Machining cast iron vs 1018, not as expected.
Close
Login to Your Account
Results 1 to 16 of 16
  1. #1
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    279
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    50

    Default Machining cast iron vs 1018, not as expected.

    I've been making a part from 1018 for a couple years, for this recent order the 1018 was unavailable, so we are allowed to switch to class 40 grey cast iron.

    I've never done any real cast iron milling, aside from small simple stuff. This part takes about hour, tons of roughing, flat and perpendicular within .002.

    For my first part I decided to run my normal 1018 program as a baseline. I was expecting the program to be slow. My expectations would.be 650 sfm would be about right, and chatter would be non existent. I expected to be able to feed faster.

    This part is held upright in a lang vise, most of the roughing is 5" away from the vise with the table at 90 degrees. Not a rigid setup, but excellent for those perpendicularity call outs.

    Roughing 5 flute end,
    650 sfm
    .090 radial
    1.25 axial
    .004 per tooth.
    This is the sweet spot for this setup in 1018. Chatter like crazy in cast, the whole system was humming, from end mill to concrete.

    Face milling 2" facemill (don't remember the exact parameters)
    1500rpm
    .005 chip perhaps.
    .035 stock depth finish,

    I ended up having to take the end mill down to 12 percent for the cast before the chatter went away, and the facemill to .010 stock remaining, and even that wasn't great.

    My question I suppose is, what is the typical things to look out for, or adjust from 1018 to cast. Thanks

  2. #2
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,584
    Post Thanks / Like
    Likes (Given)
    855
    Likes (Received)
    696

    Default

    Cast iron is more abrasive, denser, and has more surface tension. When machining cast, a rigid set up is a must and your D.O.C. is critical.

  3. Likes michiganbuck, Fancuku liked this post
  4. #3
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    279
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    50

    Default

    Quote Originally Posted by DouglasJRizzo View Post
    Cast iron is more abrasive, denser, and has more surface tension. When machining cast, a rigid set up is a must and your D.O.C. is critical.
    Seems like based on what I'm seeing a lighter step over with faster feed is the way to go. I can't do anything about the rigidity given the shape of the part. Would you say that's the correct direction to go?
    Thanks

  5. #4
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,584
    Post Thanks / Like
    Likes (Given)
    855
    Likes (Received)
    696

    Default

    Quote Originally Posted by BRIAN.T View Post
    Seems like based on what I'm seeing a lighter step over with faster feed is the way to go. I can't do anything about the rigidity given the shape of the part. Would you say that's the correct direction to go?
    Thanks
    Yes, absolutely. You would be reducing the amount of torsional force on the tool.

  6. #5
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    13,861
    Post Thanks / Like
    Likes (Given)
    4723
    Likes (Received)
    4988

    Default

    At the big shop, carbide worked best for CI. 1018 flows along the tool cutting edge while CI takes more pressure and fractures ahead on the cutting edge. Carbide always proved best for CI and a small negative land at the cutting edge proved good. . Higher heat was a factor so a thicker insert was good so to absorb some of the heat.. dry was often better than using a coolant. When a coolant was used it had to be flooding, not a mist.

    The negative land perhaps 5* and .003 to .020 wide allows the cratering common with CI to have a more cutting edge body to crater away before it affects the optimum cutting action, the wear seems to be/begin a tad away and behind the actual top face of the cutting edge.

    It was not uncommon that the negative land proved better than the whole top cutter face being negative.

    CI really beats up HSS cutting tools from the very start.

    I can't see your set-up but if it might bump onto a solid heavy block high at the part's away side so reducing vibrations and chatter might make tool life increase and part quality better, rock-solid is best for CI.

    The old Valenite value mills are good because you can set each insert under an indicator to a few tenths quickly on a plate. Having all the teeth engaged from the start is good.

  7. #6
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    10,373
    Post Thanks / Like
    Likes (Given)
    1420
    Likes (Received)
    3801

    Default

    That's weird. I had a job once machining a planetary carrier out of a 12" diameter chunk of Durabar. I thought as I was cutting it 'wow, no wonder they made entire machines out of this stuff, it's the nicest machining shit possible' I only ran with carbide.

  8. #7
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    3,008
    Post Thanks / Like
    Likes (Given)
    586
    Likes (Received)
    959

    Default

    Durabar is not even close to #40 cast iron.

  9. #8
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,622
    Post Thanks / Like
    Likes (Given)
    992
    Likes (Received)
    1839

    Default

    Gray iron has about 2/3 the rigidity of steel but roughly the same machinability as 1018.

