Milling Aluminium

Results 1 to 11 of 11

Thread: Milling Aluminium

  1. #1
    Member
    Join Date
    May 2010
    Location
    Australia
    Posts
    122
    Downloads
    0
    Uploads
    0

    Default Milling Aluminium

    Hi,

    I tried milling aluminium for the first time today and it ended with a complete fail - one broken endmill and a very quick 3 successive failed attempts.

    My first attempt was to do a 1mm pass then followed by a finishing pass of 0.53mm to break through the material. EDIT: 3.175mm/1/8" 2 flute carbide.

    @ 457mm/min - I cancelled the first attempt because the z axis appeared to bounce around.

    @ 457mm/min The second attempt ended when my endmill snapped off after I decided to just go for it anyway.

    @200mm/min The third attempt I tried cutting the material in two passes 0.765mm at a time. Again the machine was not smooth at all so I just cancelled the operation and called it quits.

    My spindle speed was 9000RPM for all attempts.

    Attached are the images from the attempts. I didn't really care about exactly where the cut was as long as it was in the ballpark so I just zerod the machine after each attempt by eye, so the attempts are one on top of the other so it looks messier than it was each attempt but not by much.

    Any suggestions as to how I might succeed if at all? I've got a chinese 6040 /w a 300w spindle. I've got a 2.2Kw spindle coming but from my very small induction into metal milling I read that aluminium should be milled at a low RPM, so I don't really know if a powerful spindle will make any difference. Mine didn't grind to a halt.

    It's not unheard of for these machines to mill aluminium and I've even seen someone very optimistic succeed with steel so I'm not sure what I'm doing wrong to be honest.

    Similar Threads:
    Attached Thumbnails Attached Thumbnails Milling Aluminium-20161129_000615_1480338468191-jpg   Milling Aluminium-20161129_000602_1480338468503-jpg   Milling Aluminium-20161129_000502_1480338468598-jpg  
    Last edited by Atomic_Sheep; 11-28-2016 at 09:17 AM.


  2. #2
    Member
    Join Date
    Jun 2005
    Location
    USA
    Posts
    1723
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Two questions.

    1) what kind of endmill are you using. Carbide? Steel? Now many flutes? 2, 3, 4, 5 ? what size? 1/8", 3/16", 1/4" ?

    2) What is your depth of cut?

    I don't know about the 300W spindle does not sound like that has the power required but the 2.2Kw will cut aluminum with no issue.

    Russ



  3. #3
    Member
    Join Date
    May 2010
    Location
    Australia
    Posts
    122
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Oh totally forgot to mention my endmill, it's a 3.175 i.e. 1/8" carbide 2 flute endmill.

    My depth of cut was 1mm for the first 2 attempts and 0.765mm for the second.



  4. #4
    Member
    Join Date
    Jun 2005
    Location
    USA
    Posts
    1723
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Set the spindle speed to 9000 RPM
    Set DOC to .5mm
    Set Feed to 254mm/min

    Also what kind of aluminum are you using? Many aluminum are gummy and they do not cut well. If you have 6061 and you use the parameters above it should cut just fine.

    Make sure you use a new sharp endmill, and if you start to hear a lot of noise try a shot of WD40, you can adjust feedrate to control the noise as well. A noisy cut means it is struggling and you need to reduce the speed.

    Russ



  5. #5
    Member dharmic's Avatar
    Join Date
    May 2015
    Location
    Australia
    Posts
    1422
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Do you have access to a feed and speed calculator? FSWizard Lite is a freebie, I think, and has setup for aluminium.

    Tool stickout length is really important when determining your DOC because, especially on small cutters, it has a huge impact on deflection of the tool. For 15mm stickout (ie total tool length protruding from chuck) and 0.5mm DOC and, assuming a 9000RPM max on your spindle, I'd be pushing more like 600mm/min feed rates to avoid burning the cutter. I'd also be pretty handy with either WD40 or - my fave for ali - a 20/80 mix of methylated spirits and water. It's important to keep the cutter lubricated so the aluminium cuts clean and doesn't build up on the cutting edges.



  6. #6
    Member
    Join Date
    May 2010
    Location
    Australia
    Posts
    122
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    I've been using trial versions of GWizard and HSMAdvisor. GWizard gave me a feedrate of 457, HSMAdvisor gave me a feedrateof 202.

    I'm cutting 6065 T5.

    I was using machine oil for lubricant.



  7. #7
    Member
    Join Date
    May 2010
    Location
    Australia
    Posts
    122
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Aluminium 2 Me 0... decided to drill along the cut to easily saw the bit, broke the drill bit, was a 3mm drillbit. Started with ~600mm/min plunge @9000rpm as per GWizard, the Z axis was jumping around like crazy... would bend under pressure when inserting, then it would bounce back once the drill bit penetrated the material, slowed it down to 400, still was jarring the Z-Axis, slowed it down to around 200mm/min (I think this is what HSMAdvisor recommended), seemed to be going better, but still broke the bit in the end.



