Need Help! CNC cutting alum. bracket (2d). - need some feeback please.

Results 1 to 10 of 10

Thread: CNC cutting alum. bracket (2d). - need some feeback please.

  1. #1
    Member
    Join Date
    Jul 2013
    Posts
    608
    Downloads
    0
    Uploads
    0

    Default CNC cutting alum. bracket (2d). - need some feeback please.

    Hi guys, its been a while since I have posted / used my CNC for that matter.

    Yesterday I designed and cut a bracket out of T6 Alum from a .25" thick stock.
    The bracket is 0.125 thick so I used a pocketing operation to mill the top down to that thickness.

    Here are my milling settings:

    Cutter, 1/4" 4 Flute (https://www.amazon.com/gp/product/B0...?ie=UTF8&psc=1)

    RPM- ~8,000
    Feed: 30 IPM (maybe I should have done 20IPM?)
    Tool Step over: 25% (1/16")
    Depth of Pass: 0.0125" (10 depth passes to a final depth of 0.125")

    Cut direction: "Mixed"

    1- What is usually the cause of a high pitch screeching sound. At some point the cutting action would make a high pitch sound for a second(s). Most always at the same places.
    2- What is the best way to minimize tool marks on the bottom of a pocket or face; or better yet what caused them? (see photos).



    Here is a video, notice the screeching at the corners - I am guessing it doesn't like to "upcut" ? (which unfortunately you always either cutting one side of a parts interior features downcutting or upcutting.

    http://&#91;<a href="https://youtu.be/jg...U7cMKHgmQ]</a>

    Similar Threads:


  2. #2
    Member KH0UJ's Avatar
    Join Date
    Jul 2016
    Location
    Philippines
    Posts
    660
    Downloads
    0
    Uploads
    0

    Default Re: CNC cutting alum. bracket (2d). - need some feeback please.

    I think the best and easiest way is to use a 3mm aluminum material in the first place to avoid refacing the aluminum material, for me the most efficient bit in outlining aluminum is the 1/8 single flute bit @ 24K rpm, pass will be 0.2mm @ 400 feed rate, in refacing stuff I dont usually use the CNC, we have a high speed surface grinder in the shop so most likely if it needs to be refaced the quickest way to do it is to load it in there. but still you can use the CNC but it takes a long time to finish. if time is not an issue then I guess it`s OK then.



  3. #3
    Member
    Join Date
    Jun 2005
    Location
    USA
    Posts
    1723
    Downloads
    0
    Uploads
    0

    Default Re: CNC cutting alum. bracket (2d). - need some feeback please.

    Your feed and speed looks ok and DOC is light, either your machine is not rigid enough or your import carbide cutter could be the issue. High pitch noise is your machine telling you something is wrong. First I would bump spindle up to 10K and my guess noise would have stopped quickly

    Russ



  4. #4
    Member
    Join Date
    Jul 2013
    Posts
    608
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by KH0UJ View Post
    I think the best and easiest way is to use a 3mm aluminum material in the first place to avoid refacing the aluminum material, for me the most efficient bit in outlining aluminum is the 1/8 single flute bit @ 24K rpm, pass will be 0.2mm @ 400 feed rate, in refacing stuff I dont usually use the CNC, we have a high speed surface grinder in the shop so most likely if it needs to be refaced the quickest way to do it is to load it in there. but still you can use the CNC but it takes a long time to finish. if time is not an issue then I guess it`s OK then.
    Wow, that is very fast, but you are also taking half at least pass.

    Do you typically want to run the spindle faster than slower for alum ?



  5. #5
    Member
    Join Date
    Jul 2013
    Posts
    608
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by CNCMAN172 View Post
    Your feed and speed looks ok and DOC is light, either your machine is not rigid enough or your import carbide cutter could be the issue. High pitch noise is your machine telling you something is wrong. First I would bump spindle up to 10K and my guess noise would have stopped quickly

    Russ
    My machine is pretty rigid. It's one of those 8020 cnc router pro rigshop. I was always under the impression that because alum would heat up I should run a low rpm. However reading glasses you post and the post above, maybe I should try to bump it up some more. Also, don't you runderstand spin a 4 flute slower than a 2 flute? And also do the you want to spin larger end mills slower?

    Thank you for the replies.



  6. #6
    Registered propellanttech's Avatar
    Join Date
    Sep 2011
    Location
    United States
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default Re: CNC cutting alum. bracket (2d). - need some feeback please.

    I would also choke up on that tool some more. I typically do not want much shank out of the collet. The more tool shank sticking out, the more the tool can flex.

    James L



  7. #7
    Member KH0UJ's Avatar
    Join Date
    Jul 2016
    Location
    Philippines
    Posts
    660
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by FoxCNC1 View Post
    Wow, that is very fast, but you are also taking half at least pass.

