[BobWarfield]

Just released:

A Quick Video Course in Feeds and Speeds

available on the CNCCookbook site:

http://www.cnccookbook.com/CCFeedsSpeedsCourse.html

Covers topics like chip thinning and why feeding too slowly can radically reduce tool life.

Cheers,

BW

[Cmailco]

A very nice tutorial for those starting out in the tool trades.

I'd just like to comment a bit on manufacturer based cutting information for a minute, as I use to work a fair bit on the development side. Your video mentions "mastering more variables" and I think that's an important aspect of cutting optimization, but probably on a much larger scale than a generic tool software can handle. At least, anything short of vibration analysis. The new cutting tool world is a mix of old and new. Granted, there are still plenty of general purpose end mills with "x" relief angle, "y" coating and constant helix rate. The hi-performance tool market however, is one of variable-helix differential pitch profiles that place the cutting edges at irregular intervals and as many variations on that theme as one could possibly imagine; different helix angles, different rates of change between them, etc., etc.. These tools tend to cost a bit more upfront but when used properly, cut process costs considerably.

I can't possibly imagine how a software, without all of this model data, can output a recommendation that is more accurate than the folks who designed and test their cutters, coming up with "general starting recommendations" in the process.

And we still haven't gotten to the other variables that have such a profound affect on stable cutting conditions, which actually have very little to do with static cutter flex calculations. If we wanted to accurately calculate THAT, we'd need to know the cutting forces exerted for each manufacturer's tool, the geometry and core thickness of that tool and a whole host of other variables that truly baffle the mind. In the end, we still don't arrive at anything all that useful because the system; comprised of the tool, gage length, tool holder, spindle and machine tool's natural frequency, haven't even been considered.

A purely academic discussion and in no way meant to be combative, as I feel a tool like this is probably helpful to some folks, but since we're on the topic.

Regards,
Chuck

[BobWarfield]

Chuck, thank you for your post.

Just to make our discussion concrete, since the end result is far from "purely academic", how about a link or two to the kind of manufacturer's data you favor?

I'm pretty familiar with a lot of it (almost gone blind from looking at so much of it to be honest), but I'll bet you have some sources maybe I haven't seen.

Cheers,

BW

[Cmailco]

As far as tool catalogs and recommendations go, OSG has one of the better systems out there. They've even gone to the Ebook Viewer for faster navigation. Like a number of hi-performance tool companies, they've also moved from providing slotting and the typical .5D radial cut guidelines to also providing HSM operation feeds and speeds as well.

In my mind, all of this is fine and dandy, because it gets you in the cut without much of a problem, provided you're using a standard LOC tool at shorter gage lengths, a good tool holder and of course, a decent CNC machine tool.

Those starting parameters are going to get you cutting without a problem, so long as everything in the setup is ideal. Taking that to the next step, you have to record data and spend some time cutting. The way I did this in the days before vibration analysis software was to start at the median range of the scale (sfm); use the low range of the chip/tooth and take a cut at .100" axial and .5D radial. If the cut runs fine with no hint of chatter, bump the rpm x 500 and keep moving in 500 rpm increments until chatter occurs, then back down and record that sfm. Now move to .150 axial, .200, .250, etc., until chatter is once again, prevalent.
Record the maximum stable cutting condition; axial depth, radial depth, spindle load, tool cutter brand and all pertinent tool data along with the holder type and all gage data. If using tool holders across various machines, record the machine used for the cutting test along with the maximum MRR achieved.

Now the cutting tests take place at various radial engagements. Let's say, .2D (peripheral), .6D (heavier roughing) and 1D (slotting). We then determine maximum depth of cut for each operation while minding the spindle load. Harmonically stable cutting can easily surpass spindle power, so it's important to pay attention to loads here. Once we've found maximum MRR for each of these cutting operations, we record the data as mentioned, and that data is recalled when programming in that particular workpiece material.

The cutting recommendations gave us the starting point, and we refined the process to work with our tooling.

So why did I go through that huge spiel about finding a harmonic sweet-spot? To make the point that the system: tool, tool gage length, holder and machine tool all play a part. Change any one of those variables and it's back to square one of "MRR optimization".

And to be honest, at most standard tool lengths; say, L/D ratios of 3:1, the recommendations are going to have you off and running without as much as a mouse fart. It's when you get into high spindle speeds (15k+) and longer gage lengths that things get a lot more difficult, but that tends to be standard fare in aerospace and many other challenging machining environments when short gage lengths are not always feasible.

Regards,
Chuck

[BobWarfield]

Here’s my problem, Chuck. As cool as vibration analyzing software is, you may as well be arguing for the machinist to purchase a bigger taper machine or a 4th axis instead of a machining calculator. All 3 belong in a different category because they solve different problems.

