[BodaciousBrian]

I fired up Gwizard to calculate my cut depth, and its result is INCREDIBLY different from what I've been doing. Before I break something trying this, I though I would post the results here.
Taig CNC mill, no coolant, just air.
I'm cutting 6061 aluminium with a 0.25 4 flute carbide endmill. I want to use max rpm - 10,000. I set cut depth and width to 0.1" and it came up with 80 IPM. Seriously?

[strohkirchw]

You need to adjust your limits in the program as the defaults are blank. I'm not sure what the chip load is suppose to be on a 4 flute but assuming .002 you'd want to run 2nd pulley and 13IPM. There's no way you're going to get a decent chip load running at 10k rpm.

You could try 3rd pulley 22IPM but you're getting pretty close to .05HP according to Gwizard. So far I've found that right around .05HP seems to be the limit on my machine in terms of rigidity.

[Jeff-Birt]

I fired up Gwizard to calculate my cut depth, and its result is INCREDIBLY different from what I've been doing.

No matter how snazzy a feed rate calculator is the answers it gives you are only as good as the data you put in and even then it is only a SWAG (Scientific Wild Assed Guess.) There are far to may differences in tool geometries, materials, and machines for them to be accurate.

I'm cutting 6061 aluminium with a 0.25 4 flute carbide endmill. I want to use max rpm - 10,000. I set cut depth and width to 0.1" and it came up with 80 IPM. Seriously?

You will want to use a two flute end mill for aluminum. At 10,000 RPM you will have very little torque and you will be generating more heat than chips. I was doing some cutting yesterday with a 3/16" 2-flute carbide end mill, the belt was at the third from the top (4,500 RPM) and I was feeding at about 8 IPM with a 0.080" DOC. If I took a smaller DOC I could have bumped the feed rate up some more.

You really need to use coolant. Just a oil squirt can with some WD-40 in it will do wonders, just squirt a little on every once in a while. I like to mix about a tablespoon of ATF in which gives it some color and increases the viscosity just a bit.

[j_pniewski]

I like to use lighter cuts on aluminum w/ the Taig. Normal roughing with a 1/4" 3 flute (carbide) in 6061-T6 I use 10600 rpm, .04" doc, 30 imp with mist coolant. A 1/8" 3 flute I drop down to .03 doc. Machine sounds very smooth and without strain but I get good metal removal rates. I've actually cut as fast as 40 imp, but I'm not doing production work, so no need to push the envelope with stepper motors and risk losing steps. The mist coolant really helps. Finish passes done at 15 imp.

Joe

[strohkirchw]

Normal roughing with a 1/4" 3 flute (carbide) in 6061-T6 I use 10600 rpm, .04" doc, 30 imp with mist coolant.
Joe

Slotting?

Edit:

Looking that up in gwizard shows .063hp. Trying to do that would easily stall my spindle. I wonder if I don't have something setup correctly. I'm running flood coolant on mine.

[j_pniewski]

Yes, slotting.

Joe

[strohkirchw]

Well that sucks for me
Looks like I'm going to be problem solving tonight

[strohkirchw]

I stand corrected

2 fl 1/4" high helix carbide endmill with .04" DOC and 35IPM with no problems.


2fl 5/16" standard carbide endmill went up to a comfy 28IPM.

[SweetJustice]

I have the same question, but more general -- how do I find MRR charts for milling by horsepower?

At this moment, I want to know: what's an appropriate MRR for my 1/4 HP taig in unknown scrap aluminum? I've spent a lot of time googling for this, I've even gone to the library a couple of times looking for charts, and the only useful thing I've found was a suggestion of .3 in^3/min, somewhere in this forum.

It didn't work. Even at half that (2mm x 2.5mm x 800mm/min), I've still managed to stall my 10mm roughing endmill. Not immediately, but after maybe a meter of cutting.

[strohkirchw]

Gwizard is saying MRR .37 is what I'm doing with a 5/16" endmill for roughing. If I try to go much past this at 10600rpm, I can hear the motor start to strain some.

[BobWarfield]

I fired up Gwizard to calculate my cut depth, and its result is INCREDIBLY different from what I've been doing. Before I break something trying this, I though I would post the results here.
Taig CNC mill, no coolant, just air.
I'm cutting 6061 aluminium with a 0.25 4 flute carbide endmill. I want to use max rpm - 10,000. I set cut depth and width to 0.1" and it came up with 80 IPM. Seriously?

