What's new
What's new

Recommended SFM for 6061 milling/drilling

couch

Cast Iron
Joined
Jun 10, 2009
Location
CA
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 (sometimes 4 flute :nutter:)
3/4" carbide endmill 2 flute (sometimes 4 flute :nutter:)
1/2" carbide endmill 2 flute (sometimes 4 flute :nutter:)
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 :nutter:) which sounds like shit 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? :eek: 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. :cheers:

-couch
 
Use a chipload of something like 1 to 2% of the cutter diameter for two flutes.

Don't use 4 flute on aluminum.

1" cutter is probably okay at 6500 rpm but if the machine has the power you could go up to 8,000 rpm.

3/4" cutter is okay at 7500 rpm or 10,000 if the machine has enough power.

DOC can be up to 1 x cutter diameter if the radial engagement is only about 20 - 40% of the diameter, for greater engagement reduce the DOC proportionately.

FLOOD coolant all the time on aluminum.

Drilling 0.202" at 4000 rpm, 10 ipm and peck every 0.2 or so.
 
The nice thing with aluminum is that you have a HUGE window of usable speed/feed ranges. 5000SFM + is not unheard of and in some instances around 8000SFM is quite possible. Depending on what style of tool you're using, you can crank all of these way up (even without TSC) given the part set up, HP, tool holder type and feed/accuracy capacity of the machine.

I don't peck very often with drills (.201 can take it) but this will depend on the final depth. The key with pumping up aluminum speeds/feeds is the coolant. Plenty of flood (as HDGP mentioned) and TSC wouldn't hurt either. There are plenty of manufacturers who make .201 thru coolant drills from HSS to solid carbide (Mitsubishi, SGS, George Whalley, Seco, Sandvik, Titex... to name a few).

Chatter could be bad for several reasons... wrong tool type, poor engagement, not enough feed (chip load), poor spindle quality, loose set up, etc, etc.
 
Let's take the 1" 2 flute carbide endmill for example. They are using it in a hard holder (set screw type) and its sticking out 5", spinning at 6500RPM with a feed of 50IPM and a DOC at .050"

Now if I remember correctly, calculating that out the chipload is way too small. Increasing the feed has caused the endmill to break, so they say. Only other way to thicken up the chip would be to slow the rpm... All this talk about increasing the rpm as fast as possible is throwing that out the window though (running slower rpm's). The setup just doesn't seem to be rigid enough which is why I'm looking into insert cutters. From past experience, I have had much better results cutting deep pockets and contours with insert cutters in steel rather than long endmills... On the other hand, this could all just boil down to insufficient amounts of coolant... I've gone out in the shop countless times and mentioned the coolant issue to the "setup" guy... "ah, its fine"...

The more we can dummy proof, the better.

Thanks for all your input!
 
Just to add a point to what psychomill said above, quantity of coolant is required, but also *quality* coolant is required. If they do not watch concentrations of the coolant, an already bad day can get much worse. For most coolants, you are wanting to be in the 7-15% range for aluminum, most likely in the 10-13% range. Now, this does vary depending on coolant mfg, but just saying....as a rule of thumb......
Aluminum needs lots of lubricity in the coolant. It also needs a lot of the "cool".... part of coolant.
 
+1 to Tony on the "quality" of coolant issue.

Along with that... quality of tooling, setup ... what I mentioned before. I run 1" endmills with 5" hangouts all day long anywhere from 7k-15k rpm and feeds from 150ipm to over 400ipm depending on the part and circumstances... and at deeper DOCs than .050. If they say it breaks (and the set up is good), it sounds like a possible coolant issue, chip recutting issue (from pocket buildup) or wrong endmill type (full flute instead of a neck back, HSS instead of carbide, wrong helix angle,... for example).

IMHO.... no matter what you decide or what your approach is... the way it's currently being "done" has miles of improvement that can be made. It's under par for sure...
 








 
Back
Top