Benchmark - How fast can you rough aluminum with your favorite cutter?

I'm interested in ExKenna's ripper mills. We like Iscar E90AL style insert mills and have several styles and sizes, I'm uncertain if I can improve my processes by making an investement in more tools. But if I think I can, I'll try.

Currently when roughing 6061-T6, we can get 7.5 cubic inches per minute of metal removal per spindle horsepower. With a 3" diameter cutter we can feed it at 100 IPM with .250 DOC with a full width cut. That calculates to 75 CI/Min. This is on a Cincinnati 10VC-1250 VMC rated at 10HP so that means 7.5 CI/Min/HP. A 2" cutter maxes at 150 IPM at .250 DOC full width, which calculates also to 7.5 CI/Min/HP. I haven't used our only Shear Hog lately, AB tools claims it will do 6 CI/Min/HP I remember it giving at least that much if not more.

What tools do you use, and what results do you get? Do solid carbide endmills produce more or less than this? Manufacturers all claim that their tools will improve productivity, I'd love to see some real world comparisons here.

Yup, in 6061 we use the Iscar E90 style insert and get a little over 80 cubic inches per minute. That was on an 1994 Fanuc controlled 15hp machine. Which comes to about 6 CI/Min/Hp if I had been maxed out. I didn't run it at 100%. I think it's around 70-90% load. This was on a resent part and it was in the cut for a while so I backed off some. I imagine that I could have hit 7.5 CI/Min/Hp if I had pushed her some.

I think I was at 198ipm @.2 deep with the 2 inch facemill.

Cool thread, this should be fun to read later.

I dont know the cubic inches/min
but cutting a profile on a plate that varied from 10% woc to 70% woc, a 60% doc with a 20 mm conventional high speed steel slightly coated ripper endmill I got the machine to 4 meters a min at 6500rpm and about 6-7hp max
I would have gone faster but was already getting smoke from the cutting action and a very weird 'back me off now' noise
Give me a TiAN? coated carbide ripper and I sure I could have pushed it to at least 5.5meters/min feed

As for shell mill, I dont know the exact make, but its 2.5" dia, run at 4500rpm, 6 mm doc at 100% woc... can push that to about 1.5 meters/min consuming about 10 hp which equals... HAILSTORM!

Boris

We haven't had to cut a lot of aluminum in the past but are starting to do more. The larger insert cutters (2.000-2.500) with serrated insert seats should be able to remove material the fastest as they're designed for very high SFMs.

...and a very weird 'back me off now' noise

Click to expand...

I've heard that before. It usually doesn't have to ask me twice.

Mattedroom said:

Yup, in 6061 we use the Iscar E90 style insert and get a little over 80 cubic inches per minute. That was on an 1994 Fanuc controlled 15hp machine. Which comes to about 6 CI/Min/Hp if I had been maxed out. I didn't run it at 100%. I think it's around 70-90% load. This was on a resent part and it was in the cut for a while so I backed off some. I imagine that I could have hit 7.5 CI/Min/Hp if I had pushed her some.

I think I was at 198ipm @.2 deep with the 2 inch facemill.

Cool thread, this should be fun to read later.

Click to expand...

That adds up to 79.2 CIM, close to your remembered 80. Divided by 15 hp gives 5.28 CIM/Hp. Is that an E90 or an E90AL tool? What insert geometry? And what brand of machine? I read here that Haas Hp figures are inflated, does that apply to other machines as well? I can see a problem comparing Hp ratings to this.

Boris said:

I dont know the cubic inches/min
but cutting a profile on a plate that varied from 10% woc to 70% woc, a 60% doc with a 20 mm conventional high speed steel slightly coated ripper endmill I got the machine to 4 meters a min at 6500rpm and about 6-7hp max
I would have gone faster but was already getting smoke from the cutting action and a very weird 'back me off now' noise
Give me a TiAN? coated carbide ripper and I sure I could have pushed it to at least 5.5meters/min feed

As for shell mill, I dont know the exact make, but its 2.5" dia, run at 4500rpm, 6 mm doc at 100% woc... can push that to about 1.5 meters/min consuming about 10 hp which equals... HAILSTORM!

Boris

Click to expand...

If I'm doing the math correctly, that converts to .236 DOC and 59IPM - sound right? If so, that adds up to 34.8 CIM or 3.48 CIM/Hp at 10 hp. What machine was that Boris?

While you are probably wanting milling rates, we don't do a whole hell of a lot of it. We do turn a hella lot of aluminum though. My MRR figures on the roughing lathes vary between 16 and 45 cubic inches/minute/hp depending on the operation. (This is on the 15 hp Mazak machines, 16 for turning, 45 for face plunging.) That's at way over 100% spindle load, but the duration of the cut is short - I don't know how much over, the meter pegs out......

