[DerHammer]

Hi, I was wondering if anybody could give me a good feed and speed for face milling aluminum plate with around an 8 blade shell mill? will coolant give the best finish and what rpm should I do also?

[djr76]

Depends how big your cutter is but pretty much a wide range of speeds. Start around .004 inches per tooth.

[GaryCorlew]

it depends a lot on your horse power and the type of insert, here is what I use 2000 rpm 64 ipm. But these are big thick parts and I have them very rigidly held down. I get just about a mirror finish which our customer is looking for. You would be much better off if you would ask your tooling supplier like I did.

[DerHammer]

Its a 3" shell mill, which looks wicked aggressive =). I also have a 5hp spindle if that helps. Should I be running coolant to get the best finish?

[fpworks]

Its a 3" shell mill, which looks wicked aggressive =). I also have a 5hp spindle if that helps. Should I be running coolant to get the best finish?

GaryCorlew said it right...get your feeds/speeds from the tooling supplier or manufacturer. YES, absolutely run flood coolant.

[DerHammer]

My shell is made by moon cutter Co out of Connecticut. I went to their website but couldnt find any data on recommended feeding speed and RPM but I did find a material data safety sheet....

Anyways, not sure if this helps or not. but I inspected it a little closer this time and its a 3 inch HSS Shell mill with with 12 blades "not removable inserts". So its the type you throw away when its dead. thanks for the advice though, ill be sure to keep the coolant flowing when running it.

[Geof]

....Anyways, not sure if this helps or not. but I inspected it a little closer this time and its a 3 inch HSS Shell mill with with 12 blades "not removable inserts". So its the type you throw away when its dead. thanks for the advice though, ill be sure to keep the coolant flowing when running it.

You do not necessarily throw it away, these cutters can be re-sharpened.

With HSS on aluminum your sfm should be around 500 - 600, possibly a bit slower; I am going from memory here not having used this type of cutter for a long time. For 3" dia you will be using 500 - 600 rpm and with only 5 hp available you are going to be limited in your doc and feed. I would stay below 0.10" doc and try something conservative like 0.001" per tooth for the feed. This gives you 0.012" per rev or around 7ipm. Bump the feed up if things are going okay and the motor is not bogging down. Flood coolant is a good idea but you could get away with just a mist or even squirting coolant on by hand.

[DerHammer]

thanks. Wow, I'm glad I asked because here I thought I was supposed to run the shell mill at like 2000rpm or something much much higher than you suggested. I've read some post on here where some suggest cranking it up and finding out what it will do. I personally like to play cautiously when I don't really know what I'm doing and learn what I can before hand.

So then, I should be running a slower rpm and feed rate for the best finish. 7 IPM is much slower than I anticipated. Another nub question then, what exactly is doc?

[Oldmanandhistoy]

Another nub question then, what exactly is doc?

Depth of cut

[Geof]

If you had a carbide insert face mill you probably would be able to run at 2000rpm; that is equivalent to 1800fpm cutting speed which is acceptable using carbide.

There is nothing wrong with cranking things up but it is a good idea to start conservative; I did say bump up the feed if the motor can drive it without bogging down. When you have accummulated few years experience then you can dive in like a maniac on the first cut .

[Fremont Dave]

I run my 3.1 inch x 3 tooth face mill at 2000RPM and 23ipm and flood on but the teeth are carbide. I've run it faster and with more aggressive feeds but I work in my garage in a dense residential so I try to keep the noise down.

[DerHammer]

So today I actually faced a few aluminum plates. I ended up feeding at around 15 IPM about with my 3" 12 blade HSS shell. I had the spindle set around 750-800 RPM and my doc was taking off about .005.

So now I have another question. No matter what combination I seem to try between feed and RPM, I end up with small ridges on the seems between the passes. There not drastically horrible, but they are there, which bugs me. If I had to take a guess, I would say that there maybe around .001 give or take a little judging from how it feels. Can anybody tell me what usually causes this, and what should I try next to break em down flush.

[GaryCorlew]

What do you have for a machine? If its one of the little bench top types and the and the ridges are all on one side of the cut, then the spindle may not be square. Are you serious with the .005 doc?? thats like watching paint dry!

[Fremont Dave]

Ordinarily I'd look at cutter deflection or stock relaxation in a tight vice but that would seem unlikely with a .005 deep cut. If you are using a knee mill, check your spindle alignment to your table. Mount an indicator on a boom which sticks out several inches radially from your spindle. Set your table so the back edge is under the spindle. Sweep the indicator in an arc on your table surface in a large arc. If the spindle alignment is perfect, the indicator won't move. If the indicator changes, it is telling you your spindle is not aligned to some degree and you can probably adjust most of it out.

[DerHammer]

I have a webb cnc knee mill from 1987 with an older fanuc 0m controller. Weights about 4000lbs, 40 taper, 5 hp spindle. Basically a Bridgeport clone similar to the old BOSS bridgeports. Its a rigid column machine which is exactly what concerns me. I fear it might just be an older machine and there could be some table sag or something. In either case, is the squareness of the table to the quill the only thing which would cause this like I fear? because if thats the case, then theres nothing I can really do about it since I have no way that I'm aware of to adjust the column .

[mxtras]

It wouldn't hurt to tram your spindle to see where it sits. It's a likely culprit.

Scott

[DerHammer]

I'm not familiar with what tramming means, can this be done to a machine with a rigid column?

[DareBee]

If you are running dry, the ridges could be caused by chip welding on the teeth. It minimum wipe a little cutting oil on the surface between passes.

[wilper73]

The lines in your materal might be caused by healing of the mill, that is the the the insert is cutting the materal left behind and being cut on the back side. Unless you slow your feed way down and increase you spindel speed you are most likley going to get this condition. and when looking up speeds and feeds try using this link, http://www.americanmachinist.com/Cal...eedsFeeds.aspx
but this may be for carbide.
good luck

[DareBee]

If you figure your cutter is "heeling" (it will only do so in 1 direction) cut from the other side.
At 1 place I worked, the "rough out mill" was deliberately set .002 out of tram just because face milling DOES work better with a small tilt (is easier on the inserts too).