Fastest MRR (6061-T6 or T6511)

[Bob La Londe]

I have a product I make (series of products) where I have to remove most of the face (leaving behind a couple bosses at one end) 0.25 inches net DOC. I've been doing it in two passes on my little high speed machines with a 1/4" 3 flute Alu-Power. One at 95IPM 20%WOC and .24DOC for the first pass and 70%WOC and 0.01DOC at 80IPM for the finish pass. I can actually run 31.5% WOC on the roughing pass, but that's a lot of load on those little 1.5Kw 24K spindle bearings. It removes a decent amount of material in a reasonable elapsed time.

Anyway, as I think about how to adapt some of the jobs (that don't absolutely require high speed to be efficient) to the new 1100 I realize that obviously won't work with it. At first I thought about just bumping that up to a 1/2" Alu-power on the 1100 in order to get the surface speed up, but I am wondering if there might be a more efficient way. Its a more rigid machine with much larger spindle bearings.

Also do a lot of work where I just surface the whole face of a piece of 6061 at .01DOC before cutting the product. For that I am thinking the SuperFly might be the most efficient tool, but I am open to suggestions there as well.

The other thread about the NYC CNC videos and Lakeshore Mills touches on this, but I thought a more specific thread might be useful. Especially since in this case I am talking specifically about 6061, and in that thread they are atleast initially talking about 4140 (which I also work with).

Similar Threads:

• Fastest I can run 303 Stainless?
• Problem- Fractures in AL 6061-T6511
• Need Help!- 6061-T6511 Chip Control
• 2014 (T6511) aluminum strength for automotive application (w/ pics)
• fastest ipm to expect

[Master_Arvist]

Check out the shear hog. It does really well in high mrr in aluminum for the spindle horsepower the 1100 has.

https://www.tormach.com/store/index.php?app=ecom&ns=catshow&ref=TTS_SHEAR_HOG

[jwatte]

I like the SuperFly.
For the slower spindle on the Tormach, thicker endmills might compensate, and they, in turn, may let you cut deeper with the same deflection.
Just beware to not overload the spindle horsepower!
I've found that carbide tooling on the 1100 isn't worth it, because you can't really get to the spindle speeds where that really matters. I mostly use <3/8" tooling though.

[AUSTINMACHINING]

I have a product I make (series of products) where I have to remove most of the face (leaving behind a couple bosses at one end) 0.25 inches net DOC. I've been doing it in two passes on my little high speed machines with a 1/4" 3 flute Alu-Power. One at 95IPM 20%WOC and .24DOC for the first pass and 70%WOC and 0.01DOC at 80IPM for the finish pass. I can actually run 31.5% WOC on the roughing pass, but that's a lot of load on those little 1.5Kw 24K spindle bearings. It removes a decent amount of material in a reasonable elapsed time.

Anyway, as I think about how to adapt some of the jobs (that don't absolutely require high speed to be efficient) to the new 1100 I realize that obviously won't work with it. At first I thought about just bumping that up to a 1/2" Alu-power on the 1100 in order to get the surface speed up, but I am wondering if there might be a more efficient way. Its a more rigid machine with much larger spindle bearings.

Also do a lot of work where I just surface the whole face of a piece of 6061 at .01DOC before cutting the product. For that I am thinking the SuperFly might be the most efficient tool, but I am open to suggestions there as well.

The other thread about the NYC CNC videos and Lakeshore Mills touches on this, but I thought a more specific thread might be useful. Especially since in this case I am talking specifically about 6061, and in that thread they are atleast initially talking about 4140 (which I also work with).

1/2" Maritool ZRN coated 3 flute serrated rougher is the best I've used >4 cubes/min. I use a shearhog for facing cuts, but its extremely loud when pushing it.

[SCzEngrgGroup]

Bob,

From all I've seen the Shear Hog seems to provide about the highest MRR, but you might also consider using a face mill. I have a 4" 5-insert 45-degree face mill that I can run at ~35 IPM at 0.05"DOC in 6061, which is ~7 cu. in./min. It leaves practically a mirror finish using polished inserts.

