Looking for endmill suggestions on roughing aluminum

Hello everyone! I'm working on a new production machining project and looking for some advice. Though I've worked with aluminum for years, this is my first large scale project. We are looking at 4,000 hours of machining a year over 4 years. At this point I'm getting heady to start programming and looking for tooling.

Machine and setup:
Horizontal 4 axis 50 taper with 500mm pallet
30 HP 15,000 RPM max (though we usually don't run past 13,000 RPM)
Older Fanuc 15M controller (1993?)
Machine is capable of high feeds but not the best at turning directions very fast or processing ramping code.
Custom made fixturing on 500lb tombstone. Fixturing should be quite rigid with large serrated edge clamps pushing stock into serrated square grippers.
Roughing tools will be in hydrolic tool holders
Has very good flood coolant and through the spindle coolant

Part:
Starting stock size is 25"x16"x2"
7075 or 7050 (haven't confirmed which yet)
Approximately 85% weight reduction so lots of pocketing
All larger pockets are about 1.55" deep with .090 corner radius and .26 inside radius

I'm leaning toward a 3/4" for roughing and will have to use a 1/2" for finishing because of the .26 inside pocket radius. I plan on drilling a plunging location before roughing as I don't want to ramp in with the rougher. Ramping eats a lot of code and the controller doesn't have much memory.

I've looked at OSG, Fraisa, Benchmark, and just recently looked at Data Flute (which I've never worked with). I'm pretty set on using a rougher with a .090 corner radius simply to reduce the material the finisher would have to remove (a smaller radius would force me to leave step in the corners for the finisher to remove which would mean more "Z" steps and more code. I notice that most of the endmill manufacturers are offering "hog" style roughing endmills with chipbreakers. I've never used this style of endmill before in aluminum and looking for some opinions on them. Basically I'm looking for others who work with roughing large amounts of aluminum and what they have found works and what doesn't work. Thanks!

When we do pockets we always pre-drill the holes and I find using These STI Drills you can fly with them, I'm currently feeding at 85.IPM with non coolant thru. They have coolant thru too. And I always use Data Flute aluminum cutting end mills for finishing in 7075 and they work great. As far as roughing goes we usually use Niagara coarse tooth roughers but I'm not sure if you can buy them off the shelf with a corner radius, I'm sure they can do it for you but at a cost im sure.

Aluminum Roughing

We manufacture a 3 flute rougher designed for aluminum. Tool has a zirconium coating which works really well in aluminum. Check it out on our site Carbide Cutting Tools : Carbide End Mills : Carbide Inserts : Thread Mill : Thread Mills : Carbidecuttingtools.com click on end mill catalog. Call for current pricing.

We've had good luck with garr alumastars and they're relatively cheap for the 1/2 inch.

The control, and chip disposal are probably going to be your two biggest issues. I'd get a half inch Hanita, MA Ford, or Destiny serrated carbide rougher and rough each pocket in two depth cuts. Depending on conditions, you might be able to get away with a single pass for the entire DOC.

25"x16"x2"? You makin' scales?

I agree with Joe with sticking to the 1/2" e/m's, a 3/4" roughing will test your drawbar/pullstud pull, and not in a good way either. We were using a Destiny Diamondback rougher (on 6061) in both 3/4" and 1/2", and have since switched to "standard" 1/2"-ers and completely dropped using the 3/4" tools. We too have good HP and rpm, but can handle large programs and it has a fast control, but we still tend to keep the roughing at <500"/min.

As far ar dropping the 3/4" tool, we have gone to using a 2" "Ripper" facemill (Look up "Exkenna" Curtis Payne and he can hook you up) and have great MRR and low HP and axis loads. The roughers do make a nicer, more compact chip which is easier to wash out and carries out less coolant, but at the end of the day, the low load (~55% max for us now runnning at about 100 cuin/min MMR) and easy (less code) toolpath wins out. We really were not trying to increase our MMR when we switched, and may have actually added cycle time, but it didn't matter too much on 30 minute roughing cycle when the total cycle time is about 5 hours...we can get two attended and two unattended loads per day, so squeezing the roughing time in half would make no difference.

Steve

chainfeed said:

We've had good luck with garr alumastars and they're relatively cheap for the 1/2 inch.

Click to expand...

Same here. 2000+ SFM and 200ipm with these all the time.

ewlsey said:

Same here. 2000+ SFM and 200ipm with these all the time.

Click to expand...

These cut sweet even on little 30 taper machines, can't emagine what could be done on a 50 taper monster!!

Check out my website for proof

Benchmark carbide: They are not the cheapest but definetly deliver results. I only have a cat40 15hp 10rpm spindle and using Benchmarks CBC350-75026-C5 I was able to take .750" depth of cut .625 width of cut at 115IPM! I would love to see what this endmill would do in your 50 taper. I was maxing my machine out for a couple minutes at a time but I was removing some serious material durring that time. Try them you wont be disapointed.
The part on my website is the under pulling parts. It's the Billet front cover. The Precision Edge Machine, LLC - Home - Zimmerman, MN

There is nothing wrong with any of the tools mentioned.. Garr, Benchmark, etc. you should have great results with any of those. Might also want to check out the Destiny Viper and it's rougher cousin, the Diamondback.

Here's a vid I shot in a friends job shop running a 1/2" Viper at .012 per tooth:

(Skip ahead to the 2:55 minute mark to see the real fun)
YouTube - ‪Destiny Viper End Mill Video‬‏

I have a job that I run that makes a 2.15" x 6.1 X 17" pocket in 6061 and for all of the roughing I use a Mitsubishi BXD4000R that is a 2 insert 1" mill (looks a lot like a mini Ripper mill). I run around .3" depth of cut with a .95 stepover at around 95 IPM. The chips are really tight, almost like BB's, and I will get about 300 pounds in the machines before we have to stop and shovel them out. I use the Destiny Vipers for all of the inside finishing work, but the chips coming out of them are a little harder to manage.

Robb Jack! Robb Jack! Robb Jack! They have all kinds of standard tool configurations for aluminum and they hall A$$! Short, Medium, Long, XLong. 2 flute, 3 flute, all different corner radii, etc. etc.

RobbJack: Manufacturers of Premium Rotary Cutting Tools - Carbide End Mills, Saws, and Router Bits

Trust me on this one.