the YG-1 Alu Power I linked to above. Flute length is .75, tool stickout is ~1.2" (can measure at home), ER20 collet into an R8 PDB. Machine is a Tormach 770M; definitely no Matsuura, but it's got plenty for 6061 so far.

    What machine do you run those settings on? Pretty similar settings to what I use normally, though I don't tend to take quite as big DoC (usually 0.3" side cuts) since my machine isn't nearly as rigid as larger machines. I know that doesn't exactly maximize tool life, but I seem to be killing end mills faster than they can wear down

  14. #11
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,962
    Post Thanks / Like
    Likes (Given)
    1591
    Likes (Received)
    1847

    Default

    Those are settings on a Haas, 10k max spindle. Cat40 side lock holder.

  15. #12
    Join Date
    May 2005
    Location
    CA
    Posts
    1,130
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    287

    Default

    ItsFlipp,

    Are your pockets large enough that you could try ramping back and forth in a straight line? (I'm assuming you are spiraling down currently).

    PM

  16. Likes Bobw liked this post
  17. #13
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,049
    Post Thanks / Like
    Likes (Given)
    212
    Likes (Received)
    656

    Default

    Gw Shultz alumagators will go right in there no problem check them out
    Don


    Sent from my iPhone using Tapatalk Pro

  18. Likes Cycle1000 liked this post
  19. #14
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,154
    Post Thanks / Like
    Likes (Given)
    707
    Likes (Received)
    1144

    Default

    Your ramp radius is .2375 and your depth is .200 per helix?
    That’s way more than 5 deg. I’d say that’s where your problem is.
    Try about .05 depth per helix.

  20. #15
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,050
    Post Thanks / Like
    Likes (Given)
    13923
    Likes (Received)
    10721

    Default

    My 2 cents..

    5 degrees is pretty steep, what is the actual relief on the end of your endmill???

    If I have the choice. I'd rather ramp than helix. Just personal experience.
    Ramp, step over, ramp back.. you have a lot more room to get coolant in and
    get chips OUT.

    If you are melting down, there are 2 possibilities. You are rubbing (5 degree helix),
    or you are recutting chips.. Also a meltdown can occur if you are taking tiny little
    itty bitty cuts.

    I'd drop the spindle speed, and drop the helix angle. Neither one of those things
    gets it done faster.. But how much time do you have to save to pay for your
    broken cutters??

  21. #16
    Join Date
    Oct 2006
    Location
    Klamath Falls, Oregon
    Posts
    3,640
    Post Thanks / Like
    Likes (Given)
    418
    Likes (Received)
    1008

    Default

    I'm gonna take a stab and say you are doing this on a Tormach 440 and don't have flood coolant. I used to do a lot of Aluminum with Kool-mist and a Shizuoka AN-S.

    Chip welding is just a thing you're gonna have to live with, with Kool-mist. The best way I found to avoid this was to drill a starter hole in the center of where the endmill has to plunge.

    Second, I used the largest endmill practical, for me it was 2fl HSS 3/4" EM. The 2fl gives more room for the chips, the HSS was because the Z axis wasn't very rigid on the AN-S and it would eat carbide endmills.

    I would also make the Kool mist extra concentrated, they might have an AL formulation.

    But the best thing to prevent this was going to an enclosed HAAS with flood coolant. Nothing will beat flood coolant.

    I stepped down to 1/2 endmills, running 3fl carbide Destiny endmills and Blaser flood coolant, worked like a charm and was soo much faster.

    Fogbuster makes an MQL system that looks better than a mister, and it uses conventional coolant like Blaser. Kool mist is crap IMHO, Blaser is way more slippery and gives a better finish. Just switching to a Fogbuster with a good coolant could solve your problem, but flood is a no-brainer solution.

  22. #17
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    206
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    104

    Default

    Before i got my brothet, I had a Novakon (similar to tormach) and tried the kool mist.its pretty useless other than light peripheral milling. Really sucks drilling etc in aluminum.i spent a lot of time making a high flow flood coolant system and all the welding problems went away.

  23. #18
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,679
    Post Thanks / Like
    Likes (Given)
    847
    Likes (Received)
    2541

    Default

    Have you tried hand applying some extra lube? An acquaintance has an open knee mill with some kind of a mist unit. He has learned to spray some WD40 while ramping. Best solution is to get a real machine with flood coolant.

  24. Likes kenton liked this post
  25. #19
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    3,564
    Post Thanks / Like
    Likes (Given)
    2000
    Likes (Received)
    1297

    Default

    Coolant Coolant Coolant and drop your ramping angle to 2 degrees

  26. Likes primeholy liked this post
  27. #20
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    30
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    7

    Default

    My sweet spot at ramping is 2 degrees. However, I dont cut a lot of aluminum nowadays. I cut mainly 1018,4140 pre, h13, d2, and some others. Oh, and stellite. I hate stellite.


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
  •