Results 1 to 12 of 12
  1. #1
    implmex is offline Stainless
    Join Date
    Jun 2002
    Location
    Vancouver BC Canada
    Posts
    1,474

    Default Best choice for free machining aluminum?

    Hi All:
    I have been given a project to quote that will need turning and slotting.
    These are fairly small parts, around 6mm diameter and 32 mm long and need to be made from aluminum (any alloy I want).
    I need to drill a 4 mm diameter hole, turn the OD to 6 mm, slot in 2 places with an endmill,
    chamfer the slots on the outside only, then part off.
    The main criterion for acceptance is surface finish on the outside and the slots...nobody cares about tolerances on this part (within reason).
    Burs are also heavily frowned upon.

    Is 2011 my best choice for a project like this or are there other grades I need to consider?

    Am I better off buying bar stock (cheap) and drilling it, or buying tubing (expensive and hard to find) and eliminating an operation?

    Is there a place that even sells 2011 in 1/4" diameter tube?
    I had no luck with a Google search.

    Thanks in advance
    Cheers

    Marcus
    Implant Mechanix – Design & Innovation - home

  2. #2
    ewlsey is online now Diamond
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    5,018

    Default

    I don't think the actual alloy matters that much for machining. The biggest factor is the heat treatment. Aluminum with a T-6 temper will be much easier to machine than a gummy untreated version.

    I mostly work with cast aluminum (356). I have had good luck with plain old 6061 though.

    Tubing will likely be an extrusion just like bar stock in that size so it probably has no effect from a material standpoint.

    Hope that helps.

  3. #3
    cncbrit is offline Hot Rolled
    Join Date
    Apr 2011
    Location
    California
    Posts
    518

    Default

    A crisper aluminium will burr less, and a higher heat treat will also be better, 7075 in T6 would be great, but it does corrode unless you anodize it.

    I would turn, drill, mill, chamfer, and part off. you will be left with a burr in the bore from the slot milling, and a part off burr on the back end.

    Set up for second opp, clean up the back side and ream through to get rid of the slot burrs.

  4. #4
    Mud's Avatar
    Mud
    Mud is offline Diamond
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    10,741

    Default

    2011-T3 would be my choice.

  5. #5
    Limy Sami is online now Diamond
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    11,943

    Default

    Quote Originally Posted by Mud View Post
    2011-T3 would be my choice.
    Mine too,........ and if the quantity is high I'd look at getting it centreless ground to size.

  6. #6
    Ox's Avatar
    Ox
    Ox is online now Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    18,173

    Default

    The 2011 will not burr much (nor will 2024) so that will help you with the cross holes, but I have found that it does not shine like 6061 from normal single point tools. 2011 is a screw machine grade, and I suspect that a flat form (dogbone type) will leave a better finish than a basic single point tool will. Much the same with steels designed for screw machines.

    However - with the L/D ratio that you have mentioned, you will likely be starting wuith 1/4" and you would likely either need to run in a Swiss Lathe if you want to turn it, or - as has been mentioned above - just toss it in a centerless grinder to bring down to spec.

    -------------

    Think Snow Eh!
    Ox

  7. #7
    implmex is offline Stainless
    Join Date
    Jun 2002
    Location
    Vancouver BC Canada
    Posts
    1,474

    Default Thanks

    Hi All:
    Thanks for all the information; yeah Ox, I am concerned about the length to diameter ratio, and may farm this job out to a Swiss guy (there are just enough parts in the run to justify it)
    Centerless ground stock is also a good idea, but only if I can get some kind of non-marring collet for the machine...standard 5C's will scarf the material up so badly I'll have gained nothing.
    My main concern (other than the finish) is drilling the hole fast...I've had some issues in the past with 6061 T6 piling up on the tool and I'm hoping 2011 T3 will be better especially with a through coolant carbide drill.
    I once had a chunk of mystery aluminum that cut like butter and made really nice small chips but was soft compared to 7075....is that how 2011 T3 cuts?
    The only thing printed on the bar remnant that I could read was something like "Microcut" or "Micro"

    Also, what do you guys think of deburring the internal edge of the slots by mounting a wire brush (like a test tube brush set up as if it were a drill) and programming it to run in and out of the hole a couple of times with some side pressure?
    Have any of you tried something like this? Did it work?

