Recommended SFM for 6061 milling/drilling

[couch]

Reason I am asking is because all of the "recommended" speeds and feeds are basically thrown out the window with the length of tools we use at our shop. I just started working at a new shop two weeks ago and I will be doing programming and some setup. I worked in a shop for years but we never had to use tools this small and long before, we rarely worked with aluminum either.

Anyways... Most of the parts we run are five inches thick and require a ton of roughing.

Basic rundown of the tools I've seen being used so far...

1" carbide endmill 2 flute
3/4" carbide endmill 2 flute
1/2" carbide endmill 2 flute
1/2" carbide ball endmill 2 flute
3/8" carbide ball endmill 2 flute
1/4" carbide ball endmill 2 flute

All of the tools listed above are often sticking out by 3",4" and sometimes 5". Chatter is sooo bad.

They are using 6500 RPM at 50IPM with a DOC of .050" (with all of their tools) which sounds like **** while running... obviously. I've been telling them their chip load is not enough, but "thats the way they have always run" so they don't want to change anything...

With the given tools listed above, what SFM should I be using while calculating speeds/feeds (keep in mind the length of the tools)? Obviously we must run them differently compared to tools that are only sticking out an inch or two.

We also drill the back sides of the parts with a .201 jobber drill and it takes forever with the rpm/feed they are using. I don't remember off hand what they are though. What SFM would be best for this application? Length is really of no concern with this since there aren't any chatter/breakage issues, only gumming up the tool. Are there any drill mfg's that offer this size drill with thru tool coolant?

Insert cutters... Surely these would help out with higher feeds and deeper DOC's... One of our mills spins up to 10,000RPM with thru spindle coolant, the other is 7,500 without TSC. As of right now there is no budget with tooling, as far as I know. I am sure they will be willing to spend some money on some quality tools that will outlast and outperform what they are currently using.

Before you guys ask, what the hell is this place doing? The machine shop is only a small part of the production there, and it is often neglected although being very important. The parts we machine are not the end product so surface finishes and cycle times are never questioned.

Basically, if you had an unlimited amount of money for whatever tools to rough/finish large parts out of 6061, aside from new machines, what would you recommend?

Damn, I sound like I've never done this before...

Thanks in advance for any replies.

-couch

[DareBee]

The best move would be to contact a Seco, Ingersol, Sandvik, etc technical rep and have them show you what you need. They will do hands on demos and/or give you money back guarantee trial period.

By the way you are talking, I bet you could cut the spindle time in half with new tooling and adjusted toolpaths.

[Chipload]

Originally Posted by DareBee The best move would be to contact a Seco, Ingersol, Sandvik, etc technical rep and have them show you what you need. They will do hands on demos and/or give you money back guarantee trial period.

A great sales rep with application knowlege is better than any tooling you can buy. Period.

For the time being, is it possible to set-up a shorter length tool to mill half way down or so. Then you would be able to increase the feeds and speeds for the shorter depths compared to the long length tools.

An endmill with a short flute length would be more rigid than an endmill with a long flute length. Also you can increase rigidity of the endmill by choosing one with more flutes because it will have a thicker cross section provided that the flute gullets are large enough to carry the chip out of the cut.

Speeds a feeds can vary greatly on the type to endmill that you use for aluminum. For general purpose carbide endmill try 600 to 800 SFM with a chipload of .008-.01 for a 1 inch endmill. For other tool diameters use the chipload for a 1 inch endmill and multiply it by your tool diameter. So a chip load for a 1/2 diameter tool would be .5*.008 = .004 chipload on a 1/2 inch tool. As far as depth of cut, start shallow. Once it works good increase the depth of cut until the machine begs for mercy. Keep in mind if your width of cut is less than the radius of the tool, the feedrate can be increased accordingly. There is a formula for that application but I do not know it off hand. I am also assuming that you are using a CAT 40 taper milling machine.


As for drilling 6061 with a HSS twist drill I use 220 SFM. Feedrate 18ipm to +25ipm. If the chip is wrapping around the drill, increase the feedrate. Peck depth about 60% dia of drill. If it is working good, take fewer pecks until the drill gulls up.

[couch]

Solid. Thanks guys.

-couch

[PixMan]

Originally Posted by Chipload A great sales rep with application knowlege is better than any tooling you can buy. Period.

Why thank you! That's the first time anyone has ever validated the 30 years of making chips I did before I went to sales. And I continue to learn everyday that I'm in the field, seeing what other shops are doing. I try to be helpful without being a know-it-all. And if I sell them some productivity improvement and/or cost-saving tool, it's a win for both of us. If you're doing well with what you have, I admit it and ask for other opportunities. No hard sell required, just guaranteed tests.

[maz43]

A great sales rep with application knowledge is better than any tooling you can buy. Period.

Great advice-I couldn't agree more. Tooling keeps getting better and better.

I get 100 IPM, .300 DOC 75% cutter width roughing with a Korloy insert mill in 6061 T6 aluminum. Tool length is about three inches though.

[dertsap]

are the tools standard endmills ?

standard 2 flute are terrible tools at extended lengths , try a 55 deg high helix or better yet 3 flute high helix , the three flute will be much more rigid , also if you get a variable flute then chatter will be reduced that much more

[couch]

Originally Posted by dertsap are the tools standard endmills ? standard 2 flute are terrible tools at extended lengths , try a 55 deg high helix or better yet 3 flute high helix , the three flute will be much more rigid , also if you get a variable flute then chatter will be reduced that much more

Yes, they are just using standard endmills, nothing special. Thanks for the info!