Cutting alloy fail


Page 1 of 2 12 LastLast
Results 1 to 20 of 29

Thread: Cutting alloy fail

  1. #1
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Cutting alloy fail

    Hi guys, can anyone tell me what I've done wrong here. First time cutting alloy and was a disaster as per the photos show. Machine is a stepcraft with a kress 800 spindle. 2mm 2 flute end mill. 1st cut was at 150mm/min at 12000rpm, 2nd at 70mm/min 10000rpm and 3rd at 50mm/min at various speeds from 10000 to about 14 or 15000rpm. As you can see the results are all very similar. Intial pass was set at 1mm step down then set it at .5mm. Had air blast on 2 attempts then just wd40 on the last. Using fusion 360 for software. Alloy is 6060. Hopefully I've included enough/correct information.




    Similar Threads:
    Attached Thumbnails Attached Thumbnails Cutting alloy fail-img_2104-jpg   Cutting alloy fail-img_2105-jpg   Cutting alloy fail-img_2106-jpg  


  2. #2
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Cutting alloy fail

    Try 1000mm/min and 12000 rpm, and 0.3mm depth per pass.

    What type of tool are you using?

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  3. #3
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Quote Originally Posted by ger21 View Post
    Try 1000mm/min and 12000 rpm, and 0.3mm depth per pass.

    What type of tool are you using?
    Do you think the feed is too slow? 1000mm/min brings images of broken cutters to the mind lol.
    cutter is from kyocera I believe
    Cutting alloy fail-cutter-jpg



  4. #4
    Registered
    Join Date
    Jan 2006
    Location
    New Zealand
    Posts
    509
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    You could try wiping the surface with some kerosene first too, some alloys of aluminium just gum up cutters really badly.

    Shannon.



  5. #5
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Thanks will try that before next cut. Is it possible that the alloy is not as was stated? maybe it is of a softer grade? Could you comment ger21 more on your suggested feed of 1000mm/min, to me that seems way too much for a small 2mm cutter but I am inexperienced so I could be far from the truth.



  6. #6
    Registered
    Join Date
    Jan 2006
    Location
    New Zealand
    Posts
    509
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    The softer grades are harder to cut and often do need some cutting fluid. The same grade of aluminium can also vary a little from sheet to sheet, one sheet might cut well and the next not so much.

    Shannon.



  7. #7
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Quote Originally Posted by Big S View Post
    The softer grades are harder to cut and often do need some cutting fluid. The same grade of aluminium can also vary a little from sheet to sheet, one sheet might cut well and the next not so much.

    Shannon.
    hmm ok mate, have a different bar there that I may try and see how it goes.



  8. #8
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Cutting alloy fail

    The mess gets worse as your feed goes down. Yes?
    You are not cutting the metal, you are rubbing it and melting it.
    Lower spin and higher feed, and make with the kero.
    And make quite shallow cuts if it's a 2 mm cutter!
    The aluminium looks a bit crappy for machining as well.

    Cheers
    Roger



  9. #9
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Quote Originally Posted by RCaffin View Post
    The mess gets worse as your feed goes down. Yes?
    You are not cutting the metal, you are rubbing it and melting it.
    Lower spin and higher feed, and make with the kero.
    And make quite shallow cuts if it's a 2 mm cutter!
    The aluminium looks a bit crappy for machining as well.

    Cheers
    Roger
    Well it didn't seem to change much as I went down in feed, I'm thinking the cut was too big but I am also starting to wonder about the alloy, just like you say. My thoughts too that it seems to be melting it and not cutting it. The kerosene, it is for lubrication/cutting?



  10. #10
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Cutting alloy fail

    I cut 5000-series sheet, which is a complete pain. Speed about 2,800 RPM and feed about 200 mm/min. It works. You are melting the stuff, and it is a marvel you have not smashed the cutter with Built Up Edge (BUE). (Google it.)
    The kero wets the surface of the cutter and prevents the aluminium from sticking. The ideas behind the conventional and very out of date 'flood coolant' are all wrong for aluminium.

    Cheers
    Roger



  11. #11
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    unfortunately I can't go that low in speed. But I am using wd40 which seems to be good as I'm lead to believe. Actually the first cut I did break cutter, but the following to cuts were ok, at a lower feed. but I think now by the comments and my own thoughts that the cut was to big and/or bad alloy. Yes I see what you mean about BUE, looks like my problem.
    The solution or next attempt should be ;
    smaller cut with higher feed, does 150mm/min sound ok? as thats what the original speed was.