Most people already have a favorite and I'm not gonna knock any of them.
Iscar E90AL, Mits BXD, Kennametal Mill One, and a few others. None of them suck, all work as intended. I have the Ripper Mill which is a BXD derivative.
Most manufacturers consider these application specific exotics and charge accordingly. Whereas most quality facemills are in the $100-$120 per inch range these type tools typically command $150 and more per inch of diameter.
The inserts are usually ground and polished so expect to pay $20 and up per tip.
I get $12.50 each for mine and that's a big selling point.
But most of the bodies are coolant thru and metal removal rates are incredible.
I've seen .020 IPT feed rates no problem.

Not to be forgotten is the old APKT/ADKT cutters. With the ground/polished inserts these can be real money makers and shouldn't be scoffed at.

How about a face mill that uses the 100 degree edge of a super sharp CNMG lathe insert that will make you a happy camper for strictly facing.

Hi Curtis - I was hoping you'd chime in. Do you have any parameters from your customers you can post? DOC, IPM, WOC, HP? I'd really like to know how I'm doing compared to others and whether I can pick up by using your tools or any others.

I too would like someone to chime in..

Im running that new 1" ripper mill at the molmet. .19 DOC 10,000 RPMs and at 120ipm it sounds like its going to blow up. I am profiling some parts, so it goes from 10% width to slotting. 100ipm sounds great, but i was expecting more?? Maybe im a bit off base

I also have the same ripper cutter in a 2.5" face mill 8000rpm's 90ipm and .150 doc full width sounds like a dream and that's about 75% load on the Mori.

Curtis, when you get a chance call or PM me. Need to talk to you about the 1'' tool holder before others try and use one...

Mud said:

If I'm doing the math correctly, that converts to .236 DOC and 59IPM - sound right? If so, that adds up to 34.8 CIM or 3.48 CIM/Hp at 10 hp. What machine was that Boris?

Click to expand...

Thats on the new VMCs we have with a 12hp motor on them, in a loverly rigid setup...(unlike that tube thing that I could only push to 250"/min because it was mounted between a 4th axis and a tailstock)
The problem with the part is that its about 4" long so you dont get time to get a good reading(10hp or about 80% is all you see).... but its never given me the weird "back me off now" noise when I was turning the speed up

Boris

Seekins-I can't get any real material removal from those 1" two insert tools either.

However, the two inch variety with a SHORT arbor are a different story. Parameters are very easy...your real unknown is the feed, which is based on power...I calculate offline:

RPM: I feel comfy with 10k rpm with an unbalanced, short, 2" wide assembly
Axial DOC: up to insert depth...0.4-0.5" is safe
Radial DOC: 30-40% of cutter width...depending on cut geometry
Feed: based on available power...I plan on 1 hp per 4 cubic inches of aluminum. (caveat: I base that on spindle power available for the rated shortest duration if I'm going to get through it quick, which is usually the case)

I can get about 100 cubic inches/minute from my Mazak 510C (25 hp for 5 min, 10 hp continuous) and about 140-ish from my Mazak Variaxis 630.





Having said that, here's an example:
Axial DOC: 0.4" (based on part)
Radial DOC: 0.8" (40% stepover for no inside corners)

Available power: 25 hp for five minutes
Available material removal: 100 cubic inches/minute (25hp * 4 cubic inches/minute per hp)
Feed: 312.5 inches/minute (100 cubic inches/minute)/(.4" axial DOC * .8 radial DOC)

...and that will be within 5% of 100% load on the spindle. If I don't want to push the machine so hard, simply reduce your available power. Personally, I like to see 85-90% max spindle load.



I hope Joe788 posts up some of his numbers...if I remember correctly, he's doing about double what I am. I know he has 18k rpm available...I often wonder if that reduces his power requirements.

Hey there Mud,
The metal removal rate for the Ripper is very dependent on machine rigidity and fixturing.
I've seen a VF-2 at 7500 rpm in full slot at .187 deep and 250 IPM. 65% spindle load, sounded good and insert life was excellent.

It seems to like .015 per tooth as long as the parts aren't thin-wall stuff.
SFM is only limited by your machine, run whatever RPM you are comfortable with.

Glen: I'll call you this afternoon. At 10K and 120 you are at .006 IPT so the cutter probably wants to be loaded up more. 100 sounds good but 120 causes a harmonic spike so once we get over this spike and into the trough on the other side it should sound fine. I can't see your set-up but if rigidity or fixturing is not a problem we need to up the chip load. So I would try 7500 RPM at 150 IPM, this is .010 feed per tooth.

At 7500 and .190 DOC in a full slot at 150 IPM this will take out 28.5 cubes per minute. You were at 22 before so it's a 25% improvement and the cutter should sound much better.

