I it ok to run carbide slow?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,005
    Post Thanks / Like
    Likes (Given)
    707
    Likes (Received)
    388

    Default I it ok to run carbide slow?

    Please see the attached picture. I am holding .750" round annealed 4340 in my sub with about .8" stick out. I am using a .375" diameter 4-flute carbide end mill to interpolate a .415" wide slot all the way through the part X .675" deep in Z (multiple passes in Z, btw.) The live em is held in a ER16 collet. At first it was chattering like a son of a bitch. Changing the feed didn't work, but lowering the RPM's on the live end mill sure did. I started at 400SFM and am now all the way down to about 150SFM @ .0025ipt. It sounds great and looks great.

    So here's my Q: Even though it isn't any faster, will the carbide still last longer than HSS when run at the same HSSish parameters? If running carbide that slow is going to ruin it maybe I'll just try an HSS cutter...

    Thank you!

    img_2493.jpg

  2. #2
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,080
    Post Thanks / Like
    Likes (Given)
    1157
    Likes (Received)
    694

    Default

    You're still better off running carbide. It'll be more rigid and last longer.

  3. Likes Limy Sami, Nerdlinger, barbter liked this post
  4. #3
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    19,649
    Post Thanks / Like
    Likes (Given)
    15089
    Likes (Received)
    15254

    Default

    Slow should be fine - and it's often the only solution to a problem - just watch for chipping, IMHO ER16 with a 3/8 cutter sticking out over .675 is pushing rigidity issues, and it's well known the one thing carbide EMs really hate is poor rigidity.

  5. Likes Nerdlinger, Bobw, aj, barbter liked this post
  6. #4
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    3,473
    Post Thanks / Like
    Likes (Given)
    714
    Likes (Received)
    2421

    Default

    150sfm is not too slow, I would expect the carbide to outlast cobalt by 2-3 times in that cut.

    As long as you're not shocking the cutter, it's happy enough. The chattery cut would beat it up a lot faster than a slower speed. 150sfm, it's still cutting free, it's just not making a very plastic chip. You'll leave more of the heat in the material rather than taking it out in the chip, but it's a light cut and you're not generating a lot of heat anyway. A beefier collet would probably help.

    Your ears are telling you this already.

  7. Likes Nerdlinger liked this post
  8. #5
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,559
    Post Thanks / Like
    Likes (Given)
    553
    Likes (Received)
    930

    Default

    In addition to the above mentioned caveats, running too slow MAY lead to a built up edge. Application of the proper cutting fluid will do much to prevent it. Seems to be more of an issue in a lathe.

  9. Likes Nerdlinger, Limy Sami liked this post
  10. #6
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,834
    Post Thanks / Like
    Likes (Given)
    855
    Likes (Received)
    2002

    Default

    Have you tried a variable flute EM? That may help break up the chatter.

    Sent from my SM-G973U using Tapatalk

  11. Likes Limy Sami, MattiJ, Mtndew, Nerdlinger liked this post
  12. #7
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    3,315
    Post Thanks / Like
    Likes (Given)
    11430
    Likes (Received)
    3713

    Default

    Do you have the programming capability to program the slot with a trochoidal path? Would your sub keep up with such a toolpath?

  13. Likes barbter liked this post
  14. #8
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,182
    Post Thanks / Like
    Likes (Given)
    259
    Likes (Received)
    1058

    Default

    Everyone has already answered, but just to add in, no, the slow speed won't hurt the carbide a bit. Most of my machines can't or rarely go above 2k rpm. I rarely run HSS for anything.

    As mentioned you could get edge buildup, but you have a coated endmill, and your running coolant, so I doubt that would be a problem.

    As I am SURE you know, the RPM contributes to the harmonics.

    You could most feed heavier when roughing, .003/.004 ipt at the same sfm if you want to speed the process up, but as mentioned, keep an eye out for chipping. I doubt it will be a problem, what 4340 I have run, is usually great cutting.

