Hello Guest it is December 10, 2019, 04:56:33 AM

Author Topic: Feeds and Speeds Milling Aluminium  (Read 3171 times)

0 Members and 1 Guest are viewing this topic.

Feeds and Speeds Milling Aluminium
« on: April 04, 2015, 08:05:52 AM »
I’m back again with my favourite stumbling hurdle. I had a very intricate job to Mill in 1.5mm Aluminium sheet. The job is quite small about 120mm x 60mm with quite a few holes and shapes.

I first tried using an 800 Feed Rate and 6,000 RPM with a 4 Flute 3mm End Mill, but it appeared to be labouring the Spindle Motor. I then changed the Feed to 400 and the Spindle Speed to 8,000 RPM.

It appeared to prefer the slower Feed Rate cutting 2/3 of the job but then it seemed to snarl-up  and then my End Mill shattered.

My questions are, am I using the wrong Feed Rate, Spindle Speed, Mill Tool  or is it because I am using too cheap a grade aluminium  ???

As always, any help would be appreciated.



  
God created Ale to make us all happy ..... 8)

Offline BR549

*
  •  6,916 6,916
    • View Profile
Re: Feeds and Speeds Milling Aluminium
« Reply #1 on: April 04, 2015, 05:22:45 PM »
You either need to speed UP the feedrate .  The reason the bit is loading up is you are melting the aluminum and it sticks to the bit. Also you may want to consider a 2 flute or 1 flute bit.

There should be many feedrate calculators on the WEB (;-)


Just a thought, (;-) TP
Re: Feeds and Speeds Milling Aluminium
« Reply #2 on: April 04, 2015, 05:32:28 PM »
Thanks for the reply, really appreciated. I am busy trying to source some decent grade aluminium sheet.

I used to have some aircraft grade; I think it was called ‘Dural’ but as usual, I gave it away. That was brilliant to work with, cut like sheet steel not like this soft crappy stuff I have now. 
God created Ale to make us all happy ..... 8)
Re: Feeds and Speeds Milling Aluminium
« Reply #3 on: April 05, 2015, 06:29:59 AM »
Dural (Duralumin) is an older name for the aluminium-copper alloys now under the 2000 series.  It's an uncommon alloy, really you'd be better off getting 6061 or 6063.

Offline RICH

*
  • *
  •  7,376 7,376
    • View Profile
Re: Feeds and Speeds Milling Aluminium
« Reply #4 on: April 05, 2015, 06:42:44 AM »
Link to info on speeds and feeds. Should cover most anything your going to do.
There are programs that can calculate, but simple look at a chart gets one in the ballpark quickly.

http://www.machsupport.com/forum/index.php/topic,20045.msg138970.html#msg138970

RICH

Offline 2CVer

*
  •  14 14
    • View Profile
Re: Feeds and Speeds Milling Aluminium
« Reply #5 on: April 05, 2015, 09:33:52 AM »
I would suggest that your using the wrong cutter. In alloy you want either a single flute or 2 flute cutter. There are software tools to help with feeds and speeds. The one I use suggests for a 3mm dia 2 flute cutter with a cut depth of 1.5mm the spindle speed should be 16,000 rpm and feed rate 950mm/min for roughing (notice I'm European and don't use inches) and 14,600 rpm and 485mm/min for finishing. The most important thing I've found is chip clearance. You have to be completely paranoid about re-cutting chips, so you need good coolant flood or high pressure mist to blow the chips away otherwise they get stuck to the cutter and it'll break. I generally use a single flute cutter with all aluminium alloys and can still have chip clearance issues if my misters are not getting the chips away. With a 4 flute cutter they will always get stuck because they get trapped in the flute even if you've got good coolant.

If your machine can't go that fast, and you mentioned 8,000 rpm, then the feed rate for roughing should be about 460mm/min and for finishing 265mm/min at 8,000 rpm.

Offline 2CVer

*
  •  14 14
    • View Profile
Re: Feeds and Speeds Milling Aluminium
« Reply #7 on: April 06, 2015, 08:43:50 AM »
Thank you all ever so much for all your help and advice - I know I can be a bit of a pain in the ASS at times especially with questions which have probably been asked a thousand times before, but as an old novice to CNC Milling I find I am learning all the time.

I have put off the job of trying to mill this crap grade aluminium until I first upgrade this rubbish Spindle Motor with something with a little bit of umph and controllability, and secondly when the two flute mills arrive and I can lay my hands on some decent 6061/63 T6 grade aluminium.

Once again thank you to all.

BTW Rich, I already have this Mill Chart - have a bit of a problem understanding it as my knowledge base is still a bit restricted but I am trying !!
God created Ale to make us all happy ..... 8)
Re: Feeds and Speeds Milling Aluminium
« Reply #8 on: April 07, 2015, 08:02:05 AM »
Hi all,
Dural I think is 2014 or maybe 2017 any not much in use anymore. The current material is 2024 and I use it for model aircraft undercarts and the likes. I have to buy it in small
quantities from an aircraft manufacturer and its worth a bloody fortune.
The good thing about the 2000 series (copper additives) is that the material can be heat treated in addition to ordinary workhardening. The piece I have left is T6 H4 grade, ie
workhardened to T6 and heat treated to H4. Its quite hard and machines really nicely and is so much more forgiving than 6000 series which is soft enough to 'smear' and load
up cutters.
I've had reasonable results with 5083 (I think!) which is a marine grade but otherwise similar to 6063.
Somewhat harder to get is 7058, mainly aircraft use, but is heat treatable. Have heard of people making pistons and things like that so real high strength stuff.
Avoid 1000 or 3000 series, real soft stuff for forming and utensils. I have used kerosene as lube/coolant when trying to cut or thread the stuff. Its so gummy it drives you crazy!

Craig
My wife left with my best friend...
     and I miss him!