Need Help! Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball nose


Results 1 to 13 of 13

Thread: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball nose

  1. #1
    *Registered User* izzydog312's Avatar
    Join Date
    Jan 2019
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball nose

    hey guys! wondering if someone could please assist me so im not going through so many bits.

    we have a sheet of 6061 aluminum that we a trying to get a nice texture ( about 1/8 '' deep for detail ) out of but we are running into problems.


    We have used a 3/8 '' end mill for the rough in, which took a fair amount of bulk away, no problems with that, cuts perfectly fine, not breaking bits.

    Once we took the most of the bulk with the 3/8'' end mill we switched to 1/8'' BALL nose bit and ran into some serious trouble.

    The 1/8'' ball nose is getting aluminum welded around the bit quickly and causes us to shutdown because there is no profile left on the bit because of all the aluminum welded on

    (note we are using the machine relief tool-path on artcam for the 1/8'' ball nose bit)

    Here is the feeds and speeds that we are running our bit at : Step over : .18
    Step Down .005
    Feed rate : 60
    Spindle : 20 000 If someone could point me in the right direction, would be much appreciated ! thanks !

    Similar Threads:


  2. #2
    *Registered User* izzydog312's Avatar
    Join Date
    Jan 2019
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    Bump



  3. #3
    Member GerryG's Avatar
    Join Date
    Sep 2018
    Posts
    83
    Downloads
    8
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    You've included no information about the toolbit beyond the diameter and tip profile - what's it made from/coated with, how many flutes does it have? Is it made of some kind of Chinesium of questionable provenance?
    I'm guessing that you're using a router, given the spindle speed and the fact you're using artcam. Are you using any kind of lubricant while cutting?



  4. #4
    *Registered User* izzydog312's Avatar
    Join Date
    Jan 2019
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    1/8 TAPERED ball nose carbine coated, short staffed made for aluminum..... From amunra.com ( the bit company )

    Yes we are using a router, and are useing artcam.... We have a cold air gun and use a little wd40



  5. #5
    *Registered User* izzydog312's Avatar
    Join Date
    Jan 2019
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    looking forward to your reply.... iv also been thinking, maybe were not clearing out enough bulk before we come in with the 1/8 '' tappered ball nose ?

    we've only used a 3/8 end mill to do the bulk on a fairly high detailed mold and still lots of bulk left for the 1/8 ball nose

    first time cutting aluminum obviously so im not very educated



  6. #6
    Member GerryG's Avatar
    Join Date
    Sep 2018
    Posts
    83
    Downloads
    8
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    I'm no expert at routing Aluminium myself, so don't get too worked up about any pearls of wisdom that I'm likely to generate.

    Personally, I'd clear as much out on the roughing pass as possible, and possibly have a light roughing pass followed by a finishing pass with the ball nose.

    I found with doing complex 3d routing on acrylic (obviously not the same, but it loves galling on to the router bit just as much) that it was best to get it as close as I could to 'finish' territory on the roughing pass, then have a couple of sequential passes with the actual finishing bit to get a good finish.

    To minimise the galling, I'd also take a good look at how much cooling you're applying to the work - it sounds to me like you might need more.



  7. #7
    Member
    Join Date
    Jun 2011
    Location
    US
    Posts
    692
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    Quote Originally Posted by izzydog312 View Post
    Here is the feeds and speeds that we are running our bit at : Step over : .18
    Step Down .005
    Feed rate : 60
    Spindle : 20 000 If someone could point me in the right direction, would be much appreciated ! thanks !
    I assume you meant .018" stepover? That's a bit high to get good surface finish, but shouldn't cause welding.
    Your step-down is way too small I think, you'll mostly be cutting with the point of the ball, which is the the worst part to be relying on. I would do a single stepdown, or 1 semi-finishing pass, leaving .005" stock and then a finishing pass. You're probably rubbing more than cutting.
    Feed rate seems too high for such a small end mill at a relatively slow spindle speed. How many flutes? Assuming it's 3, that's .001" per tooth, which would be fine for most square end mills, but for a ball I think it should be derated.

    Quote Originally Posted by izzydog312 View Post
    1/8 TAPERED ball nose carbine coated, short staffed made for aluminum..... From amunra.com ( the bit company )

    Yes we are using a router, and are useing artcam.... We have a cold air gun and use a little wd40
    Link doesn't work and I couldn't find anything about amunra end mills.