  12. #12
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Cutting alloy fail

    Sorry, I was sleeping...

    No, you need to go much faster.
    Try 1000mm/min, as I said, but with a shallower cut, like .2mm. I thought you were using a 3mm bit.

    And use a lot of WD40.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  13. #13
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Quote Originally Posted by ger21 View Post
    Sorry, I was sleeping...

    No, you need to go much faster.
    Try 1000mm/min, as I said, but with a shallower cut, like .2mm. I thought you were using a 3mm bit.

    And use a lot of WD40.
    No problem and thanks for the help, thanks to all posters for the help it really is appreciated. Ok I am scared of the 1000mm/min but will try it with the .2mm cut. I will try a few different feeds at that depth.



  14. #14
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Cutting alloy fail

    As Ger says - with those RPM you need more surface speed, but shallow cuts. Creep up on it from very shallow.
    WD40 works but is $. I use a mix of 3 parts kero to 1 part olive oil - pretty harmless stuff.

    Cheers
    Roger



  15. #15
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Thanks Roger, thats good info, I have a bit of wd40 there as I use it for other things. Going to try all the above suggestions this weekend and will report back with good results hopefully.



  16. #16
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Ok looks like we may have some success and ger21 was spot on with his 1000mm/min feed suggestion.

    Cutting alloy fail-img_2108-jpg

    these were cut at lowest spindle speed, 10000 rpm and fed at either 1000 or 1100mm/min with either a .1 or .2mm cut. Wasn't much difference between each of them though I think at .1mm cut you may be able to up the feed even more. Best thing is, no built up edge, success! Thanks again everybody for the help.

    Now my next question is will these settings work with 6061 and 7075? Also as I'm probably only ever going to cut with these alloys (and maybe acrylic/delrin/other plastic) is it worth investing in a feeds and speeds calculator such as g-wizard or other suggestion?



  17. #17
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Cutting alloy fail

    Keep experimenting. A 0.1 mm DoC might be a shade too small if the surface is not absolutely smooth. Cut, don't rub. On the other hand, I have been machining 2011 aluminium with a DoC of 0.05 mm, but with a 1.2 mm carbide ball end cutter at 3,000 RPM. Have to keep the sideways loading down when the cutter is that thin.

    6061 and 7075 are harder materials that 5000-series, so the load on the cutter may be a shade higher. But not by much if you use a sharp cutter rather than a cheap one with a square face, and they are both much nicer to machine. I have been using sharp cutters designed for HR55+ steel on aluminium - and liking it.

    Plastics - DROP the spindle RPM! You can pour heat into the Al chips and they will flay away, taking the heat with them. Pour the same heat into plastic and it may melt. Trouble! You may find it well worth while to reserve some new and very sharp cutters purely for plastics. Don't let any metal blunt their edges at all. Acetal/Delrin is nice to machine, nylon is OK, PE is a pain as it feathers. But it does have some nice engineering prioperties, so I persist.

    Cheers
    Roger



  18. #18
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Hey Roger, great tips mate thank you, I will certainly now get some cutters solely for plastics. As far as a feeds and speeds calculator is it worth getting or not really as I now know ballpark figures for feeds/speeds on the grades of alloy I will be using?



  19. #19
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    4252
    Downloads
    4
    Uploads
    0

    Default Re: Cutting alloy fail

    Some people swear by them. Me, I don't have one: I go on experience. I guess - cost me a few cutters over the years.
    Actually, there are some 'free' versions on the web, suitable for a first pass with a new material. And some catalogs from up-market cutter mfrs have very useful tables in the back. Catalogs can come as PDFs.

    Cheers
    Roger



  20. #20
    Member
    Join Date
    Jun 2016
    Location
    Australia
    Posts
    91
    Downloads
    0
    Uploads
    0

    Default Re: Cutting alloy fail

    Quote Originally Posted by RCaffin View Post
    Some people swear by them. Me, I don't have one: I go on experience. I guess - cost me a few cutters over the years.
    Actually, there are some 'free' versions on the web, suitablle for a first pass with a new material.

    Cheers
    Roger
    Thanks mate, kind of leaning the same way as you. G-wizard is fairly pricey for my needs, and as you say experience is key.



Page 1 of 2 12 LastLast

Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Cutting alloy fail

Cutting alloy fail