PDA

View Full Version : Carbide Aluminum End Mills?



HAP
07-08-2010, 07:18 AM
Just curious as to why there are carbide end mills specifically desiged to cut aluminum? From what I have read, HSS is sharper and produces a better finish. So, why would there be a need for special aluminum carbide mills? I understand the high helix angles and such for better chip ejection. And as far as the aluminun fusing to the end mill, the high tech coatings are inteded to eliminate this right? My best guess is the carbide should last forever if used exclusively for aluminum...?
Regards,
HAP

JoeFin
07-08-2010, 08:05 AM
Couple months in a production environment

Lew Hartswick
07-08-2010, 08:26 AM
Couple months in a production environment
Plus the folks that just "assume" carbide is better for everything. :-)
...lew...

Evan
07-08-2010, 08:38 AM
Aluminum contains small amounts of silicon in most alloys and aluminum casting alloys may contain very large amounts up to 15 percent. Silicon is very hard and will dull even a carbide cutter.

Plain old 6061 contains up to .8% silicon. That means for every 100 inches of cut the bit will have cut .8 inches of a grinding wheel. The grains are microscopic but they are just as hard as a rock or piece of quartz.

Black_Moons
07-08-2010, 12:44 PM
*pictures milling slots into a 8" bench grinding wheel*

I believe the "For aluminum" carbide endmills are also 'super sharp' so to speak. Much like the 'made for aluminum inserts' you can buy.

And by 'super sharp' I mean 'Has a super fragile edge and would chip in an instant if used on mild steel'

gwilson
07-08-2010, 02:30 PM
Aluminum also instantly forms a very hard,invisible coating of ALO. Every time you cut it,you have to cut that layer.

beanbag
07-08-2010, 03:14 PM
"Made for Aluminum" end mills are not necessarily super sharp. I have a set of CGS end mills where you can rather safely run your fingers along the flutes. I am not sure if this is on purpose, as every aluminum cutting insert I have seen is very sharp. In any case this end mill has a peculiar grind.
http://www.cgstool.com/IMG/IMG.EndMills/2030-UC/2030-SERIES_57x275.jpg
I think the "made for Aluminum" end mills are designed for maximal chip clearance and evacuation. The ZrN coating, I believe, is for when the SFM is so high that the aluminum slightly melts and glides over it. I know that otherwise without coolant and "normal" SFM, you will still get built up edge with this coating.

Mark Hockett
07-08-2010, 03:18 PM
Carbide can run 4 to 10+ times faster so for production it is mandatory. I run all carbide endmills up to 3/4" at my machines highest RPM, 7500 RPM, and then adjust the feed rate for the chip load of the cutter. A typical 3/8" EM will feed at 150 to 180 IPM. My next machine will be a 10,000 rpm machine and I will run that at max RPM. A HSS cutter wouldn't survive very long at those speeds.

macona
07-08-2010, 03:37 PM
There are special HSS endmill designed for aluminum. They usually have a deeper gullet to help with chip evacuation.

I use the ones from Lake Shore Carbide. Variable 3 Flute :http://www.lakeshorecarbide.com/variablefluteendmillsforaluminum.aspx

These things plow through aluminum. The variable flute reduces chatter as it does not build up a resonance. The finish on internal interpolated holes was almost polished.

Heres my mill running a 1/2" bit from Lakeshore. 50ipm and 5440 RPM. Could have gone faster but no enough spindle power.

http://www.youtube.com/watch?v=V7_W9KRe8rc

Evan
07-08-2010, 05:41 PM
Here is a video of my mill with a 26,000 rpm spindle drilling and milling aluminum at high rates using carbide tooling.

http://ixian.ca/gallery/displayimage.php?album=5&pos=0

BobWarfield
07-08-2010, 09:57 PM
Even if you don't have a spindle capable of harnessing the full potential of carbide, consider the issue of rigidity. Further, let's say you're doing some fine features, and can't just slap a big end mill in.

So, let's say you have a 1/4" HSS 2 flute and a 1/4" Carbide 2 flute. You want to cut a pocket 1" deep in 6061 aluminum and you want a reach of 1.25" to allow some leeway. You have a spindle that can only do 6000 rpm.

How do these two compare?

Let's use 1/16" width of cut. For roughing, let's say we're willing to tolerate up to 0.001" of tool deflection. I can use G-Wizard to figure the deflection of the various cuts here.

My HSS will only go about 83 thou deep before it starts to deflect more than that. So, if I have to go all the way down the full inch in steps, it takes 1/0.083 = 12 passes. Painful!

My carbide will go 3/4" depth of cut before I exceed the 0.001" tool deflection allowance. So, I can do the 1" with 2 1/2" passes instead of 12 passes.

Now maybe I can fuss with chip thinning and different depths of cut (HSS will take a higher chipload than carbide most of the time) to make it up, but it's just an example.

The smaller the tool and the further it sticks out, the more rigidity will get to be a bugaboo. Carbide sure helps with that.

Cheers,

BW

beanbag
07-08-2010, 10:16 PM
Macona and Evan:

whatever happened to chip clearing?

Bob:

I think the ideal tool for this job is a reduced neck carbide end mill.

spope14
07-08-2010, 10:19 PM
High chip clearances, coatings you would not use on steel, and the clearance also allows for high rates of coolant to get in there and get the chips out. Ran a job a few months back where a HSS cutter could get 30 SFPM in a 3/4" deep cut on a profile, ran 99 inches at full spindle out (I believe 9000 - newer Matsuura) with a SGS (I beleive that is right) cutter that looks like the cutter pictured above - three flute.

Ran the same three flute slower in a machine without coolant, bound it up fast and on a bridgeport bound up the cutter again (thank goodness for the cutting juice, or the weld would have been permanent. Used it again on the first machine in fear I had ruined it, full coolant going, 6000 RPM at 70 SFPM, like nothing ever happened to the cutter.

Most of the carbide Aluminum cutters are made for the CNC environment with coolants, ability to hit the speed and feed, and not especially sharp as they work less in a sharp cutting manner than making the chips like a negatiove rake cutter might (not saying they are neg. rake, but the action at that speed and feed reacts like that according to those I talk to). Using bridgeport or lower S/F CNC I may go HSS 2 flute or Carbide 2 flute over a three flute special end mill.

macona
07-08-2010, 11:10 PM
Macona and Evan:

whatever happened to chip clearing?

Bob:

I think the ideal tool for this job is a reduced neck carbide end mill.


T was curious how big a pile I could make. Dosnt really matter though, as long as I am not recutting chips it dosnt matter where they are and I can clean them up at one time.

On the job in the video I did not have enough coolant early on and turned one but into a ball of aluminum. Was able to save it though. Put it into some Zep Purple cleaner for a couple weeks and it slowly dissolved the aluminum off the carbide. The Zep is rather caustic.