Milling aluminum

[cnc@gci]

Can anyone give me some speed and feed rates and advice for pocketeting a plate of aluminum 6061, depth .5 with a .5 end mill. Everyone I talk to tells me something differant. any help would be much appreciated.

[Guest]

Holding it well, with a carbide 3 flute tool and flood coolant, 14,000RPM .25 DOC, .275 step over at 220IPM

 

You didn't mention machine capabilites, tool type or other determining factors

[Guest]

sure depends on your max rpm and machine hp.

i would not hesitate to run it at s10000 f90 ipm

for a start on our haas 15 hp machine.

 

oops that would be carbide for sure.

 

doug

[DaveR]

500-the moon SFM depending on how much RPM you have, .004 feed to start. I'd take .1 DOC personally with a finish pass. Like you wrote there are lots of different ways to do it. Aluminum 6061 is probably as easy as it gets, very forgiving if you are not just so on the feeds and speeds.

[Thee Rickster ™]

High helix works well also

[cnc@gci]

I'm using a Haas HMC 12,000 RPM, 1000 IPM.

[cnc@gci]

This is a fixture plate for machining composites so I want to be on the safe side to get it right the first time.

[Darren Long SPE]

Indexable tool in a balanced Toolholder.

Very Positive High Rake Polished Inserts

AP = 1xD

AE = 1xD

RPM @ MAX (15000)

Feed @ 7000

 

I kid you not!!!!!!!!!!

Check the FTP in High_Speed_Demos

ECR-B3-Solid.avi

 

An example using a Solid Carbide with Air Blast!

[ATG]

High Helix best way to go

[cnc@gci]

Do I have to worry about the end mill building up material?

[Darren Long SPE]

not if there is a sharp cutting edge, it will dull eventually.

Also Air Blast or Coolant should be good.

[Justin Beebe at Folsom Tool]

Destiny Tool makes a great 3 flute carbide endmill for aluminum called "The Viper". I have been very pleased with their performance. It won't build up material. The reason you are getting different advice from everyone is because the feeds and speeds for aluminum are so wide open.

[Guest]

quote:

---

Destiny Tool makes a great 3 flute carbide endmill for aluminum called "The Viper".

---

I LOVE those things

[35K chipper]

here one for ya destiny .5 3flute viper stealth at 30,000 rpm 1400 ipm .05 doc 90% radial mat. 6061 all day long end mill lasts about 100 hrs then i pass it on to the 8000 rpm group. my.02 worth.

35k chipper.

[chris m]

I'd run a 1/2 carbide 2 or 3 fl stub endmill in a milling chuck or ER32 collet chuck wide open at about .004/flute and flood the crap out of it with coolant. Tough to go wrong in aluminum but DO NOT use a 4 flute endmill to rough or you will end up with it looking like an aluminum dowel pin. High helix tools are nice, but a vanilla 2 flute stub endmill will work just fine if that's all you have

[cnc@gci]

Thanks for the advice guys.