  8. #8
    Member
    Join Date
    Dec 2009
    Location
    Australia
    Posts
    166
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Quote Originally Posted by Atomic_Sheep View Post
    Aluminium 2 Me 0... decided to drill along the cut to easily saw the bit, broke the drill bit, was a 3mm drillbit. Started with ~600mm/min plunge @9000rpm as per GWizard, the Z axis was jumping around like crazy... would bend under pressure when inserting, then it would bounce back once the drill bit penetrated the material, slowed it down to 400, still was jarring the Z-Axis, slowed it down to around 200mm/min (I think this is what HSMAdvisor recommended), seemed to be going better, but still broke the bit in the end.
    I just put these values into Gwizard 3mm Hss Twist drill Aluminium 6061 and it comes up with 11061 Rpm 195.2 mm feed rate peck 5.334mm
    With Gwizard and 20k rpm spindle you need to set KW Limit to 0.02 kw to get close to where you need to be even with that low Kw rate you can 1/2 the supplied values
    The values for your first cut using the 3mm end mill should have been closer to 24k RPM 1mm Cut depth 180.9 mm feed rate 185.4 plunge again until you know the capabilities of your machine you can 1/2 these values .
    Aluminium milling can be a real pain you need to use CRC or flood cooling to get resoneable results.



  9. #9
    Registered
    Join Date
    Nov 2016
    Location
    United States
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Try moving at a feed rate of 5-10 with rpm of 2500. This is how I run aluminum at work and it does just fine. Make sure your (Z) axis isn't moving thought that can break any end-mill. It looks like an extrusion so it might be the way ur holding it down. Extrusions are never acurate (FLAT) )maybe your getting vibrations, OR is your machine bolted down make sure it isn't moving as well.



  10. #10
    Member Tkamsker's Avatar
    Join Date
    Oct 2010
    Location
    Austria
    Posts
    1189
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    To learn how to cut Alu did cost me a lot of millers first don't use small mills use single flute suited for plastic shape of millers high feed is necessary to get the heat away from the cut coooling is a must low deepnes of cut use a tenth of diameter


    Gesendet von iPad mit Tapatalk



  11. #11
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: Milling Aluminium

    Quote Originally Posted by Atomic_Sheep View Post
    Hi,

    I tried milling aluminium for the first time today and it ended with a complete fail - one broken endmill and a very quick 3 successive failed attempts.

    My first attempt was to do a 1mm pass then followed by a finishing pass of 0.53mm to break through the material. EDIT: 3.175mm/1/8" 2 flute carbide.

    @ 457mm/min - I cancelled the first attempt because the z axis appeared to bounce around.

    @ 457mm/min The second attempt ended when my endmill snapped off after I decided to just go for it anyway.

    @200mm/min The third attempt I tried cutting the material in two passes 0.765mm at a time. Again the machine was not smooth at all so I just cancelled the operation and called it quits.

    My spindle speed was 9000RPM for all attempts.

    Attached are the images from the attempts. I didn't really care about exactly where the cut was as long as it was in the ballpark so I just zerod the machine after each attempt by eye, so the attempts are one on top of the other so it looks messier than it was each attempt but not by much.

    Any suggestions as to how I might succeed if at all? I've got a chinese 6040 /w a 300w spindle. I've got a 2.2Kw spindle coming but from my very small induction into metal milling I read that aluminium should be milled at a low RPM, so I don't really know if a powerful spindle will make any difference. Mine didn't grind to a halt.

    It's not unheard of for these machines to mill aluminium and I've even seen someone very optimistic succeed with steel so I'm not sure what I'm doing wrong to be honest.
    You can mill aluminum as fast as your machine can move. For 1/4" tools, I use a chipload of .0027" which is just slightly lower than the recommended manufacturer chipload. You can divide that by 2 for an 1/8" bit. by 4 for a 1/16" bit, etc. Your feedrate = chipload X number of flutes X spindle speed. In your case should be around 24.3ipm (617mm/min). On my mini mill I can cut at 150ipm with a 3-flute 1/4" endmill at 19krpm. Adjust your DoC to the rigidity of your machine.

    I always use carbide, preferably coated (ZrN, TiN, CVD), but not necessary with a little lubricant. I never buy cheap Chinese endmills. High grade endmills don't cost that much, and if you have your parameters dialed in, last a long time. This particular aluminum looks pretty gummy, so I probably in this case use a 1/4" low-helix single edge spiral "O" flute endmill. You do NOT want to use a high helix endmill on soft stringy aluminum because that will just make it stringier and gum up your tools. A low helix will shear better, and the single edge will allow you to run a slower feedrate (actually half the double flute speed.)



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

Milling Aluminium

Milling Aluminium