What's new
What's new
By:
Advanced search…

You guys that cut Aluminum...

Motorsports-X

Motorsports-X

Hot Rolled
Joined
Nov 22, 2014
Location
Texas
I have cut hard steel for years, so forgive my inexperience with this soft stuff..

got a 3 flute .750 end mill using a 1" depth of cut (stick out is 4.00)

Calcs are telling me to run it at the max RPM with about a 120ipm feed rate. Thing is, I Dont want to burn up this tool SOO.. where should you run it for life, vs speed?

Standard way of doing thing brings you in under 2200RPM, but im not sure how the ZrN coating makes these things live?

Anways, just some generic aluminum cutting advice would be appreciated!
 
Motorsports-X said:
I have cut hard steel for years, so forgive my inexperience with this soft stuff..

got a 3 flute .750 end mill using a 1" depth of cut (stick out is 4.00)

Calcs are telling me to run it at the max RPM with about a 120ipm feed rate. Thing is, I Dont want to burn up this tool SOO.. where should you run it for life, vs speed?

Standard way of doing thing brings you in under 2200RPM, but im not sure how the ZrN coating makes these things live?

Anways, just some generic aluminum cutting advice would be appreciated!
Click to expand...

400 sfm in alum? sounds a bit slow even for HSS.

Run it at max speed like the calc suggests.
 
max speed according to the calc is 12000 rpm (2700 sfm) at 109ipm

how is tool life going to be at that speed?
 
nothing is too fast for aluminum. have hit up to 2000 SFPM with the right conditions...

3/4" is a very large cutter diameter for aluminum slotting at an inch depth (assuming full WOC since you didn't specify), make sure your vise is bolted down properly..
 
This is a 3 flute made for Ali? Carbide? Machine?................. Run the snot outa it.........................oh, and you really can't burn up in Ali.................just make it weld to the cutter and ruin your day. The stick out is what will limit your cut. You may have to reduce your radial depth of cut.
 
sorry Im dynamic milling with a .2 engagement down the contour to 3.5" deep.

I'm only concerned because someone else's money, and this is a 400 dollar end mill.. need it to last through a significant amount of parts

12000 rpm 112ipm (deflection limited according to the calculator) lifetime 423%

6000RPM 40ipm 2094% lifetime


seems like a lot of deflection for a .750 carbid tool... but ok..


the other thing is.... 2000% of what? ive never liked that about this calc.. what is 100% lol.
 
The other element not being discussed is the machine this is on. Can your machine handle that cut? Have you ran the horsepower calculations to make sure your machine can handle the cut?

My CNC mill is a 8K RPM spindle and can put a 1" EM in it. It will stall out immediately with that cut because it is only a 1HP Mill. :D
 
I run a 3/4" SwiftCarb Rampmill ~9800 RPM 300 IPM at 2" DOC and .103" WOC. In a Haas VF6SS. In a sidelock. That maxes out at about 130% spindle load (IE when it's actually feeding at 300). According to SwiftCarb's online calcs that's an 18HP cut. In your case I might back the radial down a bit to start with but otherwise shouldn't be too bad. What's the machine and tool holder?
 
Like other guys already said, there's no such thing as too fast in Al (6061 at least) as long as you have the right coating (or no coating at all is better than some coatings) and keep the chips out of the cut.

Is your tool a necked or reduced-shank 3/4"? You said 1" DOC and 4" stick-out.

I've run 1/2" ZrN tools at 16,000 RPMin 6061, for, like, a really long time. Dozens of hours of cutting time? Can't say I've ever had one "burn up". Coating wears off eventually, or Mr Slammy comes along and breaks it, but burn it up, in Al? I don't think so.

Regards.

Mike
 
What machine?

Whatever your max rpm is. I run everything at 16k in 6061 unless I get into chatter. I run A 2" facemill at 16k and 200ipm. It's cut 16.5k linear feet and inserts still look new.

Don't worry about wearing it out. I have many endmills that have been in my Speedio for a year and have A LOT of cut time on them.

I don't care for coating for aluminum unless it's Destiny's Stealth coating. The ZRn coatings round the edge over making for more load and a not very nice finish. At least all the ones iv'e ran.
 
Pay attention to the toolholder too, if you really work a long tool it can "wobble" it's way out of the holder. It might be a good application for a short sidelock holder to ensure it can't come out. If it's a Haas machine be sure the drawbar isn't worn out (broken bellevilles).
 
Machine is a brand new vf2ss with 30 horses. (so 20 lol) 12k spindle

i backed the radial down to .180 and im going to run it around 6000/50 for a bit and work my way up and see how it runs.

You guys pushing these things 200/300 ipm.. the calc says im deflection limited anytime I approach 100... The neck is .712 for 3.375 (from the tip) I would figure that a .020 chip load would be within the tools limit, but maybe im wrong? at the speeds im getting out of the calculator, chipload is like .004 hell thats probably going to rub the tool to death lol
 
I read the other day (I think in an old Modern Machine Shop article) that with current machining technology we don't even come close to the max SFM in aluminum (obviously this depends on the type of machine). I wish I could find the article but it eludes me.
 
dksoba said:
I read the other day (I think in an old Modern Machine Shop article) that with current machining technology we don't even come close to the max SFM in aluminum (obviously this depends on the type of machine). I wish I could find the article but it eludes me.
Click to expand...

I remember that article but can't remember where I read it either (I was thinking CTE but couldn't find it there either). IIRC it was about 20k surface feet is the top limit. Can't imagine that testing.
 
im betting the limit isnt the rpm, probably machine acel and decel. 20k sfm isnt to hard to get to with a big tool. but you would have to let that thing eat at 900ipm
 
You must log in or register to reply here.

Similar threads

S
Newb to machining looking for some advice on milling aluminum
Replies
7
Views
1K
rjwalker1973
rjwalker1973
dandrummerman21
3/4" 4 Flute Variable AlTiN vs 3/4" 3 Flute ZrN Endmill in Aluminum Bronze Alloy?
Replies
8
Views
2K
exkenna
exkenna
G
Phase Perfect PT-355 shutting off.....?
Replies
12
Views
8K
gearsoup
G
J
Melting Aluminum and Clogging Endmills
2 3
Replies
46
Views
20K
706jim
7
6061Mike
Need help with small tool stepover, doc, etc...
Replies
17
Views
4K
wheelieking71
wheelieking71








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top