584,871 active members*
5,561 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking > MetalWork Discussion > Tips for milling copper anyone ?
Results 1 to 17 of 17
  1. #1
    Join Date
    Dec 2003
    Posts
    40

    Tips for milling copper anyone ?

    I've been trying to mill some .125" copper sheet with my CNC Sherline mill. I have tried 1/8" and 1/4" end mills, increasing rpm, decreasing rpm, slowing down the feed rate and I still am having no end of problems. Besides the really big burrs, I find that the end mill wants to really dig in quite often and of course then the software looses it's place and I end up with more scrap metal. I'm cutting fairly light passes of .010" and my next thought is to decrease even that.

    I could sure use some guidance here.
    David J. Morrow

  2. #2
    Join Date
    Sep 2005
    Posts
    86
    Quote Originally Posted by DJ Morrow
    I've been trying to mill some .125" copper sheet with my CNC Sherline mill. I have tried 1/8" and 1/4" end mills, increasing rpm, decreasing rpm, slowing down the feed rate and I still am having no end of problems. Besides the really big burrs, I find that the end mill wants to really dig in quite often and of course then the software looses it's place and I end up with more scrap metal. I'm cutting fairly light passes of .010" and my next thought is to decrease even that.

    I could sure use some guidance here.
    Sounds like you need to increase your feed rate. If you are getting big burrs, you are not getting rid of the heat fast enough. Coolant, either mist or flood will help too. Also, make sure you are using sharp end mills.

  3. #3
    Join Date
    Oct 2004
    Posts
    4
    I have been machining a good bit of copper (and silver) this week as well. I agree with the boost in RPM.
    I have been running .125" carbide 2 flute endmills at 3000rmp and a feedrate of about 2 - 3 ipm cutting at a depth of .025" and no coolant. This has produced very nice cuts. I am however using a much bigger mill...hope that helps.
    RMJ

  4. #4
    Join Date
    Jan 2005
    Posts
    224

    Wink

    A "trick" I heard about years ago:
    Put a piece of dry ice on the part.

    Colder is better when machining copper.

    Good luck,
    Pres

  5. #5
    Join Date
    Apr 2003
    Posts
    10
    I have read in Guy Lautard's, a fellow Vancouverite, Third Bedside
    Reader that milk works good on copper. I have not tried this myself but it might help. He suggests just bruhing it on.

    Good Luck,
    Vern

  6. #6
    Flood Coolant And Left Handed Endmills Is The Answer.
    L.S. Tool & Precision Inc.
    Taking machining to the
    next level, combining creativity, ingenuity and the technology of CAD/CAM & CNC Machining
    “When ingenuity makes all the difference”
    http://hometown.aol.com/lstool1/myhomepage/business.html

  7. #7
    Join Date
    Nov 2004
    Posts
    18

    Reduce the cutting dept

    Use small cuts and a lot of coolant. :violin:

  8. #8
    Join Date
    Dec 2005
    Posts
    25
    Try Using A Roughing Carbide Endmill And Heavy On The Coolant Mix

  9. #9
    Join Date
    Aug 2005
    Posts
    92
    Copper and its alloying elements are incredibly abrasive. Use sharp carbide mills, replace them often, and keep the flute count down, i.e. 2 instead of 4, and get the rpm as high as your machine can allow. Use a fairly shallow cut, but don't just skim the part with the end of the tool because that will dull the tool and work-harden the surface. I have milled 1/8 copper (101 oxygen free and 110) with a 1/8" carbide endmill at 4000 rpm, 1/16" deep. Getting the chips away from the cutter is the single most important thing you can do as the chips will be work-hardened to a point much harder than the base stock. Re-milling the hardened chips is hell on even carbide cutters. I would try a good water-soluble cutting oil mixed a little on the heavy side (about the appearance of whole milk, and a slippery feel between the fingers) in a fairly high-pressure air-mister. Crank the air pressure up to get the chips out of the way. Yes, you will get some discoloration of the copper by the coolant, especially if it stands on the copper for any length of time. Yes, you will get a shop full of mist which isn't the nicest thing for sinuses. Open a window and use a fan to blow the mist outdoors if need be. Or invest in a mist collector. You will make better parts this way. I forgot to add that the mist will help dissipate any heat that develops, but copper conducts heat so well that this shouldn't be a serious problem.