Should rename this thread...

"Cubes per Horse" is not a measurement of how fast or how much since the math is flawed. Be careful not to confuse this with cutting forces or capabilities. Just because one guy is cutting at 4 ci/hp and someone else is cutting at 7 ci/hp doesn’t mean the second guy is doing any better or that he's got a better cutter. It really only means he's got different cutting parameters.

AB Tool's calcs (and many other tool builders nowadays) leaves out a bunch of data. It's overly simplified. "Cubes per Horse" is a sales gimmick. The math also only assumes you are always operating at WOT, but even that is not a constant. We all know that different motors have different drops from its rating. All AB did was ensure that they can define parameters for "6 ci/m per HP" across different machines... and they did. Most people can't or don’t attain 6ci/m per HP because they are not cutting within these parameters. Are these people doing terrible??? No, not at all. But look at Curt’s posts and notice he doesn’t mention cubes per horse… smart man. Cutting speeds also have an effect on HP consumption which is not calculated in this math. Plus, when you start getting above 5000 to 6000 feet, many geometries can start to consume more power again. Cutting speeds are also affected by cutting diameter which again is not part of this math. HP consumption is also greatly dependant on cutting diameter, again, not part of this math.

Most of you probably already realize this but I only bring it up for the ones who are wondering whether or not they’re doing the “right” thing or smart thing. You can attain 6 cubes per horse with a high speed endmill. But just because one guy can get 10 cubes on one machine doesn’t mean I can get 10 cubes on a different machine… but I may still be “faster” than him because my MRR is much higher. The reality is that the cubes per horse may be much higher for many people in their usage but the math doesn't use enough variables.

The metal removal rate for the Ripper is very dependent on machine rigidity and fixturing.

Click to expand...

And this is true for all cutters because it affects the capability and power consumptions as well. Cubes per horse can be used for "ballparks" I suppose as long as you operate within a perfect world. My world isn't perfect, I don't use it...

Ok, after reading and watching this thread, I've noticed everyone seems to be familiar with "the ripper". Anyone care to clue me in on what this is? And I hope his name isn't "Jack".

Setup rigidity is much more important than seeing how fast you can remove material. Im not unhappy with the Ripper in any way and more than likely it is designed for much larger parts where pocketing or lots of material removal is needed. I am doing some facing down in areas, but mostly profiling out my part because of the 2.7" depth

I am holding onto a block of 6061, 1/4" into 2 Kurt 3600's. Its not going anywhere, but much more than 100ipm and i cant hear anything but the inserts slapping aluminum.

I'm with Dave on this, what's a ripper?
Inserted or solid cutter? Faceing or profiling? What Size? or DOC capability.

I do machine some AL, but hardly ever big enough as to even spend the time required to chuck up a 1" + tool, set it up and program it, specially when a 1/2" need to follow after it for corner cleanup. It is simply to state that I have no experience with them at all.
What I do know is I usually rough with a 1/2" 3 fl serrated rougher. In order to make my programs modal to accomodate the MiniMill, I typically use 4000 RPM/ 35 IPM feed. That is @ .75" DOC ( 1.5X Dia) slotting.
If only profiling witn no more than 50% ongagement, I push it up to 45-50IPM, same or slightly more DOC.

Dunno how that figures as I have never took the time to calculate the removal rate. It is also not a scientific feed/speed useage, rather that this combo sounds acceptable on the Mini and downright soothing on the VF4.

When I used my Iscar facemill on aluminum a while back I didn't even think about cubic inches per hp. I was after MMR and trying to keep my SFPM within spec. I only have 6k rpm on most of my machines and I find it to be a limiting experience with aluminum. With that being said I don't believe I needed more RPM with the facemill I was using. On Monday I'll look up my specifics and post back.

I find this post to be interesting because I have never heard of Hp per cubic inch but I understand the concept. But I completely understand Psychomill's feeling on the subject. So many different factors affect how much you can cut and MMR is king. But never the less, still interesting conversation.

If not for these type of discussions in this forum I would have never pushed my mill that hard. The fastest our mill area leader ever pushed a face mill might be 30 inches per minute and that's who I learned from. After reading here so many times about this sort of thing it taught me a lot. Things like Variable flutes, Metal Removal Rate, running dry, air blasts and thru spindle coolant. I now lobby my father to purchase machines with these features and I buy better tooling. So far it has fallen on somewhat deaf ears but the tooling has paid off. But time and nagging go long ways with parents.

Come on Lions, win one.....

Seymour,

Since no one has piped up yet, I'm guessing by "ripper" they may be talking about the Shear hog, made by AB tools. Other than that, my only guess would be a carbide hog mill.