Page 3 of 3 FirstFirst 123
  1. #21
    I would cut alloy at 6000rpm and take smaller cuts and go faster on the feedrate with coolant on.
    If the chips get big then it will jam up.
    My machines have flood coolant.
    The ideal would be air jets to blast out the chips.

  2. #22
    On a small mini mill i dont see how a good result will be obtained when deeper cuts than 1mm??? Normal 2 flute carbide cutter 30 degree upcut will give best results all over. 5 euro from China. There are better made for aluminum bits but they are not made for small machines anyway. They are made for serious machines and can give much higher material removal rate, which in this case is not viable.

    What aluminum you are cutting? No name piece of aluminum could be absolute shit to cut. Buy only aluminum alloys made for certain purpose.

    From my experience i can cut using any bit up to 3 flutes. Even straight ones or carbide tipped made for wood only. And result is always perfect. The key i say again is the machine rigidity. Any vibration heats the process excessively and things happen. Use the HSMAdviser calculator and you will see that perfect cut is never so deep as many people think.

    As a general rule of a thumb that perfect cut happens at 12k rpm 1500mm/min 1 mm depth with any bit 6-12mm.


    the tool stick-out is the another detail you should pay attention to. As even if machine is sturdy, the unnecessary stick-out changes the game quite much.


    Click image for larger version. 

Name:	aluminum cutting.PNG 
Views:	17 
Size:	102.8 KB 
ID:	21618
    Last edited by Boyan Silyavski; 1 Week Ago at 06:38 AM.
    project 1 , 2, Dust Shoe ...

  3. #23
    I have some end mills that are the following spec.
    12 diameter 4 flute.
    30mm flute length.
    42 degree helix.
    Solid carbide with a high hardness rating.
    They are what i use for every material.
    I can use them on plastic and alloy and stainless no wories.
    If i am cutting an external profile in alloy i can go full depth cut and cut with the side of the cutter and cut 1mm off the profile at 3000mm/ min with coolant on.
    Internal holes and pockets i just run 0.5mm cuts at high feedrate so it doesnt take long anyway.
    But we dont do high volume work so thats ok to us.
    Maybe if we had a high volume we would have to use specific alloy cutters to speed up internal machining
    Last edited by Ukmiller; 1 Week Ago at 07:48 AM.

  4. #24
    Well, since I originally posted, I've been learning a bit about my mill and no more endmills have been broken.

    I now use the Alu-power carbide 2 flute and 3 flutes from Cutwel. They are a little more expensive but they work well. I know it's overkill but I like good quality sharp and shiny tools :)

    My mill can only do 2000revs. which I always use.

    Using Fusion360 with Adaptive to cut a pocket or remove material I use an 8mm 3 flute cutter, Helix plunge down fairly slowly (20degree angle) to about 6mm depth with a plunge feed of 300 and WOC of 0.5mm. Once it reaches the 6mm depth, I go faster at 350 feed and 0.5mm to enlarge the pocket. Then repeat the same with the next 6mm depth and so on.

    I use no coolant or air, just a vacuum to suck the swarf. No problems at all at these settings.

    It's fairly conservative, I am sure I could go deeper at these settings.

    I have tried more WOC, up to 1mm, but that's when the problems start. The TTS type tools can start pulling out of the collet with the consequent accident to follow.

    I am sure that if I just used a normal R8 collet only, I would be fine with 1mm width cuts, but with an 8mm cutter it seems to be too much force for the collet to grip the TTS tooling properly. It's fine with smaller diameter endmills though.

    Edward

  5. #25
    2000 is quite slow for alloy but if you have no coolant or air then i would say you couldnt go any faster anyway.
    Aluminium melts so easily and can break cutters

  6. #26
    This video shows it all, fairly slow plunging, then faster feed (350mm/m) when it reaches its depth. 6mm tool at 2000revs. Using adaptive, leaving 0.2mm to the sides, then finally Contour to finish off to size. Then a tool change to a chamfer tool. This was a test for small ball bearings holes. They fitted to perfection.




    Edward
    Last edited by Edward; 1 Week Ago at 09:37 AM.

  7. #27
    That shows how you machining very clearly.
    I would get sacked if i machined that slow though!
    But we have 6000rpm and coolant blasting.
    Can i ask why you cut clockwise?
    I always cut holes anticlockwise to reduce chatter.
    Try running the same program the other way to see if it improves the finish you get.

  8. #28
    Quote Originally Posted by Ukmiller View Post
    I would get sacked if i machined that slow though!
    Surely if you had good reason no one could argue

    Quote Originally Posted by Ukmiller View Post
    But we have 6000rpm and coolant blasting.
    And having 3 times the spindle speed would seem to be a contributory factor in allowing you to cut faster?
    If you will not be swayed by logic or experience simply pick the idea you
    like best, but ask yourself why you sought advice in the first place and,
    for a simple life, perhaps consider not doing so in future

  9. #29
    Quote Originally Posted by Ukmiller View Post
    That shows how you machining very clearly.
    I would get sacked if i machined that slow though!
    But we have 6000rpm and coolant blasting.
    Can i ask why you cut clockwise?
    I always cut holes anticlockwise to reduce chatter.
    Try running the same program the other way to see if it improves the finish you get.
    I think I machine at the speed that my machine allows me to, give or take. I could use coolant or air, but I am happy to compromise and go slower without it.

    Regarding climb or conventional milling, as you can see in the video if you have the patience, or fast forward, as I know these videos can be boring, I do the Adaptive clearing in Fusion360 using conventional milling and then as a finish pass I do a last pass (Contour in Fusion360) using climb milling removing the last 0.2mm. This gives me a perfectly shiny and smooth finish, in fact, as good as what I get from any professional workshop.

    Regarding the alloy, I normally use 6082T6 which seems to machine fine to me.

    So I am happy with a general feed speed of around 350mm/min. WOC around 0.5mm at 2000revs. If and when I have the need for faster speeds, I will build myself a nice router and I will study the good advice that this forum contains. Or I will convert a larger mill. I think for the moment I have a nice little mill that is sturdier than many a cheap router, and does what is supposed to do quite nicely, albeit relatively slowly.

    Yes, I broke about 4 endmills at the start, but now things seem to have settled down and if something breaks, it's usually my fault.

    Edward

Page 3 of 3 FirstFirst 123

Similar Threads

  1. Aluminium passivation - for aluminium to be used outside
    By CHudson in forum Metal Finishing Techniques
    Replies: 4
    Last Post: 06-04-2011, 08:18 PM
  2. HELP Gary, I'm having a disaster
    By Robin Hewitt in forum Linear & Rotary Motion
    Replies: 3
    Last Post: 16-04-2009, 09:07 AM

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
  •