Regards,
Ray L.

[Bob La Londe]

Bob,

From all I've seen the Shear Hog seems to provide about the highest MRR, but you might also consider using a face mill. I have a 4" 5-insert 45-degree face mill that I can run at ~35 IPM at 0.05"DOC in 6061, which is ~7 cu. in./min. It leaves practically a mirror finish using polished inserts.

Regards,
Ray L.

A compact face mill might work, but remember I am taking off a 1/4 inch of material. Its going to take multiple passes because the Tormach isn't powerful enough or rigid enough to push on full depth. My Hurco Knee mill will push pretty hard, but even it is not really rigid enough to push the 3in face mill I have for it very deep.

One of my goals with the Tormach 1100 is to setup a series of "pallets" using tooling plate so I can load multiple small parts and cut a batch at a time. Instead of just one at a time. Parts like this in the picture attached. You can see why I am removing a 1/4" of material, and why I have to have a finish pass just looking at it. Put 8 pieces on the mill and press start. Then pull four complete units off the machine ready for secondary operations.

[SCzEngrgGroup]

Bob,

The number of passes is irrelevent - look only at MRR. Whatever tool gives the highest MRR will get the job done in the shortest time, even if it takes twice as many passes.

You should also take into account tool life. A Shear Hog may get the job done faster, but with a single cutting edge, it will likely wear out faster. A face mill has up to 5 or 6 inserts, and each has 4 or 5 cutting edges, so the inserts will last a lot longer, which may well make it MUCH cheaper to operate in the long run.

Regards,
Ray L.

[Bob La Londe]

Bob,

The number of passes is irrelevent - look only at MRR. Whatever tool gives the highest MRR will get the job done in the shortest time, even if it takes twice as many passes.

You should also take into account tool life. A Shear Hog may get the job done faster, but with a single cutting edge, it will likely wear out faster. A face mill has up to 5 or 6 inserts, and each has 4 or 5 cutting edges, so the inserts will last a lot longer, which may well make it MUCH cheaper to operate in the long run.

Regards,
Ray L.

Given that the Tormachs only accelerate at 15iss (unless its ben changed since I asked) the number of passes can be relevant. Most FS tools don't take that into account.

[syscore]

Given that the Tormachs only accelerate at 15iss (unless its ben changed since I asked) the number of passes can be relevant. Most FS tools don't take that into account.

I don’t think that figure is correct. That would take 7 seconds to get up to it’s blazing 110ips rapid speed. I believe that it accelerates to 110 ips almost instantly (well, fast enough that acceleration is negligible with regards to passes). Rapid speed however isn’t negligible.

[TurboStep]

I don’t think that figure is correct. That would take 7 seconds to get up to it’s blazing 110ips rapid speed. I believe that it accelerates to 110 ips almost instantly (well, fast enough that acceleration is negligible with regards to passes). Rapid speed however isn’t negligible.

I'm not sure why Bob is so occupied with the acceleration - I also find it very fast to reach rapid speeds. However, 100ips really would be blazing
Step

[syscore]

I'm not sure why Bob is so occupied with the acceleration - I also find it very fast to reach rapid speeds. However, 100ips really would be blazing
Step

Lol. I just got it. I missed the "per second". Now we are worried about a tenth of a second to accelerate.

[Bob La Londe]

That's 15 inches per second per second (iss). That number is quoted directly from a response from Tormach tech support. Its not in question. Its not a guess. Its not a wrong answer. Its very definitely not irrelevant. Its the constant rate at which the machine can accelerate. It is the factor that determines how far the machine must travel before it reaches its programmed speed.

If you are just doing plane old long move 2 and 2.5D machining operations (even if you are fooling yourself into thinking its 3D because you are working with a 3D model) and your jobs are relatively short, you ( I mean you personally and/or collectively, not editorially ) may not realize much difference, but I do jobs running into the millions of lines of code with hundreds of thousands of very short 3D moves that often take hours to machine. 25iss vs 15iss can mean the difference of hours in a single job. Constant velocity mode can help, but unless you have it set to make squares to look like circles, not as much as you might think. Programming efficiency also make a lot of difference.

