Everything about machining aluminium, can you help?

I have a litle knowledge about aluminium and how to machine it.
From what i know:
- Very sharp inserts must be used;
- 45 deg, 2 fluts mills must be used;
- HSM milling are not allowed if machine can´t afford at least 60/70HP reliable power;
- Tool coating should be avoied.

I will have to machine a lot of aluminium in next months, lathe and mills will be used to do it. I do not think my knowledge about it is enough to machine the fastest and reliable way i can. What advices can you share about this subject?
Thank you!
Best regards!

Oddly enough, I use almost exclusively 3 flute endmills for aluminum.

HSM paths any time I can get a depth of cut more than about half the endmill's width, while typically using less than 1hp.

Very sharp endmills are a good idea.

I like coatings on my larger roughers.

But then again, I'm not an expert on such things.

ricardo_gt said:

- Very sharp inserts must be used;
- 45 deg, 2 fluts mills must be used;
- HSM milling are not allowed if machine can´t afford at least 60/70HP reliable power;
- Tool coating should be avoied.

Click to expand...

Frankly none of this is canon, except probably sharp inserts.

We use three flutes as much as possible, and aluminum-specific models such as YG's Alu-power or Destiny's Viper. They work very well. Multiple tooling companies are also making higher flute-count tools for HSM roughing and finishing operations to reduce cycle time and increase finish quality. I have two samples right now that are 5-flute aluminum roughers for low-engagement toolpaths.

Lower helix can work well also. M.A. Ford makes an awesome 3-flute end mill we use for some aluminum extrusion (8020 basically) that we use dry. IIRC it's a 37° helix, but I'll try to remember to check when I'm back at work tomorrow.

HSM is absolutely a great idea! In fact it works better on low-power machines, and we utilize it constantly on our Haas and even the Fadal.

Coatings are going to be application specific. The Ford tool I mentioned above has a coating, which is what allows it to be used dry. Every other tool we've tried has clogged up as the aluminum builds on the cutting edges.

ricardo_gt said:

I have a litle knowledge about aluminium and how to machine it.
From what i know:
- Very sharp inserts must be used;
- 45 deg, 2 fluts mills must be used;
- HSM milling are not allowed if machine can´t afford at least 60/70HP reliable power;
- Tool coating should be avoied.

I will have to machine a lot of aluminium in next months, lathe and mills will be used to do it. I do not think my knowledge about it is enough to machine the fastest and reliable way i can. What advices can you share about this subject?
Thank you!
Best regards!

Click to expand...

ricardo_gt said:

HSM milling are not allowed if machine can´t afford at least 60/70HP reliable power

Click to expand...

^^^ I've never heard that one ? Is that like a 50 taper machine and massive aerospace parts... 60 to 70 reliable horse power ?

@ricardo just out of interest what size of parts and size of machines (just to make sure) lol. i.e. metal removal rates that are within two orders of magnitude of what you are actually needing to do.

Also wondering what the max rpm you have for the equipment you are using/achievable surface speed?

Curious as to how much material you have to hog out ?

I will use hyundai mill, 10000rpm.
I was thinking on OSG as tools, they have a sucssess case study at Makino.
The lathe is also hyundai and go only to 3000rpm, so, using enough high feed could break the inserts at no time...
Aluminium is 6061 aluminium.

It’s aluminum...
-2-3 flutes
-anything less than 1xD full slotting is fine, over that 25-33% stepover with HSM paths works great
-wind it up and make sure you compensate the feedrate for radial chip thinning -make sure you get the chips out of the way.

Most importantly balanced material removal and depending on the part a specific roughing operation

What operations will you be doing on the lathe? Deep or large hole drilling/boring?

I have yet to find anything that out-cuts an SGS S-carb in aluminum.
That's not to say I don't have drawers full of OSG, MAford, Kennametal, Niagara, YG1, Benchmark, Lakeshore, ETC, even Accupro!
They all work great. I agree that 3-flutes seems to be the magic number. The more RPM the better, until tool size overcomes machine rigidity.
In 40-taper HAAS's I run maxed out at 12k RPM up to 1/2" dia. 3x LOC. 5/8" is pushing it @ 12k.
When I have to run a 2" LOC or more 3/4" tool for tall stuff I have to slow the spindle.
For example: I run a 1" dia. 3.5" LOC 3-fl full-depth @ 1500 RPM and 30ipm taking about .025" and get a butter smooth finish in a HAAS @ about 40% spindle load.
Which is probably 3hp!

I use 3 flute roughing/finishing in aluminum with a ZrN finish all the time and it works great. I am NOT an expert machinist by any means but we've been running these for two years in aluminum and they're working great for us!

As stated...3 flute s-carb endmills work fantastic. Ground and polished inserts for turning work extremely well also. You can feed 1/3-1/2 the radius roughing in the lathe, with a DOC of 2-3 times the radius. I'd stick with a .03 radius in your case, SFM approx 1000 or better. Aluminum is nothing to be scared of by any means. Good luck.

ricardo_gt said:

I have a litle knowledge about aluminium and how to machine it.
From what i know:
- Very sharp inserts must be used;
- 45 deg, 2 fluts mills must be used;
- HSM milling are not allowed if machine can´t afford at least 60/70HP reliable power;
- Tool coating should be avoied.

I will have to machine a lot of aluminium in next months, lathe and mills will be used to do it. I do not think my knowledge about it is enough to machine the fastest and reliable way i can. What advices can you share about this subject?
Thank you!
Best regards!

Click to expand...

.
if you cannot figure out how to machine aluminum you got problems. obviously can machine aluminum on smaller 1.5hp machines just cannot turn metal into chips as fast as bigger machines. about only thing to watch out for is chips sticking to flutes clogging the mills and drills. many a apprentice has had to use hammer and a screwdriver. coolant helps as well as dont use dull tools
.
biggest thing about going fast and using a lot of hp as you will need you ear plugs as it will sound like a big router.