Feeds and speeds for aluminum milling

[tgmcg]

I'm using the following feeds and speeds for milling alloy 6061 and Fortal (7075) aluminum plate, bar and billets..

0.250" dia x 2-flute end mill...........15 ipm x 2500 rpm

0.500" dia x 2 flute end mill............8 ipm x 1250 rpm

Endmills are center-cutting TiCN coated HSS

Spindle motor is rated for 3600rpm/3HP w/2-speed gearbox. Am using an inverter for continuously variable speed control between 50-3600 rpm.

Am contrmplating the need to mill relatively large (for me) components from blocks of materials, say 3" x 6" x 14" blocks. These components took quite a while to mill the first time around at the above.

I have not yet tried using roughing mills for initial stock removal, though this seems an obvious thing to try. Seeems logical that an objective should be to remove the most material at powers close to the rated spindle motor power. Can also try carbide tools, but have hesitated doing so since first attempts 2 yrs ago resulted in lot's of broken tools.

I'd be most grateful for any recommendations or comments on how I might reduce my machining time.

Thank you.

Best regards,

Tom

 

[loojian]

As I know,coated HSS can't be used in cutting alloy aluminum material.Using general HSS or carbile.

 

[mrainey]

A lot depends upon what your finished part looks like. In general, rough end milling aluminum is best done with two or three flute tools with lots of chip clearance. I've had best success with relatively shallow cuts coupled with high speeds and feeds. You have to keep coolant at the tool tip - difficult with deep cuts and lots of chips.

Just for facing, think about face mills with carbide inserts. For example, a 3" diameter tool with five inserts at 1400 RPM, 28 inches per minute - .125 depth of cut - comes in at just under 3 HP.

I have a free machining calculator that will give you a wealth of information and let you play "what-if" games with a couple of mouse clicks. Good luck.

http://dl.winsite.com/bin/downl?14500000037133

 

[metman]

I agree with mrainy if you are facing which it sounds like unless you need grooves made by end milling.

Just the other day I used an old fashioned brazed cemented carbide fly cutter with 1-1/2" diameter sweep at 2500 rpm on 6061 using .1" depth of cut (close fpm equivilent to mrainy's 3" dia at 1400rpm). I don't know the feed rate. Was using about 40% of max feed on generic power feed of Bridgeport with 2hp and medium strain on motor.

The single point fly cutter seems to work even better than a multiple insert face mill for hogging (better chip clearnce?). I had one machinist/toolmaker tell me that Bridgeport is not designed to handle the type of face mill I had been using. I am not sure that I understand why. This is a 3" dia tool holder with about 8 carbide inserts.

Jesus is THE life,
Leonard

 

[mrainey]

3" diameter with 8 inserts is a very fine pitch face mill - you're right, probably not enough chip clearance for roughing aluminum.

Rule of thumb for aluminum - positive rake, fewer rather than more flutes.

 

[tjager]

Hi

I would recommend the following tool. ( I am not advertising for that company. Just had great success with their tool)
It is made by AB-Tools Inc. (abtoolsinc.com).It is called a shearhog. Comes in different sizes. We use that tools on our CNC's with speed up to 15000 rpm and 550 in./min at a depth of cut of up to .25. Of course the setup is more rigid than on a Bridgeport. You probably can run that tool (1.5 dia ) at 2700 rpm and at a feed of about 36 ipm at a depth of cut of .25 depth .You can add a bit of spraymist or some Kerosene as a lubricant. It uses little tool pressure because of the way the insert are ground.

Hope this helps

Tony

 

[metman]

Tony,
I think we have that same tool which we use on our Haas verticl mill and KOMO router for Aluminum. I treid it once on the Bridgeport and it works great but B'port can't take advantage of the high rpm which is limited to a little ofver 3,000rpm. Therefore when surfacing a wide swath, the fly cutter can possibly outperform the trick AB Tool unless we have a larger diameter (1.5&quot as you suggest. I will check into this. Thanks for the reminder.

I also like Kerosene for cutting Aluminum but am quickly swtching to WD-40 which smells better and seems to work better albiet more costly. My current boss doesn't seem to object to the cost so why not? I had a previous boss that was touting the benefits of WD-40 and then when I started using it "consertively" because it isn't cheap, the boss criticised me for using the expensive stuff. Is there any accounting for the inconsistancy of bossing?? Go figure!

Jesus is THE life,
Leonard

 

[jbel]

metman,

We have used a 3" shear hog face mill on a bridgeport with great sucess. The investment you make in the tool will more than pay for itself in time saved when compared to any conventionl face mill. The downside is that the bridgeport doesn't have the rigidity to take full advantage of the tool. By that I mean that you cant run it at 3000 rpm if you value life and limb. That being said it is still a heck of a lot more productive than conventional mills.

I think that Iscar has just come out with mills specifically designed for aluminum. SGS Inc. also has a large line of products that work extremely well in aluminum.

One more word of advise. When you buy any of this stuff talk to either the distributer or the factory rep and describe your cutting conditions to them. Then ask them for recommended speeds snd feeds BASED ON YOUR CUTTING CONDITIONS AND SETUP. The shear hog catalog may have some astronomical cutting speed to use but you will not be able to achieve that cutting speed in a bridgeport, and if you could the setup isn't rigid enough anyway.

Good Luck!!!

 

[tgmcg]

I want to thank all of you so much for your kind assistance.

For the most part I'm using 2-flute end mills. The coated endmills "seem" to work okay. Am using Tullco Premier Poly-Cut water-soluble coolant. Since the machine is not equipped with splash guards, any oil-hydrocarbon based coolant would make a huge mess in my shop.

I initial feeds and speeds were obtained using the feed/speed tables in the Machinery's Handbook 26th Edition. However, it is not clear to me how one reconciles the different feeds and speeds quoted for aluminum in Tables 10 versus those in Table 15. For example, Table 10 quotes f/s=15/165 optimum and 8/850 avg for end-milling with HSS. Whereas Table 15a recommends 0.003 ipt for <1/2&quot; dia HSS end mills. 15, 8, 3...which is it??

Generally speaking, I do not exceed 0.5D axial depth of cut with endmills.

I don't do a whole lot of facing. Mostly pockets, drilling and profile cuts......letting the finished part drop through from the stock. Nor do I make many finish passes, the only exception being close tolerance bores. It's all prototype work, so surface finish isn't so critical.

I'm using a Shizuoka AN-S knee mill w/ 3HP spindle motor. It's a pretty stiff/heavy machine relative to a B'port.

Thanks!

Tom

 

[jbel]

McGuinness,

While Machinery's handbook is a great place to look for general references, your cutting tool distributer should be able to dial you in to the optimum speeds and feeds based on your cutting conditions, setup, machine rigidity, etc.
The numbers supplied by the distributer will reflect the technology incorperated into the cutting tools, while machinery's handbook gives a much more general number to work from.

 

[tgmcg]

jbel,

I've been ordering my cutters from McMaster-Carr and ENCO, not the cutter mfg directly.

Do you think the cutter folks will be helpful if I don't order from them directly? I suppose it can't hurt to ask.

Best regards,

Tom