I am looking for the least number of total passes at the best possible material removal per pass. I realize that the part of the job referenced in the premise for the initial post is a very small percentage of the total job, but it may a large percentage of the part of the job I run on the Tormach. If it takes 5 minutes or 10 minutes is no big deal if you are only doing it once. Its huge if you are going to do it on 8 parts in a single setup, and run that setup several times in a day.

Acceleration is the second reason I took so long to buy a Tormach. The first was when a bunch of you guys climbed up some poor guy's @ss because he was doing tons of short 3d moves and his Tormach couldn't handle it. I only bought one now as an intermediate machine to be able to do some partially brain dead repetitive jobs semi unattended. The little Speedmasters will still get the bulk of the complex 3D work until I can afford something with a bigger envelope and a higher acceleration rate or I make the time to just build it. I may split jobs between doing roughing and "secondary" on the Tormach, and only the complex 3D part of the jobs on the Speedmasters. To be fair I don't think the Speedmasters are as good in many ways, but they are faster in every other way. Speed, feed, acceleration. All faster. And yes it makes a huge difference in the money shot work.

I'll let the ips mistake go. We all know you meant ipm. So how far do you really think your Tormach has to travel before it reaches 110IPM?

Here is a rather good article about the significance of acceleration (and I don't even like Bub Warfield)

https://www.cnccookbook.com/estimati...ditor-feature/

Interestingly he picks a great example where I see it every day. Spiral interpolation "drilling." The little high speed machines I have do not plunge drill well, so I have to use spiral milling on them.

[Steve Seebold]

If you’re looking for maximum material removal rate, then a Tormach is definitely not for you.

I have owned a FADAL, a Haas and for the last 6 1/2 years a Tormach PCNC 1100. And I’m here to tell ya, if maximum material removal is your goal, cross the Tormach off your list.

[syscore]

"So how far do you really think your Tormach has to travel before it reaches 110IPM?"

t = v/a
d = 1/2*a*t^2

v = 110/60 = 1.8 ips
a = 15 ipss

t = 1.8 / 15 = 0.12 s
d = 1/2 * 15 * (0.12)^2 = 0.112 inches

If all your moves were that small and all you were doing was accelerating and decelerating, then doubling the torque of the steppers (and the acceleration) would save 50% time. But such a machine would also have twice the speed of a Tormach. The reality is that hardly any jobs are 100% or even 50% or even 25% acceleration/deceleration. And doubling the torque without doubling the speed will gain only 10%. Complaining about the acceleration of a Tormach is like complaining about the acceleration of a moped. Not only can't the moped accelerate very fast, it also can't go very fast. Go figure. Warfield made a straw man argument. And here it is...

"You can begin to see that a machine that has very high rapids, say 1200 IPM, but not enough acceleration, will hardly ever be able to take advantage of those rapids."

Who makes such a machine? It doesn't even exist. Just like this one...

"A machine with very slow rapids, say 110 IPM, but a very high acceleration."

Btw, you do realize that the very best average speed that you can get out of a 110 IPM machine is 110 IPM, assuming the steppers (servos) can accelerate it to 110 IPM instantly.

[Bob La Londe]

You can make all those arguements, but a .112 inch is a very long way when doing complex 3D work. I set the clearance plane on certain types of operations at about .05 inch just to reduce the amount of time the tool spends out of the cut. It makes a very measurable difference in job time for certain types of 3D finish passes. I'd set it to even less, but its pretty scary to see a tool rapid across a part at a nearly invisible clearance height.

I'll have to ask Ahren what his 1200 IPM routers accelerate at. I bet they accelerate pretty fast, but somebody might well set one at low Tormach acceleration for a variety of reasons. I bet "that" machine does exist. I know on my little router I found when I was tuning it there was a real world trade off in acceleration and top rapid speed. I had it doing reliable rapids at 600IPM, but I had the acceleration set low. I think I started at 12iss. When I raised the acceleration it faulted over a certain speed. 450 IPM was the marginal rate if I recall. Its been years since I last had to tune or adjust it. I currently have it setup and running reliably at 300IPM and 30iss. Its a fairly small router and I rarely cut over about 180 IPM with it so 300/30 is ok for it. Real world experience. First hand.