  8. #8
    Member QuinnSjoblom's Avatar
    Join Date
    Nov 2017
    Location
    bigfork
    Posts
    591
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    You said coated, but with what? Some coatings are much worse than no coating at all if it's not the right kind for aluminum. Zrn is great for aluminum. As for cooolant, 6061 was a nightmare for me when running dry. Instant chip weld. You said you're using a bit of wd40 which is fine, but are you applying it every couple minutes as it cuts? I use a cheap 20 dollar mist setup from Amazon with kool mist coolant. Works great, never chip welded since. I'm also using what some would consider a "router" but a very rigid one with a 2.2kw Chinese spindle. Check your tool runout with an indicator on the flutes close to the end of the tool, turn the tool backwards by hand to see where each flute peaks at. Runout is very important with these smaller tools. If you have a thou of runout, only one flute is gonna be cutting which means your chip load is gonna be much higher than what you calculate. If you find runout, try turning the tool and the collet in different positions until getting it as good as you can. As others have mentioned, you will benefit from multiple passes. I would rough, then do a semi finish leaving maybe 5 thou, doesn't need to be as fine of stepover for semi finish. For the final pass, you want the endmill taking a consistent amount of material for the whole cut. If it's passing through a variance of material thickness, tool deflection changes and gives inconsistent surface



  9. #9
    *Registered User* izzydog312's Avatar
    Join Date
    Jan 2019
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    Thank you everyone for your suggestions, will be firing up the cnc in a couple days to try some new things.... Things i plan on trying are :

    Changing stepover from .18 to .05

    Useing a 3/8 , 1/4 and 1/8th bit for the rough in, instead of jst the 3/8th bit

    Spraying every so often with wd40

    change stepdown from .005 to . 03

    Anybody have an idea for Feed rate and spindle speed ? a lot of controversy about it online and tough to find the right speeds we are currently running feed rate : 60 and 20,000 spindle speed

    Amanatool.com is the site we get out bits and they are Solid Carbide ZrN Coated

    If anyones got any other suggestions to try, please let me know asap! thanks



  10. #10
    *Registered User* izzydog312's Avatar
    Join Date
    Jan 2019
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    Bump



  11. #11
    Member QuinnSjoblom's Avatar
    Join Date
    Nov 2017
    Location
    bigfork
    Posts
    591
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by izzydog312 View Post
    Thank you everyone for your suggestions, will be firing up the cnc in a couple days to try some new things.... Things i plan on trying are :

    Changing stepover from .18 to .05

    Useing a 3/8 , 1/4 and 1/8th bit for the rough in, instead of jst the 3/8th bit

    Spraying every so often with wd40

    change stepdown from .005 to . 03

    Anybody have an idea for Feed rate and spindle speed ? a lot of controversy about it online and tough to find the right speeds we are currently running feed rate : 60 and 20,000 spindle speed

    Amanatool.com is the site we get out bits and they are Solid Carbide ZrN Coated

    If anyones got any other suggestions to try, please let me know asap! thanks
    Your coating is good, for spindle speed and feed rate, you need to calculate sfm and chip load. This us going to give a different rpm and feed rate for each cutter. I usually go 800 to 1000 sfm on aluminum, but that's with a constant spray of kool mist. For chip load I usually go a bit under a thou with a 1/8, and 2 thou for a 1/4.

    If you aren't familiar with speeds and feeds, watch this video. https://youtu.be/uw8uL2jjEBs



  12. #12
    *Registered User* izzydog312's Avatar
    Join Date
    Jan 2019
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    Quote Originally Posted by QuinnSjoblom View Post
    Your coating is good, for spindle speed and feed rate, you need to calculate sfm and chip load. This us going to give a different rpm and feed rate for each cutter. I usually go 800 to 1000 sfm on aluminum, but that's with a constant spray of kool mist. For chip load I usually go a bit under a thou with a 1/8, and 2 thou for a 1/4.

    If you aren't familiar with speeds and feeds, watch this video.
    Appreciate your reply, curious to what SFM is ? and does anyone know of any easy to use calculators ?



  13. #13
    *Registered User* Rza25's Avatar
    Join Date
    Jan 2019
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default Re: Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball

    Quote Originally Posted by izzydog312 View Post
    Appreciate your reply, curious to what SFM is ? and does anyone know of any easy to use calculators ?
    Hi, 'I use this
    https://play.google.com/store/apps/d...lter_tools.wmc



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

Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball nose

Looking for help with speeds and feeds, machine relief on aluminum with 1/8 ball nose