Yep, seriously. Take a look at what some of the other postings are getting. If I had 10K rpm I'd be running that on my IH mill easily.

But, and this is a big BUT, there are limiting factors.

For hobbyists, they will boil down to your machine rigidity, your coolant and chip clearing practices, and your CAM program. Let's consider each.

For machine rigidity, horsepower is your proxy. Horsepower is what will be pushing against the machine to overcome its rigidity. We'd like to think our machine manufacturers would not put a motor that's too big on the machine, so we can start with that. G-Wizard will scale back your cut to stay within the horsepower limit you set for your machine.

But, if you have a very lightweight machine, perhaps the motor is still a bit much. You will get a feel for that. Just scale back the horsepower limit. You can use MRR too, it's almost the same as HP.

BTW, that 10K rpm by 80 IPM cut is 0.4 HP. That seems like a lot for a Sherline. If we stick a 1/4 HP limit on, GW scales back to 7300 rpm and circa 50 IPM. Why scale back rpm? Because it adds tool life, so start there first. Also, scaling back feedrate too much reduces the chipload to the point that the cutter rubs, which reduces tool life.

What about coolant and chip clearing?

This has got to be the #1 reason I hear from hobby machinists for breaking cutters. Especially when slotting or going around corners, they fail to clear chips. If you don't have flood, or a continous mist with enough airflow to move the chips out, you have to stand over it with an air gun in your hand. Be very paranoid about recutting chips. On some materials (stainless!), the chips are work hardened. Imagine tossing handfuls of hardened sharp objects into the path of your cutter.

Some materials are sticky (aluminum and stainless). With nothing to lubricate, the chips want to stick to the cutter to the point they weld on and you have mess with eventually a broken cutter. Fix it by first (you knew I was going to say this) clearing the chips and second, making sure an appropriate liquid is available to lubricate, at least as a mist. If you don't have a mister, spray on some WD-40 every now and then. There are high end endmill coatings that lubricate for dry cutting, but they are material dependent and as a hobbyist, you don't want to pay the premium for them. So lubricate with mist or your can of WD-40.

Lastly, there is the CAM program, and some of it is how you use the program, and some is what the program is capable of.

If you've ever seen those crazy loopy HSM toolpaths, and looked at the feeds and speeds available for them in G-Wizard, you will know they appear to defy the laws of physics. If I take your same cut parameters, but specify I will cut the slot with a trochoidal path and no more than 30% engagement, suddenly I can go 10K rpm and 113 IPM, and that's with the 1/4 HP limit still on!

You've also no doubt experienced chatter in corners, or maybe even broken a cutter in a corner. HSM basically cuts corners without ever going around a corner.

What does this have to do with Hobby CAM? Well, let's say you have to profile the outside edge of a part. You have a choice. You can spiral out or spiral in. Always take the spiral in! If you spiral out, you're down in a slot with the cutter. That's much harder on it.

How you enter the cut matters, and there's lots about that on my mill surface finish page.

Lastly, there is the issue of jerking the tool around. If you look at the g-code, some CAM does a better job generating code that moves the tool very smoothly along the desired path. Others will jerk it around. Even a little micro-jerking matters.

Probably more than you wanted to know!

BW

PS Soigeneris, you need to learn more about feeds and speeds. The differences you talk about are all at the high end, not the bottom. It's very possible for a calculator to completely accurate in those conditions. In fact, its possible for it to be completely accurate exceeding manufacturer's recommended data if you have the right Knowledge Based-machining capabilities to compensate.

[Jeff-Birt]

PS Soigeneris, you need to learn more about feeds and speeds. The differences you talk about are all at the high end, not the bottom. It's very possible for a calculator to completely accurate in those conditions. In fact, its possible for it to be completely accurate exceeding manufacturer's recommended data if you have the right Knowledge Based-machining capabilities to compensate.

Well, I know enough to that the original numbers the OP got were garbage. It has a lot to do with the old adage about GIGO though. There are also so many different tool geometries (and vast differences in the quality of the tool themselves) that even with everything else configured correctly in a feed/speed calculator you will only every be close to an optimal number.