I'm not guessing. I see the real world results in practical experience. I don't care. I bought a Tormach for what it can do. Not for what it can't do. I just pointed out a very real very provable reason for why and how I wanted to optimize the tool paths for an operation. More passes is less efficient. If one tool takes 20 passes at full depth and another takes 2 passes at 1/20th of depth (40 passes) its a factor in net time to perform the operation. Acceleration may be a factor. Of course the feed rate and actual material removed per pass are is a factors, but the point in the post that brought this up is a Tormach can't really push a face mill as hard as a face mill can be pushed. The fellow who suggested the face mill may well have mentioned it for just that reason. I suspect there is some history there.

"WELL IF YOU WANT HIGH MATERIAL REMOVAL YOU HAVE TO BUY SOMETHING BIGGER BADDER AND MORE EXPENSIVE!!!!" ROFL. Yeah I know, but that's not what I was asking. I want to know what best removal rates are I can get with Tormach.

My little Speedmasters don't rapid much faster, at 150 IPM (and published spec is now lower), but they are all set to accelerate at 25iss. Relatively they are a low rapid and higher accelerating machine.

Instead of being defensive about Tormach or attacking Tormach as some folks seem to falsely think I am doing. I'm just trying to optimally use my Tormach. If you are blind to its limitations or think anybody who mentions them is the mortal enemy you can't do that.

I know somebody wants to say, "Well you shouldn't own a Tormach and you should just go away and never talk about Tormach again unless you want to only belch rainbows about it." That's just misguided. There is much more to be gained by honest discourse on its assets and its liabilities.

P.S. I'm not going away, and I am going to get the most out of my Tormach.

[syscore]

"Instead of being defensive about Tormach or attacking Tormach as some folks seem to falsely think I am doing."

I wasn't being defensive nor did I think you were attacking Tormach. I thought the discussion turned silly. First we are talking about a simple facing op and MRR, and before you know it, we are talking about acceleration, complex 3D parts and a million lines of code. And as far as I can tell, everyone was trying to help. Even the guy that said buy a HAAS, or at least something more substantial than a Tormach. How do you get from asking about the max MRR for a facing op, to acceleration? Oh, I remember. Someone mentioned using a facing mill and getting an astounding 7 MRR, but you quickly pointed out that would not do because it would require passes and Tormachs can only accelerate at 15 ipss. And then I guess we said "So?"

[Bob La Londe]

Well, until next time then. LOL

[mountaindew]

Bob,

From all I've seen the Shear Hog seems to provide about the highest MRR, but you might also consider using a face mill. I have a 4" 5-insert 45-degree face mill that I can run at ~35 IPM at 0.05"DOC in 6061, which is ~7 cu. in./min. It leaves practically a mirror finish using polished inserts.

Regards,
Ray L.

I noticed they have a 2 insert hog now

Tormach web site

TTS Shear-Hog - 2". Insert mill especially designed for aluminum roughing - achieve up to 6 CIM per HP
Cutting Diameter: 2"
Insert: ADEH-43x
No. of Inserts: 2
Max. Cutting Depth: 2"
TTS Body with ATC Geometry

[TurboStep]

I noticed they have a 2 insert hog now

Tormach web site

TTS Shear-Hog - 2". Insert mill especially designed for aluminum roughing - achieve up to 6 CIM per HP
Cutting Diameter: 2"
Insert: ADEH-43x
No. of Inserts: 2
Max. Cutting Depth: 2"
TTS Body with ATC Geometry

MD
You forgot to mention one very important "attribute"

$395.00 !!!

Step

[syscore]

MD
You forgot to mention one very important "attribute"

$395.00 !!!

Step

That is kind of crazy when you can buy 1/2" roughers with much greater depth of cut for less than $20. About the price of just one insert on a shear hog.