Need Help!- Suggestions for face milling aluminum

[flathead]

I'm looking for some suggestions on how to properly face mill some cast aluminum parts that I have. I need to make the top and bottoms of the castings flat and parallel. Here's what I'm working with. I have a 3" face mill like this http://www.wttool.com/product-exec/p...tters_Toolmex_
I'm using a CNC'd Industrial Hobbies mill w/Mach 3 and flood coolant. The spindle is a 2hp VFD.

I have done a few parts using the feed and speed calculated by Mach3's surfacing wizard (aprox 1000 rpm, 16.2 ipm). I used .010" depth of cut. The parts look OK, but not great as far as surface finish. They also take quite a while to run because the parts are 20 " x 7" in size.

Should I be able to get more aggressive with my cuts or am I in the ballpark here? What is a "normal" depth of cut for a 3" face mill? This is the first time I've ever used a face mill, so I'm not quite sure what to do. Any suggestions?

thanks

[ddwadley]

Generally you want to take a deeper cut in cast anything... so your tool isn't rubbing on the scale. With that 3.0 Dia tool I would ramp up your RPM to maybe 2500... and you should be able to take cuts much deeper than .01". If you need to don't hesiate to take .125" DOC. .. As for your surface finish... with the RPM running much faster... I bet you could finish at 30 IPM.. and rough at 60 IPM at least.

Hope this helps

[mc_n_g]

Make sure your inserts are ground or polished style. If not I doubt you will get the finish you want. Pay the extra money and get insert for aluminum. They should have a sharp knife edge to them not the pressed edge for insert used on steel.

After you have the correct inserts then do everything dd tells you.

Also the terms 'flat and parallel' have limited meaning. 'Flat and parallel' to what measurement level? You will be limited by the ability of your equipment and clamping pressures.

[Superman]

Originally Posted by mc_n_g Make sure your inserts are ground or polished style. If not I doubt you will get the finish you want. Pay the extra money and get insert for aluminum. They should have a sharp knife edge to them not the pressed edge for insert used on steel.

I agree here. don't use coated anything, all edges must be sharp.

TIP
If you are on an open machine, try a little spray of kerosene to stop the built-up edge happening on the last cut of each face

[Glacern]

As others have stated, use a polished insert with an extra sharp top rake.

Does your facemill use the same SE 1204 inserts as the cutter shown in your link? If so, we have Korloy SEHT1204 (aka SEHT43) X83 inserts for aluminum available on our webstore that should fit the bill. For a starters, try the same speeds and feeds but double or triple your DOC.

Just to show what these inserts can handle, we recently filmed a demo with our 4" 6-flute 45 degree facemill and the Korloy inserts cutting 6061 at .125" DOC, 3000 RPM, and 300 IPM, with a 120% spindle load on a 30hp Mori Seiki VMC. Finishing was done at .015" DOC, 8000 RPM, same feedrate. The video will be available on our website soon.

http://www.glacern.com/fm45

[Glacern]

Originally Posted by ddwadley Generally you want to take a deeper cut in cast anything... so your tool isn't rubbing on the scale. With that 3.0 Dia tool I would ramp up your RPM to maybe 2500... and you should be able to take cuts much deeper than .01". If you need to don't hesiate to take .125" DOC. .. As for your surface finish... with the RPM running much faster... I bet you could finish at 30 IPM.. and rough at 60 IPM at least. Hope this helps

Excellent numbers for a VMC, but they might be a tad aggressive for a 2hp motor...

[flathead]

Guys,

Thanks for all the suggestions. I think that the inserts I'm using must be the problem. I am using the inserts shown in the link in my first post. I didn't buy the cutter or the inserts first hand so I'm not sure if the inserts I have are cheap imports or USA made (Wholesale Tools sells both). But, regardless they are coated carbide.

I think I'll switch to inserts for aluminum. As far as I can tell, WT doesn't offer them. So I may order from you Glacern.

Thanks

[PixMan]

FWIW, I have a friend who machines a lot of 6061-T651 aluminum. The parts he makes are for laser machines, and the surface finish is critical. The customer want no tool marks, and a smooth matte finish.

His current process is to face the blocks off with a 3" diameter 3-insert face mill, a Valenite Economizer. He runs that at 35ipm @ 3500rpm. The finish is good, but he has to tumble the parts to get the matte finish. It takes about 20 to 30 minutes to get the proper finish.

I loaned him my 3" diameter 6-insert Valenite V650 "V-Flash" cutter, loaded with PCD inserts. He now runs at 7500rpm, 225ipm and the finish is 2-4 Ra. Now it only takes 3-5 minutes to turn the mirror finish into the customer's preferred finish as there's minimal tool marks. The cutter is designed so that you can adjust the inserts within a couple of microns and do this with the inserts already snugged-up in the cutter. One shot adjustments, FTW. I think he's going to be buying one of these cutters....I know I want mine back!

[BobWarfield]

Agree completely on the inserts. How did they work out for you?

FWIW, that facemill on cast aluminum pops out the following on my G-Wizard feeds and speeds calculator:

SFM: 1080
RPM: 1400 (which about all she'll do, so that's good!)
Feed: 45 IPM

FWIW, you'll want to make sure the mill is really trammed right. The 3" facemill only makes that even more important.

You don't say what stepover you're using either. You might experiment a bit, but I'd try maybe 65%?

Cheers,

BW

PS You're welcome to try G-Wizard:

http://www.cnccookbook.com/CCGWizard.html

[shukongcn]

I am nc novices













.............................................
CNC programming