    The net result in your case is the need to dial back the parameters.

    The vibration damping characteristics of gray iron don't really apply to small workpieces.

  10. #9
    Join Date
    Dec 2005
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,961
    Post Thanks / Like
    Likes (Given)
    494
    Likes (Received)
    651

    Default

    Quote Originally Posted by BRIAN.T View Post
    so we are allowed to switch to class 40 grey cast iron.
    Oh lucky you


    Sent from my iPhone using Tapatalk

  11. #10
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    279
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    50

    Default

    Quote Originally Posted by adh2000 View Post
    Oh lucky you


    Sent from my iPhone using Tapatalk
    Haha yeah, there is a reason they listed it as the alternative. It's not great.

  12. #11
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    279
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    50

    Default

    Quote Originally Posted by Orange Vise View Post
    Gray iron has about 2/3 the rigidity of steel but roughly the same machinability as 1018.

    The net result in your case is the need to dial back the parameters.

    The vibration damping characteristics of gray iron don't really apply to small workpieces.
    I was hoping I'd hear from you! This is interesting information, and seems to be on par with what I saw today really getting into it. I was only able to get through about 5 parts before I left for the day, but it was running well.

    Interesting side note, 8 percent increase in sfm cleared up all the chatter.. hopefully 700sfm isn't too hot. What do you think?

  13. #12
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    279
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    50

    Default

    Quote Originally Posted by michiganbuck View Post
    At the big shop, carbide worked best for CI. 1018 flows along the tool cutting edge while CI takes more pressure and fractures ahead on the cutting edge. Carbide always proved best for CI and a small negative land at the cutting edge proved good. . Higher heat was a factor so a thicker insert was good so to absorb some of the heat.. dry was often better than using a coolant. When a coolant was used it had to be flooding, not a mist.

    The negative land perhaps 5* and .003 to .020 wide allows the cratering common with CI to have a more cutting edge body to crater away before it affects the optimum cutting action, the wear seems to be/begin a tad away and behind the actual top face of the cutting edge.

    It was not uncommon that the negative land proved better than the whole top cutter face being negative.

    CI really beats up HSS cutting tools from the very start.

    I can't see your set-up but if it might bump onto a solid heavy block high at the part's away side so reducing vibrations and chatter might make tool life increase and part quality better, rock-solid is best for CI.

    The old Valenite value mills are good because you can set each insert under an indicator to a few tenths quickly on a plate. Having all the teeth engaged from the start is good.
    Great info! Thanks, I'm definitely not using HSS anything, I probably haven't used a hss end mill in 2 years. For the setup, I can't (don't want to change it) it's a 5 axis setup, work on all sides, most faces are perpendicular to one another .002. splitting up the ops would be problematic I think.

    So far with the info you and other provided my ends mills are doing great. Thanks

  14. #13
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,622
    Post Thanks / Like
    Likes (Given)
    992
    Likes (Received)
    1839

    Default

    Quote Originally Posted by BRIAN.T View Post
    I was hoping I'd hear from you! This is interesting information, and seems to be on par with what I saw today really getting into it. I was only able to get through about 5 parts before I left for the day, but it was running well.

    Interesting side note, 8 percent increase in sfm cleared up all the chatter.. hopefully 700sfm isn't too hot. What do you think?
    700 sfm should be perfectly fine. Full slotting endmills run the slowest at 500 SFM. Everything else runs faster. We run our facemills between 800 and 1000 sfm. Dry of course.

  15. #14
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    1,134
    Post Thanks / Like
    Likes (Given)
    144
    Likes (Received)
    460

    Default

    What a contradiction, cast iron and a lot to rough!
    Cast parts are there to reduce the amount of machining.
    We seem to have lost one great idea of industrialisation.

    If you have to rough cast iron, reduce Vc by a third to half compared to mild steel.

  16. #15
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    279
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    50

    Default

    Quote Originally Posted by Mechanola View Post
    What a contradiction, cast iron and a lot to rough!
    Cast parts are there to reduce the amount of machining.
    We seem to have lost one great idea of industrialisation.

    If you have to rough cast iron, reduce Vc by a third to half compared to mild steel.
    While I understand what you're implying, the part is not cast, it's cast iron bar stock. Perhaps I could look into having them cast. I wonder what that would cost.. interesting.

  17. #16
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    13,861
    Post Thanks / Like
    Likes (Given)
    4723
    Likes (Received)
    4988

    Default

    At the big shop we decided to make a part of nodular cast iron so we had the Detroit Testing Lab run a machining test on that material. I should have kept a copy of the results but did not.


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
  •