    The funny thing about machining and the human brain... if it sounds good... it probably IS good. It is VERY rare that something sounds good, but is bad, and something SOUNDS bad, and is good. Except maybe an inserted high feed mill in tool steel... those just sound BAD.

  15. Likes Nerdlinger, Fancuku liked this post
  16. #9
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    8,918
    Post Thanks / Like
    Likes (Given)
    2141
    Likes (Received)
    6162

    Default

    I'd bet the limitations aren't the collet system, it's the weak spindle geometry and bearings that such close coupling of spindles makes inevitable. A proper milling spindle and ER16 collet system would allow much heavier cuts (I do this with my Haas - wussy for a VMC, but still worlds stiffer than the spindle shown).

  17. Likes AARONT, Nerdlinger liked this post
  18. #10
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,005
    Post Thanks / Like
    Likes (Given)
    707
    Likes (Received)
    388

    Default

    Quote Originally Posted by TeachMePlease View Post
    Do you have the programming capability to program the slot with a trochoidal path? Would your sub keep up with such a toolpath?
    One of my goals is to try this when I have time. I would think there would be a C-axis feed rate limitation but just imagine what it would look like if it worked

  19. Likes TeachMePlease liked this post
  20. #11
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,005
    Post Thanks / Like
    Likes (Given)
    707
    Likes (Received)
    388

    Default

    Thanks for the replies, everyone! So far so good...no identifiable wear after about 45 min of cutting!

  21. #12
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    3,315
    Post Thanks / Like
    Likes (Given)
    11430
    Likes (Received)
    3713

    Default

    Quote Originally Posted by Nerdlinger View Post
    One of my goals is to try this when I have time. I would think there would be a C-axis feed rate limitation but just imagine what it would look like if it worked
    So, just as an FYI, on SOME machines you can adjust a parameter to make the C Axis feed at 100x the programmed feed. Might be something worth looking into.

  22. Likes Nerdlinger liked this post
  23. #13
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    11,286
    Post Thanks / Like
    Likes (Given)
    3863
    Likes (Received)
    3986

    Default

    Having a good sharpening source and pulling at a specified number of parts or wear land can make carbide the better choice,,so avoiding broken cutting edges. Good to have all the same OD in sets if ODs need be ground, so all come back at perhaps .365 after re-sharp...

    I used to run re-sharpen step cutters with grinding the worst facet first .. noting the take off at the first grind ..setting them in rows listed: ..take .010/ take .020 /take .030 and so on ..than the second step I would just take the same with the what row telling the amount.... so cutting sharpening time almost it half on a long run.

  24. Likes Nerdlinger liked this post
  25. #14
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,310
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2671

    Default

    never had a problem running carbide slow. its not slow its a sfpm and feed that works better with
    1) stickout length of end mill
    2) tool holder length
    3) machine rigidity and hp limits
    4) part vibration limits
    ..... a basic chart of feeds and speeds is for short stickout, short and rigid tool holder on a rigid machine with high horsepower available. even a 1" dia end mill if short you can be needing close to 5 hp and putting high cutting forces on part. many a machine has to be limited on feeds and speeds and depth and width of cuts cause its a machine limit or part holding or vibration limit, not a cutter limit. that is problem is coming from machine, tool holder or part more than from the end mill itself.
    .
    many metals are abrasive and carbide last longer usually than hss as long as not breaking the corners off from excess vibration

  26. #15
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    3,315
    Post Thanks / Like
    Likes (Given)
    11430
    Likes (Received)
    3713

    Default

    Quote Originally Posted by DMF_TomB View Post
    never had a problem running carbide slow. its not slow its a sfpm and feed that works better with
    1) stickout length of end mill
    2) tool holder length
    3) machine rigidity and hp limits
    4) part vibration limits
    ..... a basic chart of feeds and speeds is for short stickout, short and rigid tool holder on a rigid machine with high horsepower available. even a 1" dia end mill if short you can be needing close to 5 hp and putting high cutting forces on part. many a machine has to be limited on feeds and speeds and depth and width of cuts cause its a machine limit or part holding or vibration limit, not a cutter limit. that is problem is coming from machine, tool holder or part more than from the end mill itself.
    .
    many metals are abrasive and carbide last longer usually than hss as long as not breaking the corners off from excess vibration

    Tom, tell us about your experience with light duty (comparatively) subspindle lathes?

