Best cutting life for cast aluminum tooling plate hogout?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    May 2005
    Location
    AZ
    Posts
    2,293
    Post Thanks / Like
    Likes (Given)
    207
    Likes (Received)
    783

    Default Best cutting life for cast aluminum tooling plate hogout?

    So, we have a small VMC (Sharp 2414) in place for doing small volume R&D/prototyping work. Our parts often require use of cast aluminum tooling plate, for stability in the finished part. We are currently running a part from 2" thk x ~8" x ~10" cast plate, starts out at about 23 lbs, finished weighs a bit less than 4 lbs. Lots of material being removed with 3/4" 2-flute carbide endmill, typically 1/2"-5/8" DOC, stepover maybe .5-.6 X diameter. Programmed speed 6K RPM. Final depth of pockets is anywhere from 1" to about 1.7".

    Cutter life for the end mills seems short, going from nice-looking part without much burr to a pretty ratty-looking burred edge in 2 parts, total time per part maybe a bit over an hour for rough-out, and interim handling and chip management activity. These endmills are Ultra brand, 45 helix for aluminum.

    Anyway, looking for suggestions for highly durable endmills, or insert tools to consider for significantly better lifetime. Thanks --

  2. #2
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    17,913
    Post Thanks / Like
    Likes (Given)
    13489
    Likes (Received)
    13352

    Default

    have you tried using a roughing end mill, they REALLY hog it out and break up the chips as well, then switch to a finisher.

    Breaking up the chips also makes them easier to wash away

    Maritool has a good rep on PM https://www.maritool.com/Cutting-Too...198/index.html

  3. #3
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,872
    Post Thanks / Like
    Likes (Given)
    13136
    Likes (Received)
    10317

    Default

    math time.. ROUNDED #'s..

    So you are removing approx 20lbs.. Taking an hour including chip removal and what not...

    Lets say half an hour. That 6-7 cubic inches a minute.. That's a 1hp cut.. At .6 woc, and .6 doc,
    that's approximatley 17ipm.. Which gives you .003 per rev...

    Is it possible to rub a carbide tool to death in cast tooling plate?

    I haven't run them all that much, but I had one of those Destiny tools with that black coating stay in the
    machine for over 2 years, that thing still cut like a champ until I ran into a bolt.

  4. #4
    Join Date
    Dec 2007
    Location
    Southeastern US
    Posts
    6,383
    Post Thanks / Like
    Likes (Given)
    837
    Likes (Received)
    2780

    Default

    Is 6k RPM all you have?

  5. #5
    Join Date
    May 2005
    Location
    AZ
    Posts
    2,293
    Post Thanks / Like
    Likes (Given)
    207
    Likes (Received)
    783

    Default

    Thanks for the feedback. We have 10K RPM available. The parts are 1st-time pieces for an instrument development project, which is also a process development project for trying out some novel techniques in both the instrument construction and the machining processes. We want to come out with good parts right at the outset due to time constraints, so we may be a little tentative in making chips. The fact that it is cast plate with some thin tall walls is also a cautionary element...I am not running the machine or writing the programs (that guy works for me); my numbers are visual estimates just from what I observe.

    Thanks for the suggestion on rougher and Destiny tools. We'll look into any and all options.

  6. #6
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    17,913
    Post Thanks / Like
    Likes (Given)
    13489
    Likes (Received)
    13352

    Default

    Specfab, IMO the art of hogging is to take as big a cut as possible, at the maximum chipload possible, then worry about the spindle speed ......maintaining that DOC & stepover + feed rate as you up the spindle speed, until you max out on either the cutter speed or spindle load.

    But, and especially, - when cutting deep pockets chip clearance is vital. Recutting chips will shag out any tool LONG LONG before it's expected life is up, - it doesn't do much for the finishes either ! and personally speaking I still favour the old school method of hosing the coolant in a fast as you can to flush the chips out.

    Richer coolant also helps a lot with aluminium.

  7. #7
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    946

    Default

    Have you tried any of the Ripper Mills from Curtis? If the pocket size is large enough you can use a 2 FLT 1" tool and ramp into the pockets, the inserts are razor sharp and throw the chips out of the pockets so very little recutting and the inserts are cheap and last for ever. The only down side to the 2 FLT tool is they are a little nosy at lower RPM but get 10K or more and their sweet sounding but you'll need a fully enclosed machine otherwise it will rain chips on your head.

  8. Likes Limy Sami, Bobw, G00 Proto liked this post
  9. #8
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    17,913
    Post Thanks / Like
    Likes (Given)
    13489
    Likes (Received)
    13352

    Default

    Quote Originally Posted by Captdave View Post
    Have you tried any of the Ripper Mills from Curtis? If the pocket size is large enough you can use a 2 FLT 1" tool and ramp into the pockets, the inserts are razor sharp and throw the chips out of the pockets so very little recutting and the inserts are cheap and last for ever. The only down side to the 2 FLT tool is they are a little nosy at lower RPM but get 10K or more and their sweet sounding but you'll need a fully enclosed machine otherwise it will rain chips on your head.
    Good call Captdave,

    FYI inc a vid, 1 INCH RIPPER MILL

  10. #9
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    7,113
    Post Thanks / Like
    Likes (Given)
    341
    Likes (Received)
    6018

    Default

    Cast plate is abrasive but nicer for chip control.
    Do not use .5 to .6 stepover or the tool will flank wear early. (one should never use 50% step on any material, it's a tool dynamics bad spot thing)
    Get above or below this value then test carbides and tool geometry.

  11. #10
    Join Date
    May 2011
    Location
    No. Cal.
    Posts
    366
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    216

    Default

    Will second Bobw's remarks...

    0.5in dia. 3fl Destiny with stealth coating. Been in the machine for year or more. We cut mostly 6061 cast plate or Mic6 as we build instruments for use in research lab environment (mostly microscope add ons) and need the stability and flatness. Run aforementioned cutter at 10K, 30% stepover on offset tool paths at .8-1d depth of cut. With HSM toolpaths, we lower the engagement of 15-20%, same or somewhat higher feedrates. Usually helix into pockets regardless of tool path type. Leave 0.01 for finish bottom and sides using same tool.

    Depending on how thick your partitions are, may need to run with less stepdown and machine all pockets at each depth.

    If we get into deeper pockets or larger plates, may move to 0.75dia. Destiny, and finish with 0.5in dia. As others have mentioned, getting the chips out is the key. We'll flood the area heavily and use the chip throwing capability of the Destinys or occasionally Lakeshore cutters to get the chips out of the way.

    Fred

  12. #11
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,694
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2544

    Default

    many alloys are abrasive. not hard but abrasive and are hard on tools.
    .
    take a grinding wheel, you can open the hole up going slow rpm and just drill it out with a twist drill. of course drilling a grinding wheel with a hss twist drill will dull the drill bit quickly.
    .
    i often use 1.75" dia roughing end mill taking 1.75 doc and 1.5 woc at 20 ipm feed in aluminum. you need hp and ability to get chips out of the way fast enough and got to be able to hold the part securely.
    .
    they make 4" roughing shell mills too. 1" doc at 3.5 woc is possible often more is possible. again you need hp and ability to hold parts and flush chips out of the way fast enough

  13. #12
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,055
    Post Thanks / Like
    Likes (Given)
    160
    Likes (Received)
    1417

    Default

    Quote Originally Posted by Freds View Post
    Will second Bobw's remarks...

    0.5in dia. 3fl Destiny with stealth coating. Been in the machine for year or more. We cut mostly 6061 cast plate or Mic6 as we build instruments for use in research lab environment (mostly microscope add ons) and need the stability and flatness. Run aforementioned cutter at 10K, 30% stepover on offset tool paths at .8-1d depth of cut. With HSM toolpaths, we lower the engagement of 15-20%, same or somewhat higher feedrates. Usually helix into pockets regardless of tool path type. Leave 0.01 for finish bottom and sides using same tool.

    Depending on how thick your partitions are, may need to run with less stepdown and machine all pockets at each depth.

    If we get into deeper pockets or larger plates, may move to 0.75dia. Destiny, and finish with 0.5in dia. As others have mentioned, getting the chips out is the key. We'll flood the area heavily and use the chip throwing capability of the Destinys or occasionally Lakeshore cutters to get the chips out of the way.

    Fred
    I would agree with all of this. I can't see how you could be losing a quality carbide endmill in 2 parts. The Diamondback with Stealth I currently have loaded has plowed several hundred # of chips, in 6061, 7075, and a little MIC-6, and shows no signs of deterioration.

    Assuming your machine can handle it -- 25% stepover, 2xD axial, .006" - .01" chip depending on ability of control to keep up, max RPM. If your spindle bogs, decrease the stepover.

    Regards.

    Mike

  14. #13
    Join Date
    May 2005
    Location
    AZ
    Posts
    2,293
    Post Thanks / Like
    Likes (Given)
    207
    Likes (Received)
    783

    Default

    Thanks, ever'body -- good info to work with. We'll look at the actual cutting parameters (rather than my guesstimates from the sidelines) and see where we can adjust to improve lifetime, and look at the other cutters suggested. I certainly thought lifetime should be "somewhat" longer.... We are running coolant at 9-10% to help a little with cast material and deep pockets, and we have been trying to improve the coolant nozzle distribution as well, to make sure we are clearing chips out.