  10. #10
    Join Date
    Jul 2003
    Posts
    10

    Smile angle of cut

    A mill or drill in brass or copper will act like a wood screw, tapping in and grabbing. One solution to this is to use a low helix mill where the flutes look more like a reamer than a mill. The fellow who suggested dry ice is on the right track. This makes the metal more brittle so that the chips will break off instead of grabbing. About twenty years ago a machinist at GE here was killed when trying to drill a 4 inch hole in copper. The drill grabbed, pulled the part from the chuck and killled the operator. My disasters have been less eventful, thank heaven. I nearly destroyed a $3000 cooling jacket one afternoon trying to drill a 1/16" hole without switching drills, and I knew better! After 3 hours of peening the jacket back in shape, a low helix did the trick.
    Custom CNC Software - ACME Profiler,
    Bar Code Engraving, rapid prototyping
    Promoting CNC ballistic excellence

  11. #11
    Join Date
    Jan 2006
    Posts
    7
    i have always had good luck with vanilla flavored HSS or Cobalt e-mills 2flute of course, replacing them often. They have a sharper edge than carbide and cut cleaner. Lots of coolant and like everyone else said keep the chips out of the way.

  12. #12
    Join Date
    Feb 2005
    Posts
    3
    Does a negative rake mean anything?. I was taught to almost blunten the drill for Copper, Brass and Ali. Also used Parafin/Keroseen for Small stainless holes.

  13. #13
    Join Date
    Oct 2005
    Posts
    14
    I used to CNC end mill multiple 18" long 1/8" wide slots about .100" deep (1pass!) in ally sheet 1/4" thick about 15 by 24 area, clamped down all around the edges. Std 2 flute Hss or carbide mills would snap off. The problem is the cutters are too long & weak, centre of the cutter is too strong, the flutes too small causes build-up & welding of ally into the cutter ie crowds up the soft sticky swarf. SO... I cut away one flute altogether to make a single flute cutter, this allows the special aluminium flood coolant to get in & the swarf to get out, the feedrate was able to stay the same or even faster! The chip per tooth was twice or more but the cutter would take it OK. You also shorten the end to leave the strongest mill you can. On bigger diameter cutters you just back off everything you can around the tip area, into the centre &2nd relief behind, & felt buff polish the top raked flutes with an air grinder. When plunging in to make pockets, use side feed as well to "ramp"-down. This leaves a slope for the coolant to get in & flush. Soft copper is sticky like ally & behaves much the same.
    The idea of LEFT hand spiral cutters is good, in that it pushes your thin sheet job downwards onto the table etc so if your job is being grabbed UPwards this negative spiral will stop it, & you don't get a raised burr up top, but you then have negative rake, possibly pushing the swarf down onto the bottom. LOOK at your cutter after any problem, if it has metal welded into it its telling you to try the above solution. Some cutters are sold especially for cutting soft metal. Single flute cutters can be bought or made specially. If you buff polish the carbide surface that the chip slides over (rubbing & trying to weld on), to a mirror shine & then re-sharpen the end to get razor edge back, you can even mill dry! Free machining grade copper is available, I think it has sulphur in it. We used this for edm electrodes, although edm wear is a bit higher.
    Highest revs you can, .002" per tooth max feedrate, heaps of special aluminum flood coolant, or spray mist that won't harm your health if you inhale the fog!

  14. #14
    Join Date
    Jan 2005
    Posts
    224
    Quote Originally Posted by fredhh47
    ... I would try a good water-soluble cutting oil mixed a little on the heavy side (about the appearance of whole milk, and a slippery feel between the fingers) in a fairly high-pressure air-mister..
    I agree!
    In fact, after 50+years of machining experience, a mist coolant system is almost always the best way to cut any metal, IMHO.

    Using an inexpensive Shop-Vac, with the hose close to the cutter, gets most of the vapor extracted. A foam filter, inside the cannister, catches alot of the vapor.
    If you want it all out, put a hose on the exhaust side of the Shop-Vac and run it to an outside vent/window.

    Of course, a good quality electrostatic filter will trap all of it but that is rather expensive (e.g. Smog-Hog)

    Flood cooling works ok, but it is so messy that I won't use it anymore.

  15. #15
    Join Date
    Apr 2006
    Posts
    65
    I don't quite understand why everyone is recommending a two-flute end mill and high RPMs. Wouldn't a four flute provide the same at half the speed, or provide an even better cut at the same speed?

  16. #16
    Join Date
    Jun 2006
    Posts
    629
    split,

    It's all about chip evacuation. Two flute cutters flute have more room to get the chips out of the cut.

    Try using solid carbide with TiAlN coating.

    If you have abunch of parts nested in a sheet of material, try drilling multiple holes in the middle of the sheet to keep it from hsaking rattling and rolling around. Vibration will kill any cutter in any material.
    "It's only funny until some one get's hurt, and then it's just hilarious!!" Mike Patton - Faith No More Ricochet

  17. #17
    Join Date
    Jun 2005
    Posts
    6
    Two flute or one flute is best, you got to get those chips away cleanly.

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •