What's new
What's new

Avoiding Chatter with long tool

Jacob653

Plastic
Joined
Jan 8, 2021
I need to buy a tool and I'm hoping for some help on deciding. Ball endmill, .5" Dia, 3" flute length, 6 overall, 3.25" tool stickout, and carbide.

The thing I want advice on is if I should go 3 or 4 flute when I'm cutting 6061 aluminum. Yes I know that 3 flute is the go to, but because of the large tool stickout and flute length. I'm worried about rigidity and chatter while machining. The machining operation is doing a radius at the bottom of a 3" hole.

Thank you.
 

Jacob653

Plastic
Joined
Jan 8, 2021
@Mike1974 I wanted to use 3" cut length tool because I wanted to finish the wall as well when I'm at the full depth.
 

Delw

Stainless
Joined
Jan 8, 2019
@Mike1974 I wanted to use 3" cut length tool because I wanted to finish the wall as well when I'm at the full depth.

It will work just fine, providing you get a quality cutter. 3 flute like niagra alum mills, Garr alumistars. I use them both, I usually crank my rpms down to 6500 max with a ball I generally run about .025 which of cut at 40 IPM full length then a dry ass or 2 finish is 63 . it cuts better on my Fadals than on my vf2ss.
if your trying to hold a tight roundess call out and better finish slow the rpm up to about 5k
I always rough with a straight enmill if possible
 

Nibleswick

Plastic
Joined
Dec 31, 2019
One thing I found that helps if you are having chatter troubles when you've got a lot of stickout is to lower your spindle speed. Having a heaver chip load stabilizes things, but I'll have to leave it to more knowledgeable and experienced minds to explain why.
 
Joined
Nov 19, 2007
Location
marysville ohio
@Mike1974 I wanted to use 3" cut length tool because I wanted to finish the wall as well when I'm at the full depth.

I do some parts in 7075 with 4" deep triangle shape pockets.. I have Garr make me 6" end mills with 3/4 length of cut and reduced diameter, .020 for 3.5" they leave a beautiful finish I step down in .25 increments. I Had no luck with the end mills you describe.
 

Booze Daily

Titanium
Joined
Sep 18, 2015
Location
Ohio
The 2 posts above mine are my go to tricks.
Slow spindle speed. Sometimes really slow.
Step down and make multiple passes til you’re at your finish depth.

Also one more trick to add. Make a small arc move in the corners. If you just plow in there it’s going to chatter every time.
 

OVodov

Plastic
Joined
Sep 10, 2019
The best recipe in this case is to use proper holder. I would avoid of using collet chuck or weldon chuck. Shrink fit, milling chuck or hydraulic chuck are better choice.
I used kennametal and IMCO and they work great. So any carbide tool can work up 6 times length.
 








 
Top