    Carbide Bob -- thanks for the definitive statement about stepover ratio.

    LimySami --"Specfab, IMO the art of hogging is to take as big a cut as possible"... That was something that I still remember from an interview I had with the shop manager at Harvard Astro lab shop, back in mid-80's when I first discovered I didn't know much: "The most important thing is to get rid of the material as fast as possible..." Still sticks in my mind to this day.

    Finegrain, Bobw, Freds -- sounds like a winner in the Destiny line.

  15. Likes Limy Sami liked this post
  16. #14
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,423
    Post Thanks / Like
    Likes (Given)
    887
    Likes (Received)
    803

    Default

    Quote Originally Posted by specfab View Post

    Finegrain, Bobw, Freds -- sounds like a winner in the Destiny line.
    I've been using YG Alu-Power 3fl endmills. I haven't worn one out yet, they get changed because they occasionally run into something that isn't AL. They can be had pretty cheap on ebay. They work so well I don't bother with roughing endmills any more.

  17. #15
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,055
    Post Thanks / Like
    Likes (Given)
    160
    Likes (Received)
    1417

    Default

    Quote Originally Posted by triumph406 View Post
    I've been using YG Alu-Power 3fl endmills. I haven't worn one out yet, they get changed because they occasionally run into something that isn't AL. They can be had pretty cheap on ebay. They work so well I don't bother with roughing endmills any more.
    I also use Alu Power for all finishing and little work. I still like the 1/2" and 3/8" Diamondbacks for 2 reasons:

    1. Lower spindle load
    2. Chips are much more dense -- 1" or 1-1/4" long strings from a non-segmented endmill are way fluffier and fill the pan much more quickly

    Regards.

    Mike

  18. #16
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    17,913
    Post Thanks / Like
    Likes (Given)
    13489
    Likes (Received)
    13352

    Default

    Quote Originally Posted by triumph406 View Post
    I've been using YG Alu-Power 3fl endmills. I haven't worn one out yet, they get changed because they occasionally run into something that isn't AL. They can be had pretty cheap on ebay. They work so well I don't bother with roughing endmills any more.
    You probably know there's a simple dodge to making a roughing cutter

    Get a cheap diamond tile saw blade, then mark with a sharpie each flute of the EM in say a 1/4'' pitch helix, then grind your own chip breakers in to the flute - a .030 to .040'' deep nick is plenty.

    Okay, maybe it's not the real McCoy, but it still works, .......and when you're in a hole or have a load of cutters on the cheap, nothing beats a few $ in the pocket

  19. #17
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,630
    Post Thanks / Like
    Likes (Given)
    686
    Likes (Received)
    1856

    Default

    Quote Originally Posted by Freds View Post
    Leave 0.01 for finish bottom and sides using same tool.
    You're finishing with the Diamondback? Don't the serrations leave an atrocious wall finish?

    I use mine for floor finishing all the time, but come in with another tool for the walls.

  20. #18
    Join Date
    May 2011
    Location
    No. Cal.
    Posts
    366
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    216

    Default

    Quote Originally Posted by gkoenig View Post
    You're finishing with the Diamondback? Don't the serrations leave an atrocious wall finish?

    I use mine for floor finishing all the time, but come in with another tool for the walls.
    Diamondback? I think somebody else mentioned that. We use Destiny Viper 3fl, Stealth coating for both rough and finish.

    Fred

  21. #19
    Join Date
    Aug 2012
    Location
    Alberta
    Posts
    23
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    9

    Default

    I know that this is an old thread but it might be of some value to revive it.....
    I’m machining cast aluminum blanks and just thought I would add this:
    Check the part for residual sand from the casting process.
    I have rough cast blocks I am machining and it has beaten the APKT inserts that I have been using for almost a year.
    The casting have entrained sand from the casting process and I suspect that is what caused the inserts to wear rapidly.

    I’m not sure what the best way to get rid of the outside layer of these blocks is.

  22. #20
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,055
    Post Thanks / Like
    Likes (Given)
    160
    Likes (Received)
    1417

    Default

    Quote Originally Posted by Upnorth4 View Post
    I’m not sure what the best way to get rid of the outside layer of these blocks is.
    Don't know if this would help, but how about a 30-40% engagement conventional cut? Push the dirty skin generally straight out into space instead of mashing it into the rest of the cut.

    Regards.

    Mike


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
  •