  27. Likes Mike1974 liked this post
  28. #16
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,310
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2671

    Default

    Quote Originally Posted by TeachMePlease View Post
    Tom, tell us about your experience with light duty (comparatively) subspindle lathes?
    .
    i have worked on many less rigid and low hp machines. and i have had to remill many parts made on subspindle lathes that had so bad chatter vibration marks on them they got sent to cnc mill to remachine the bad spots
    .
    my point and its very basic every machine has rigidity and hp limits. many a machine can take a larger tool in tool holder but not take any where near the limits of what the tool can take. its more a machine limit.
    .
    its like apprentice wants to order a 2.5" carbide insert drill (over $1000.)cause salesman says you can drill 30" per minute. but and its very basic if that drill will need 30 hp and you got a 5hp machine obviously not going to be able to drill at that fast a rate. you will have to drill at a slower rate cause its a machine limit. or its often a part limit too. not every part and holding method can hold against the cutting forces. even if held part vibration can be so bad as to damage cutter in minutes. not a tool limit but more a part and work holding limit
    .
    i obviously use a excel spreadsheet to auto calculate feeds and speeds AND hp and cutting forces. it will indicate by cells going red when i exceed limits like hp. its adjustable cause limits are specific to each machine. so it will not indicate a part or work holding limit as easily but will say hp and cutting forces needed

  29. #17
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    8,626
    Post Thanks / Like
    Likes (Given)
    463
    Likes (Received)
    7079

    Default

    No it won't work, I read it on the internet....
    Built up edge can be a problem but it only occurs in a specific range where the welding occurs. Most users will go faster to get rid of it, you can also go slower which few people want to try.
    There is a sort of no-man's land band in the surface footage chart dependent on a lot of factors in the cut. At a higher temp and speed it will not weld due to chip flow speed, at a lower temp it can't weld.

    Part of this need for speed has to do with the carbide of many decades ago when larger grain sizes and porosity were common.
    The other being that carbide will chip, HSS will not. In manual applications at low speeds often a first contact will be a hit. HSS won't care.
    In 4000 series soft steel I've run micro-grain carbide down as low as 30 SFM.
    At this speed the life over HSS verses cost is indeed questionable.

    All applications are different, in your case I'd want to be just north of 100-150 SFM on the bottom but that does put you in the chip weld area so coatings, coolant and such.
    Bob

  30. Likes Nerdlinger liked this post
  31. #18
    Join Date
    Sep 2016
    Country
    UNITED KINGDOM
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default

    I'd bang a carbide drill in 1st to the remove the meat. Give the endmill more life and speed your endmill up.

  32. Likes Fal Grunt liked this post
  33. #19
    Join Date
    Sep 2016
    Country
    UNITED KINGDOM
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default

    Quote Originally Posted by Paul Hope View Post
    I'd bang a carbide drill in 1st to the remove the meat. Give the endmill more life and speed your endmill up.
    You would get much better tool life. The drill would piss it. The endmill would also smash the remaining material at a much higher speed and feed. Just be change a little bit at the angle of the drill.

  34. #20
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,415
    Post Thanks / Like
    Likes (Given)
    896
    Likes (Received)
    1525

    Default

    Quote Originally Posted by Nerdlinger View Post
    Thanks for the replies, everyone! So far so good...no identifiable wear after about 45 min of cutting!
    That's pretty good for a 3/8" EM in an ER16!


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
  •