Alum Roughing.

[kunfuzed]

Here's how we've been roughing aluminum lately, specifically in cases where long reach is needed.  Open to suggestions for options we may be over looking (Tooling, paths, etc).

 

2024 T851

Haas VF3
Nikken Milling Chuck
3/4" R.06 Garr 143r relieved to 3.5
Mastercam Dynamic Optirest toolpath
.150 Radial step over by .625 step down
8100rpm, 150ipm feed

 

Chatter seems to be the limiting factor, most likely do to tool length, but hanging out on the Technigrip fixture probably doesn't help either.
 

 

<iframe width="560" height="315" src="https://www.youtube.com/embed/lxdCWUdTHjQ" frameborder="0" allowfullscreen></iframe>

 

 

Thanks!

[MrFish]

You could try a different cutter as we find the Garr 143m cutters do take quite a bit of pressure to cut. If you look at the grind you can see that the first clearance grind is quite flat.

[BenK]

Check out Benchmark Carbide. Here is the tool number for their .75 aluminum roughing tool with a 3.375 reach. CBC350-75026NS54-C5

[Gary]

I bet the part is chattering more than the cutter on that. A balanced set screw holder would probably be more rigid. But what you have ain't bad.

I usually go inserted cutter with big step over and .075 depth of cut on something like. About the same feed rate so I don't know what would be faster

[Machineguy]

On that setup

CARBIDE SQUARE TOOTH ROUGHER

 

10000 RPM

150 IPM OR BETTER

.500 DIA

.500 DEEP

.250 STEPOVER

COOLANT ON FLOOD

LEAVE .02/.03 FINISH WALLS

.010 FLOOR

 

They are 3/4 an 1.0 dia roughers

It breaks the chips up without the tool pressure

[kunfuzed]

We've used some 1/2" YG Alupowers before that seem to do pretty good, may try it in a 3/4.  It's interesting though YG seems to have much slower speeds listed for their cutters.

 

Maybe not using the .06 corner radius as well?  Square may have lest tool pressure?

[kunfuzed]

On that setup

CARBIDE SQUARE TOOTH ROUGHER

 

10000 RPM

150 IPM OR BETTER

.500 DIA

.500 DEEP

.250 STEPOVER

COOLANT ON FLOOD

LEAVE .02/.03 FINISH WALLS

.010 FLOOR

 

They are 3/4 an 1.0 dia roughers

It breaks the chips up without the tool pressure

Not a bad idea.  We've never tried any carbide roughers for aluminum.  We used to use a lot of PCT Powdered Metal truncated roughers, but ran much slower.

 

What Manufacturers do you suggest?

[Müřlıń®]

Push it twice as fast and load up the chatter..

[kunfuzed]

Push it twice as fast and load up the chatter..

I was able to get it up to 200ipm in a vise set up, but I guess I was to scared to try it here.  Hot parts on a deadline, but of coarse when aren't they... lol.

 

Also I stalled the machine out due to an "Excessive Tool Imbalance" error at the S8100/F150.  The solution there was dropping the RPM 10%, which of course also loads it.

[JoshC]

Nice choice on the toolpath, Opti rocks! if you have any high feed mills laying around for aluminum you could use a really large step over with that optirough, then turn off the step up option and set your step down to the cutters reccomended Depth of cut (which should be small if its a high feed mill). Just a thought, may still have some tool chatter but a larger dia high feed mill shouldnt chatter too bad. plus by eliminating the stepup setting you wont be burning the end of the solid carbide up as bad.

[kunfuzed]

Nice choice on the toolpath, Opti rocks! if you have any high feed mills laying around for aluminum you could use a really large step over with that optirough, then turn off the step up option and set your step down to the cutters reccomended Depth of cut (which should be small if its a high feed mill). Just a thought, may still have some tool chatter but a larger dia high feed mill shouldnt chatter too bad. plus by eliminating the stepup setting you wont be burning the end of the solid carbide up as bad.

I was just thinking about that!  Do you guys use any down in the .75 to 1.0 range?  I like that size in this case for less corner clean out in finishing.  I do worry that the part would still chatter due to fixtureing, but maybe not!

 

and thanks!

[Pilot Plant Supervisor]

I use a lot of the Seco High feed mills R217.21. 3/4" 3 flute 900 sfpm in steel 75% step over .025" step down .025" chip per tooth. I haven't tried in aluminum yet, but I believe they make an aluminum insert. Our Haas mills can't keep up with the cutter, but you can sure remove the metal in a hurry. I'd love to run them in a high end machine.

[crazy^millman]

I have run an ISCAR 3 Flute 2" diameter Alum-Tec tool at 24000 and 1200 imp with 60% step over and .125 depth of cut. Was pulling close to 90hp and metal removal was 180 cubic inches a minute of 2219 T851. Bead blasted the side of the machine it was running on and threw chips up to 40' away from the machine in all directions.

[taperlength]

Technigrip is a good fixture.  I use a torque wrench to get consistent clamping force on it.

I just looked at Garr's pdf  and for the 143r they write "For CAT 40 machines using tools over 5/8" diameter, speeds and feeds may need to be reduced by as much as 50%"

[kunfuzed]

I can see one advantage with an insert mill, or a feedmill and a shallow depth is you can utilize the alternating climb/convential motion in the dynamic toolpath.

[THEE THAINZ™]

Look into Mitsubishi AJX cutters, they should have a 3 or 4 flute that would work if your not into ISCAR.

[BCW]

Like others have said... .06 rad isnt that big, but going square may help.

 

But with it attached to the rotary like that I think you are not going to get much better than what you have. Seems fine to me.

[?Mark]

I must be going too fast. Already stripped the paint off the trunnion of 5 axis matsuura on the first job...2 weeks, lol 

[THEE THAINZ™]

If it took 2 weeks too slow.............

Destiny also makes a pretty good end mill in there VIPER line.

[AMCNitro]

Helical endmills...

[Matthew Hajicek - Singularity]

 

 

Helical endmills...

 

I got a couple of those for cutting nests into aluminum jaws.  Might get to try them out next week once the machine is in and hooked up.  I also got Helical for Ti and 17-4.

[AMCNitro]

I got a couple of those for cutting nests into aluminum jaws.  Might get to try them out next week once the machine is in and hooked up.  I also got Helical for Ti and 17-4.

Download their app, it works great.  

[JAMMAN]

I use OSG Blizzard mills for roughing aluminum but a smaller diameter... .375. I have held it right beside a Garr and they look practically identical but the OSG doesn't ring like the Garr on what I'm doing. Too bad I can only get 6000 RPM. 80 IPM .05 depth like 50% step rest rough path. I know wimpy but all my machine can handle.

[AMCNitro]

I use OSG Blizzard mills for roughing aluminum but a smaller diameter... .375. I have held it right beside a Garr and they look practically identical but the OSG doesn't ring like the Garr on what I'm doing. Too bad I can only get 6000 RPM. 80 IPM .05 depth like 50% step rest rough path. I know wimpy but all my machine can handle.

You cant go full depth of cut with .125 step over?  IMO(putting on the flame suit) full depth of cut with a smaller step over works better, you're utilizing the hole flute, not just the tip.  Which machine is it?

[kunfuzed]

Hey thanks for the suggestions guys, hope to try some new cutters soon!  But like others have said, I'm probably limited by the fixturing, and the fact that it's a Haas.   Do the the "grown up" machines that start with "M" handle long stickouts without chattering?  Even in a vise, if I go much faster with a tool like that the harmonics pick up.