1. Welcome to the New & Improved BladeForums. New software info here. Please report problems in Tech Support, and read existing threads before posting! - Spark
  2. I've changed the default forum style to Flat Awesome based on feedback. Don't like it? Click here to change how the forums look Feedback on this is welcome here.

What type of end mills are best suited for machining aluminum?

Discussion in 'Shop Talk - BladeSmith Questions and Answers' started by Fred.Rowe, Aug 8, 2009.

  1. Fred.Rowe

    Fred.Rowe Dealer / Materials Provider Dealer / Materials Provider

    May 2, 2004
    I am getting ready to manufacture a run of aluminum parts next month and would like to know the best type of end mills for the job. I am using a Bridgeport J head mill and will be cutting a 1/2 inch wide slot in 3/4 inch bar stock. The slot needs to be flat at the bottom.

    Fred
     
  2. JasonSCarter

    JasonSCarter

    Dec 20, 2008
    2 flute HSS wont be a bad choice but Carbide would last longer. how many parts are we talking in the run?
     
  3. Fred.Rowe

    Fred.Rowe Dealer / Materials Provider Dealer / Materials Provider

    May 2, 2004
    I will be using them for extended runs so will put the money into the carbide cutters. Is the reason for choosing the two flute cutters is they will not load up as much as cutters with more flutes?

    Thanks Fred
     
  4. JasonSCarter

    JasonSCarter

    Dec 20, 2008
    yea Aluminum is a gummy metal, and needs a good chip relief to reduce chatter.
     
  5. Nathan the Machinist

    Nathan the Machinist KnifeMaker / Machinist / Evil Genius Moderator Knifemaker / Craftsman / Service Provider

    Feb 13, 2007
    Yeah, the idea is with aluminum you can double the chip load - no problem, but recutting and welding is a problem when slotting. So you use a 2 flute. Actually, I think most shops these days use a 3 flute for slotting because with modern cutter geometry it works as well as the old two flutes, it is stiffer, and you can feed 50% faster.

    If you're doing much of these you should use an endmill with aluminum specific geometry. I love the OSG blizzards for aluminum. Great finishes and chips pouring out of the slot like water out of a hose. But I use the MSC aluminum Accupro because they're cheap, and they go on sale 30% about once a week (just check the website in the morning) and they work well. Look at this one:

    http://www1.mscdirect.com/CGI/NNSRI...id=13665Pstoreid=1040626Ppagenumber=593Pmode=

    BTW, the ZrN coating is the tits if you ever want to machine copper. Now that is gummy.

    In high productivity machining, but on a Bridgeport (do you have coolant?) I'd slot aluminum with a 1/2" three flute aluminum geometry endmill, perhaps in top gear 2720 RPM, lock the Y axis then feed it at 30-40 IPM. The depth of cut will be a function of spindle HP and rigidity, try 1/8" to start. If you're not using coolant try WD40 (one thing it is good for is machining aluminum).

    BTW, I regularly turn that exact cutter at 6000 RPM in aluminum, but on a heavy mill.
     
  6. JasonSCarter

    JasonSCarter

    Dec 20, 2008
    Nathan you are the king, when it comes to this stuff. I use old school stuff. Infact I think my Machinary handbook I consulted is only the 23rd edition. :D 6 grand through aluminum huh? geeeeeeeze!:eek:
     
  7. Fred.Rowe

    Fred.Rowe Dealer / Materials Provider Dealer / Materials Provider

    May 2, 2004
    Thanks for the feedback, Jason and Nathan; makes a lot of since.

    I'll be looking for the aluminum specific cutters you have suggested; I want to get the best out of my production time and your advice will help to make this possible.

    Fred
     
  8. Nathan the Machinist

    Nathan the Machinist KnifeMaker / Machinist / Evil Genius Moderator Knifemaker / Craftsman / Service Provider

    Feb 13, 2007
    It isn't as loony as it sounds. Aluminum likes RPM. Though you have to feed it correctly so you're achieving an appropriate chip load. With the right cutter with the right geometry and coating - some folks might turn a 1/2" in aluminum at 10,000RPM or more and feed at 200 IPM or more. They call this "high speed machining" and they can achieve impressive material removal rates. It requires special care when ramping into and out of a cut to prevent shock, but most of the better CAM systems have algorithms for this. But everything has to be just right, and the mills are heavy.

    This morning I'm facing down some 12X24 aluminum plates. I'm using a 3" face mill at 1800 RPM, which is actually more SFM than a 1/2" turning 10,000 RPM. And my mill really isn't that heavy. I'm misting the plate with WD40 before I start, but it is otherwise dry, and the plate is only slightly warm to the touch when I'm finished.
     
  9. JasonSCarter

    JasonSCarter

    Dec 20, 2008
    Wow those speeds and feeds are astonishing...The closest I have to CNC is a powered x axis table on a 1974 Bridgeport with a J head and after market digital readout. I cut my teeth on a 1860's line shaft horizontal mill we retrofitted for electric power. then moved to a 1930's Kearney & Trekker 3 1/2B Horizontal, we restored & made an arbor for to accept R8 collets to use end mills horizontally. So yea I'm used to using OLD tech!

    Jason
     

Share This Page