Then you have to consider the effect of how the tool paths themselves are generated as you were eluding to. If you use a CAM program like SurfCAM that can generate toolpaths based on tool engagement angle then the optimal feed/speed rates are drastically different than using toolpaths generated in a conventional manner. The other very large consideration is the effect of cutting feeds/speeds on tool life. You can 'push' a tool to cut much faster than what the manufacturer recommended but what does that do to its longevity. There is some range of settings where you strike a balance between optimal material removal and optimal tool life that is the most economical for operating a given machine. You would be amazed at the amount of chips generated by large companies like Boeing to test tooling and find the best feeds/speeds for their requirements. This data can then be fed back into their system for feed/speed rate calculations.

Most hobbyist folks also do not have flood cooling, or super rigid machines, or really high quality tooling so what works on other machines may not work on theirs.

I wasn't picking on your program in particular Bob, rather I was pointing out the fallacy in taking what ever numbers 'any' feed rate calculator pops out as gospel. When someone is just starting to learn about this stuff it compounds the problem as they just try to plug in what ever numbers the calculator says (not knowing any better). I can't tell you the number of support calls and emails I get about feed/speeds where folks are breaking bits because they are just plugging in numbers that a calculator gave them. (again a general statement not direct at your product in particular)

I'm also not saying that feed/speed rate calculators are not a valuable tool, rather they are a complex tool that you have to know how to configure properly, know how to use properly and even then you have to perform a sanity check on the figures they provide. If you understand that the numbers you get out of it are only as good as the numbers you put into it and treat it as an iterative process where one can keep refining the model (i.e. settings) used to perform the calculations based on experience then the utility of the tool will be improved.

[BobWarfield]

Well, I know enough to that the original numbers the OP got were garbage. It has a lot to do with the old adage about GIGO though. There are also so many different tool geometries (and vast differences in the quality of the tool themselves) that even with everything else configured correctly in a feed/speed calculator you will only every be close to an optimal number.

That's why we provide all of the information to the calculator, like the HP limit. Then the numbers are correct.

BTW, when you speak of "optimal", I won't even address that here. G-Wizard has a whole set of features like the Cut KB to facilitate that, but arriving at "optimal" is an involved process of experimentation. I'll save it for a post on CNCCookbook. Many professionals use G-Wizard and it is helping them get to "optimal".

Then you have to consider the effect of how the tool paths themselves are generated as you were eluding to. If you use a CAM program like SurfCAM that can generate toolpaths based on tool engagement angle then the optimal feed/speed rates are drastically different than using toolpaths generated in a conventional manner.

That's why we have a constant engagement angle calculator built in. It's also why we have specialized calculators for interpolation and ramping. It's why our Cut KB records all this and more to help you build a database of what works and what doesn't that G-Wizard can learn from.

In this way, we deal with the reality that not all toolpaths and situations are the same.

The other very large consideration is the effect of cutting feeds/speeds on tool life. You can 'push' a tool to cut much faster than what the manufacturer recommended but what does that do to its longevity. There is some range of settings where you strike a balance between optimal material removal and optimal tool life that is the most economical for operating a given machine. You would be amazed at the amount of chips generated by large companies like Boeing to test tooling and find the best feeds/speeds for their requirements. This data can then be fed back into their system for feed/speed rate calculations.

There are a number of issues here that you want to be careful of, Jeff. Let's just start by not even trying to exceed mfg's recommended feeds and speeds, but rather to understand those recommendations, what they mean, and where that mfg was coming from. The mission of the core G-Wizard features is to arrive at that understanding and give the best possible feeds and speeds within that envelope.

You don't know, for example, whether the mfg is giving you dead safe recommendations that will not set the MRR world on fire, or whether the recommendations are a little hotter for marketing purposes. I have some numbers from Siemens research that say it is usually the latter (I hope you're not surprised, LOL). So how to deal with this, absent running specific manafacturers recommendations?

The answer is that you crunch through a whole bunch of manufacturers of apples-to-apples cutters to sift out the real picture. You can't make meaningless comparisons where the coatings are different or one is a high or variable helix and the other is not. If you do this for at least a dozen, you have some interesting data. You need to decide where to "cut" the data. G-Wizard aims for just below average to factor out that marketing bias. That's an oversimplification, but I won't bore you with the statistics.

If you prefer, you're welcome to override that with your manufacturer's specific data, and we even make it easy to download that data from our online library for many cutters. This is a really nice way to compare advertised cutter performance before buying.

