Suggestions on "high(er)" speed aluminum milling

I'm hoping to get some ideas from those with more experience with more "rpm" than I have.

This will be deliberately vague but hopefully I can convey enough information for useful suggestions.

A little background-our shop cuts steel in a pretty niche market. We have been and are successful. Our biggest customer has had us doing a specific type of part for them in aluminum recently, kind of a "family" of parts. To the point of us adding a new dedicated machine to process these.

Many similar features but no 2 parts the same ever. It is not aerospace, but often reminds me of such, having really only seen pictures of spar type plane parts. Lots of pockets with realatively thin walls and floors. These have no real critical tolerances, but a fairly large area of material removed. But the defined walls and features preclude really hacking off chunks with larger tooling.

Generally the features of the part define the tools used. Our most common roughing tool is a 3/4" carbide end mill currently. With smaller tools to finish defined radiuses and other features.

We are currently running these on one of our VMC 64X32X32 6000 rpm geared head 50 taper machines. This is our "standard" machine as we have 6 similar ones. We need the travels for the normal work we do.

We have recently acquired a machine to run these parts and it will require a different approach however. We have no concern over the ability to make it work, but being able to jump a few early hurdles would be helpful.

The machine is a no-name Taiwan bridge mill. (WellMax CNC) The machine has 40X32x30 travels so it will take up less floor space. It is a HSK 62(?) spindle with 20k rpm to cut some aluminum. A 40 tool carousel and Mitsubishi 830(?) control.

My real questions relate to tooling and programming for this type of mill. We normally run essentially everything at 6k and feed around 100ipm. The machine we have been using is a box way machine so a lot of high speed direction changes are not its favorite thing to do.

The material is all 6061 sheet, we will never have to cut over 1" deep. We use MasterCam X9 to program. With the 50 taper and 6k spindles, we have not really used any of the dynamic tool path features up to this point. We have been limited to 500k program size and machine limits up to this point.


There is anticipation of using "MQL" ( min quan lube) on theses parts-does that really work for slotting/pocketing in 6061? I have never done it and am skeptical, but that's why I'm asking.

Is there a "point" to switch to single flute tooling as far as rpm and federate? I don't have the spindle ratings with me but I know the range is from 3k to 20k, a lot different than what we are used to. We have purchased a fair number of hydraulic holders to go in the machine. Do we have to worry about pull out with aggressive milling? We currently have been using side locks with flats but again only at 6k in a Cat 50 mill never used HSK yet.

I am anticipating using more dynamic milling, but is it really advantageous at only 5/8-1 inch depths of cut in aluminum? The machine has supposedly 2 gig memory, so that will remove one of our old hurdles- not actually on our floor yet.

Well that turned out to be a lot more story and fewer questions than my intent. If anyone made it this far, I am really hoping for some suggestions on applying our rpm, and making better use of our software for this application.

I would be glad to offer more info to clarify if needed.

Thanks in advance,

Mike

Absolutely use the dynamic tool paths for these types of parts. I cut many parts with aerospace like cut-outs. My favorite routine is to drill as fast and as hard as I can using a 5/8" parabolic drill, then do a dynamic tool path using the drilled hole geometry as "air space". This allows the cutter to plunge into the hole and immediately start taking a consistent chip load.

Depending on how big these cutouts are, I would probably just use a 1/2" carbide end mill. I am usually horse power limited so these give me vary good material removal rates, plus (assuming a greater than .260" corner radius)I usually have a very nice and consistent chip load on my finish pass.

A 1/2" EM buried 1" deep, I usually cut about 120 IPM at 12k rpm. Then I adjust my radial step-over to get the spindle load that I like. My guess is, that will be around 20%-25%.

I use flood coolant, but a properly programmed HSM path can get away with air blast only.

I could run much harder, but I don't like to put too much abuse into my machines.

With the type work you describe, in roughing your limitation will be how much HP that 20K spindle has and if it has much power, how well you can hold onto the part.

Yes, you'll have to think about pull out of the tool, even with hydraulic holders. A lower helix endmill may not cut and throw chips out of pockets as well as a fast helix, but will be less prone to pulling out. A good MQL setup will clear away the pockets, you doubtless have the air compressor service to feed it. Don't run the MQL too rich, and set up a duct to remove airborne mist and floating Al dust.

Have you considered chip wrangling? You'll have a lot of them to remove.

Don't forget to look at corn cob type roughers, IMHO the answer for restricted RPM, they can be fed harder and break up the chips treat.

We have a process established to hold the stock really pretty well. We have had more of an issue with finished parts bowing from material removal. We have been able to deal with it, hopefully the lower cutting pressure with smaller higher rpm tool will alleviate some of that.

Machine has twin screw-type augurs for chips dumping into a conveyor, being a bridge machine instead of a c-frame layout seems like it will help with chip flow too.

The mist control seems like something we have made no effort to address, good point.

Our technique currently is to plunge out the center with a flat bottom inserted tool. 1" dia. 6000 rpm 50 imp plunge. No peck, remember max depth is 1". Then pocket from center out with appropriate size e.mill, being limited to about 100 imp we just use a 70% step over with parallel or whatever tool path works. Then finish as needed per print. The tool, spindle power or workholdng has not been limiting as much as feed rates have been. Does no good to program 300 imp if machine won't corner over 120 i.m.p.

The high helix e.mill does a good job of pulling chips out, especially once there is some open room. Definitely helps chip evacuation with having a start hole.

We are not new to machining, and I am completely open to better approaches, but more real primary interest is making use of the rpm and additional federates we can have with a linear machine.

Use 1/2" aluminum specific end mills for your pocket depths. This keep the 'pull out'' of your end mills down, as well as your tooling costs. 12k rpm 100 or more ipm and 1" depth of cut; 70% step over. Don't waste time changing tools from flat bottom insert drills to your end mill. Just helix down at the feeds/speeds suggested and you will drill the 'hole' in less time than you can change tools. You will not believe the volume of chips you have to dispose of!

Red James said:

Use 1/2" aluminum specific end mills for your pocket depths. This keep the 'pull out'' of your end mills down, as well as your tooling costs. 12k rpm 100 or more ipm and 1" depth of cut; 70% step over. Don't waste time changing tools from flat bottom insert drills to your end mill. Just helix down at the feeds/speeds suggested and you will drill the 'hole' in less time than you can change tools. You will not believe the volume of chips you have to dispose of!

Click to expand...

There you go, Mr. James obviously has more horsepower than my machines... I would have a hard time evacuating the chips if I helixed that deep and my machines would come to a rapid halt if I tried 70% step over at 1" deep. I'm a little bit jealous right now. You would have to remove the chips with a snow shovel

Don't forget that one of your restrictions with aluminum is how fast you can get the swarf out of the machine.

Scruffy887 said:

Don't forget that one of your restrictions with aluminum is how fast you can get the swarf out of the machine.

Click to expand...

It is equally true for steel.

In my original response I forgot to mention that I use TSC and an ER32 collet. The slots in the collet let the coolant blow the chips out of the hole. Good catch!!!