    Do you typically want to run the spindle faster than slower for alum ?
    On my experience using a 4 flute bit is only for 8000 rpm below spindle, rule of thumb is the more flute = lower rpm higher torque spindles, on a 24k rpm spindle the max torque of the motor is on max speed, a cheap self made 1/8 carbide bit is good enough on this rpm range, using a 4 flute @ 24k by the time it goes in contact with the aluminum material it will quickly fill the teeth gaps on it, then by the time it's filled, it will create so much heat then melting the aluminum even more then it will get dull and eventually shatter due to super heat generated, and it happens in a blink of an eye, a single flute carbide @ 24k is more than enough to cut aluminum without super heating the material itself, you can run it for three straight days (8 hours a day) without sharpening it, a good coolant is also a one factor to continuously lubricate and cool the tip of the bit which for me l just use cooking oil + kerosene (50/50) good enough to cut a thousand parts aluminum materials.




    Blank tungsten carbide rod I used. sharpen it using a carbide grinder (Green Stone)



    4mm aluminum, 1 hour and 6 minutes not including the bending and tig welding.



    Custom Radiator Guard for CRF250, 3mm aluminum, 2 hours and 30 minutes in each side.



    3mm aluminum Custom plate number holder, 6 minutes per piece.

    Attached Thumbnails Attached Thumbnails CNC cutting alum. bracket (2d). - need some feeback please.-tungsten-carbide-rod-jpg   CNC cutting alum. bracket (2d). - need some feeback please.-skid-plate-jpg   CNC cutting alum. bracket (2d). - need some feeback please.-crf250-radiator-guard-jpg   CNC cutting alum. bracket (2d). - need some feeback please.-6-jpg  

    CNC cutting alum. bracket (2d). - need some feeback please.-custom-made-single-flute-carbide-bit-jpg  
    Last edited by KH0UJ; 03-27-2017 at 11:33 AM. Reason: Spelling Correction due smartphone typo error, Pictures added


  8. #8
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: CNC cutting alum. bracket (2d). - need some feeback please.

    Quote Originally Posted by FoxCNC1 View Post
    Hi guys, its been a while since I have posted / used my CNC for that matter.

    Yesterday I designed and cut a bracket out of T6 Alum from a .25" thick stock.
    The bracket is 0.125 thick so I used a pocketing operation to mill the top down to that thickness.

    Here are my milling settings:

    Cutter, 1/4" 4 Flute (https://www.amazon.com/gp/product/B0...?ie=UTF8&psc=1)

    RPM- ~8,000
    Feed: 30 IPM (maybe I should have done 20IPM?)
    Tool Step over: 25% (1/16")
    Depth of Pass: 0.0125" (10 depth passes to a final depth of 0.125")

    Cut direction: "Mixed"

    1- What is usually the cause of a high pitch screeching sound. At some point the cutting action would make a high pitch sound for a second(s). Most always at the same places.
    2- What is the best way to minimize tool marks on the bottom of a pocket or face; or better yet what caused them? (see photos).



    Here is a video, notice the screeching at the corners - I am guessing it doesn't like to "upcut" ? (which unfortunately you always either cutting one side of a parts interior features downcutting or upcutting.

    http://&#91;<a href="https://youtu.be/jg...U7cMKHgmQ]</a>
    8000rpm X 4 flutes x .0027" chipload = 86.4ipm. You're running your machine too slow. Also too shallow - you're using too much of the tip of the tool which is the most inefficient part. Toolpath is another thing. If you have Fusion360 or other, try a high-speed (constant engagement) toolpath. If you're using traditional offset toolpath then you'll have increased tool engagement at the corners, then you'll have to compensate by running slower, or set your machine to exact stop (or set your CV angle higher.) Some form of lubricant, as well as coated endmills (TiN, ZrN, CVD) helps a lot. Also, with traditional offset toolpath, use climb cut.

    If your machine cannot cut at that speed, use a tool with less flutes and plug into the formula.

    Looking at this part, another way to get a good finish is to set a boundary twice larger than the diameter of your tool, and use a zig-zag toolpath. The tool won't be making turns on the material itself, which should improve the surface (and give a nice prismatic effect.)



  9. #9
    Member
    Join Date
    Jul 2013
    Posts
    608
    Downloads
    0
    Uploads
    0

    Default Re: CNC cutting alum. bracket (2d). - need some feeback please.

    Great responses (and pictures) that I missed. thank you everyone.
    I don't use fusion since I have inventor.. and the CAM for inventor is pricey. I have also invested in Rhinocam... =(

    - - - Updated - - -

    Sound like I want to get a tool with less flutes.



  10. #10
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: CNC cutting alum. bracket (2d). - need some feeback please.

    Quote Originally Posted by FoxCNC1 View Post
    Great responses (and pictures) that I missed. thank you everyone.
    I don't use fusion since I have inventor.. and the CAM for inventor is pricey. I have also invested in Rhinocam... =(

    - - - Updated - - -

    Sound like I want to get a tool with less flutes.
    Just bring your parts from Inventor into Fusion and use Fusion's CAM... it's free for hobby use, so why not?



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

CNC cutting alum. bracket (2d). - need some feeback please.

CNC cutting alum. bracket (2d). - need some feeback please.