Next issue is with how the manufacturer's data is presented. It's all set up for 2D paper catalogs in tables. They can only use a few variables--Material and Cutter Diameter. Perhaps a few correction factors for things like slotting or depth of cut.

Of course the real world is a smoothly varying multidimensional space. And the physics are a lot more complex than the simple SFM, chipload, feed, and speed formulas we all learn at birth as machinists. Radial chip thinning, lead angles, and many other factors come into play. G-Wizard is designed to interpolate those variables to solve that issue over paper tables.

You can be well within manufacturer's recommended numbers and still get better feeds and speeds for a specific cut simply because you analyzed more variables than they could present in a 2D table and covered more of the physics.

RE Boeing, I won't be so amazed as I've read their papers. :wave:

The systematic processes they use are what Cut KB lets shops do. Eventually, we will let shops share their data online. 1000 machinists working together online can do what 1000 machinists working inside a company can do.

Most hobbyist folks also do not have flood cooling, or super rigid machines, or really high quality tooling so what works on other machines may not work on theirs.

Yet it does work surprisingly well! To understand the impact of flood cooling, understand what the flood coolant does:

CNCCookbook: Dry Machining

This post is long and getting longer, so I'll leave you with that link. But the #1 issue for most materials is clearing the chips. Keep the chips completely clear and you're most of the way there, no matter how you accomplish it.

The #2 issue is lubrication so the chips don't weld. That's also easy for hobbyists.

A distant #3 is the actual cooling effects. This is only a big deal for certain materials that don't conduct heat well (Titanium!) and for levels of precision we can't achieve.

As for rigidity, understanding the HP of the cut and the equivalent HP your machine's rigidity can "resist" is all you need to know to work around it. Yes, you can't make a 15 HP cut on your Sieg X2 and it is a pity. But at 1/4 HP, or whatever the number is for your machine, rigidity is no longer your limiting issue. Other factors like runout will be.

I wasn't picking on your program in particular Bob, rather I was pointing out the fallacy in taking what ever numbers 'any' feed rate calculator pops out as gospel. When someone is just starting to learn about this stuff it compounds the problem as they just try to plug in what ever numbers the calculator says (not knowing any better). I can't tell you the number of support calls and emails I get about feed/speeds where folks are breaking bits because they are just plugging in numbers that a calculator gave them. (again a general statement not direct at your product in particular)

I'm also not saying that feed/speed rate calculators are not a valuable tool, rather they are a complex tool that you have to know how to configure properly, know how to use properly and even then you have to perform a sanity check on the figures they provide. If you understand that the numbers you get out of it are only as good as the numbers you put into it and treat it as an iterative process where one can keep refining the model (i.e. settings) used to perform the calculations based on experience then the utility of the tool will be improved.

I've had several thousand machinists use G-Wizard. A few of them break cutters. We've diagnosed the issues together (I certainly don't want to ship a product that breaks cutters!) and worked through them. Some of the locals have been involved. There are some great threads with KVOM over on Practical Machinist, for example.

I've had more than a few users tell me G-Wizard helped them stop breaking cutters, get higher MRR, and improve surface finish. I've had a few tell me they wished it was more aggressive out of the box.

I would argue that if you're a beginner who hasn't the luxury of apprenticing under an expert, you absolutely want the best feeds and speeds calculator you can lay hands on. How else are you going to determine what to do?

Send your customers my way if they're breaking cutters. We'll help them out.

Tormach has been very generous in promoting G-Wizard in some of their videos and blog. They do it precisely because it was so challenging helping beginners come to grips with feeds and speeds.

All this and more is explained in my video course on feeds and speeds:

A Quick Video Course in Feeds and Speeds

BTW, there's no magic. Everything G-Wizard does is something you could figure out and do for yourself. I started it out as a big Excel spreadsheet. It just makes it a lot easier to punch the values in and go. I do encourage interested parties to try to go through all the calculations for yourself. You'll learn a lot that way.

I'm also very happy to help folks understand how this all works. Drop me a line if you have a question. It's easier to understand than you'd think, and it makes good sense once you know how it all works.

Just remember: The whole purpose of speeds and feeds calculations, the reason they were invented, was to make machining predictable enough to be more commercially profitable.

Cheers,

BW