    CNCBrit, I was hoping to do the job in a single op; running the part complete including deburring from one end, but drilling my hole just deep enough that the cutoff will intersect it.
    All of the blade is then pushing into solid metal and with luck and fiddling, I hope there's virtually no burr left.
    That's one of the reasons I'm considering turning the parts from solid rather than buying tubing.
    I've been successful this way in the past but I'm certainly open to suggestions and criticisms.
    Production turning is my weakest capability...I just don't do very much of it, so I've never gotten a chance to get good at it.
    Cheers

    Marcus
    Implant Mechanix – Design & Innovation - home

  8. #8
    Limy Sami is online now Diamond
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    11,943

    Default

    Nylon 5C collets - wonderful things within their capabilities

    '' I once had a chunk of mystery aluminum that cut like butter and made really nice small chips but was soft compared to 7075....is that how 2011 T3 cuts?''

    It does for me,.....or what I've been sold as 2011 T3 does.

    ''Also, what do you guys think of deburring the internal edge of the slots by mounting a wire brush (like a test tube brush set up as if it were a drill) and programming it to run in and out of the hole a couple of times with some side pressure?
    Have any of you tried something like this? Did it work?''

    Yes I have and it did, and I'd use it again.

    Cut carefully with really sharp tools 2011 T3 / T6 produces very light burrs.

    ''CNCBrit, I was hoping to do the job in a single op; running the part complete including deburring from one end, but drilling my hole just deep enough that the cutoff will intersect it.
    All of the blade is then pushing into solid metal and with luck and fiddling, I hope there's virtually no burr left''

    Look in to the thinbit type part off tools, with inserts ground for Alu, with a 15deg angle.

  9. #9
    Ox's Avatar
    Ox
    Ox is online now Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    18,173

    Default

    I meant to grind the part AFTER they were done.
    This way you can use serated collets if you want, and/or eny handling marks on the bar will be taken off AFTER the part is complete - and not 11'10" of bar attached to it.
    This will also attack eny OD burrs on your milled windows.


    Yes - 2011 and 2024 chip up unbelievably good and throw very small burrs.
    However - it is about 1/2 aggin as expencive per foot. It weighs more per foot than 6061 as it has 9% (?) copper in it.


    --------------------

    Think Snow Eh!
    Ox

  10. #10
    newg3 is offline Plastic
    Join Date
    Jun 2007
    Location
    Maine
    Posts
    43

    Default

    All the 2011 we use has to be RoHS compliant...not sure if all 2011
    already is but maybe this is something to think about

  11. #11
    implmex is offline Stainless
    Join Date
    Jun 2002
    Location
    Vancouver BC Canada
    Posts
    1,474

    Default This is all very interesting

    Limy: I was completely unaware that nylon 5C collets are available...I guess I don't get out enough; thanks for the tip.
    Ox, I've got no experience with centerless at all...I didn't even think of the possibility of feeding them through as finished parts...it's a good thought but wouldn't you worry about having the occasional slot catch on the support blade of the centerless grinder and boogering the part?
    Also, with such a thin wall, and a skinny (about 1 mm wide and 1 mm thick) rib between the two slots (they're spaced at 120 degrees BTW, not 180 degrees), would you still be confident that the cylindrical grinder could process these without a hitch?
    As an alternative, if I turned them from thicker, stiffer bar, say 5/16" , could I get around the deflection from the rotten L/D ratio if I took it to diameter in one pass, then drilled it and slotted it.
    I know it'd waste more material, but I'm thinking it might give me a better result than trying to shave a smidge off a 1/4 inch bar sticking out 35 mm.

    Actually, the more I talk this job through, the more inclined I am, to farm it off to the Swiss guys, especially since the customer wants to stay under a buck apiece if he can.
    Thanks again for all your help guys, it's appreciated.
    Cheers

    Marcus
    Implant Mechanix – Design & Innovation - home

  12. #12
    Ox's Avatar
    Ox
    Ox is online now Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    18,173

    Default

    I ass_u_med that you were just puting windows in the sides. If your slots go all the way to the outside - then that doesn't doo well in the C/less.


    -------------

    Think Snow Eh!
    Ox

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
  •