You can’t figure out how much to adjust your feedrate for chip thinning with vibration analysis software.

You can’t interpolate the spread out and generic values in a tool catalog’s recommendations with vibration analysis software.

You can’t tell when your depth of cut means you should be conventional milling instead of climb milling with vibration analysis (most CNC machinists just put it on climb for all cases and forget about it).

You can’t adjust the feedrate for lead angle or for the effective diameter of a ballnose cutter with vibration analysis software.

You can't tell when to drill a pilot hole or use a parabolic drill.

You can't tell with a smaller endmill when your rules of thumb have failed and the endmill is deflecting like crazy because you should be using it at Y depth of cut or stickout instead of X.

These are just a few of the dozens of things a good calculator will do for you. And they’re things that do have to be done because the tooling catalogs don’t integrate that stuff into the data, whether you’re talking about OSG, Hanita, or whomever else.

The starting parameters actually won’t get you cutting without a problem if you ignore all those problems. Don’t take my word for it. All those same tooling companies publish tech notes on it. That’s what’s built into G-Wizard—those manufacturer’s tech notes.

If you want to look at the real choices for machinists to solve these problems, consider these:

They can leaf around tons of different tables, tech notes, and specialized calculators. Sure I can find a table of chip thinning adjustments or a calculator for it somewhere. Your own site links to Kennametal's machining horsepower calculator. It’s a bunch of blanks. You have to go look up a ton of information to use it. That’s a painful nuisance to do manually when it could be integrated with a lot fewer input parameters. Yet I know machinists who were using a stack of catalogs, web pages, and a desk calculator. Boy were they ever happy to switch to a real machinist’s calculator.

Machinists can build a custom Excel spreadsheet that tries to bring it all together. This is by far the most common approach among my machinist customers. But that’s a pain to put together, the UI isn’t as handy, and it still doesn’t cover all of the cases G-Wizard does.

They can just trust their CAM software does it. Most of it doesn’t, and I have machinists using everything from OneCNC to Mastercam who like G-Wizard’s results better, not to mention the low end software which is even less helpful.

In short, these are all problems machinists have to solve before they can worry about vibration analysis. You ask why use generic data when you can use manufacturer’s data? Great question! The answer is, “Why indeed?” Plug your manufacturer’s data into the calculator. It’s all the same sort of format. I’ve got a recommended SFM by material and a chipload by diameter. Works great and still does all of the adjustments mentioned.

As a matter of fact, I have several manufacturer’s reps who’ve been making all their customers aware of G-Wizard because it helps them show off their products better.

Heck, forget G-Wizard. There are other great calculators out there. Check out Michael Rainey's MEPro, for example. Very nice piece of work. I just can't imagine why every machinist wouldn't want a machinist's calculator of some sort.

Cheers,

BW

[Cmailco]

I don't know why this discussion shifted to vibration analysis software as I only mentioned it once in my last post. I don't expect anyone, unless they're serious about HSM, to purchase VA software. I simply outlined the typical process used –and often still used– before the software came mainstream and did so to make a few points, which seem to have been lost.

That maximum metal removal rates (MRR) cannot be achieved with a generic calculator just as it cannot be realized adhering to the manufacturer's recommendations because neither evaluates all the variables. So which one is more useful?

The tool manufacturer designs, simulates and spends a great deal of laboratory time in the development phase. That information is passed on through their general recommendations. Some provide more information than others but in all reality, there is no one universal 'best' answer because as mentioned –the number of variables doesn't stop at the cutter.

The software on the other hand, assumes a typical cutter geometry, does not differentiate between say, the standard 90º interval 4-flute and the differential pitched 4-flute mill, can not possibly compensate for the difference between the variable helix and standard helix end mill.... lots of variables unaccounted for, standard features on most hi-performance milling tools these days. And so far we're only talking about end-mills, we haven't even begun to discuss various other inserted cutting tools like say, hi-feed cutters. My guess is, you'd trust the manufacturer's recommendations on that? I'd hope so, since they all –brand to brand– require different programming parameters due to insert style, rake, relief, gage length, etc..

The software doesn't seem at all useful for the work that 'I' do, but that's not to say it won't or hasn't worked for others. Just as you cannot say that speed/feed charts from manufacturers haven't worked for others because they've worked fine as starting points for me, and I'm experienced enough to know how to adjust those parameters to the cutting conditions. That's something you can never remove from the process with a piece of software.

20k rpm spindle, 100 hp linear gantry mill. Workpiece is 120"x90"x6" 7075-T6 and let's assume it is secure, tool is a 1" diameter 3-flute coated carbide end mill, L/D = 5, HSK shrink-fit. Give me best RPM and estimated best MRR for slotting, .7D pocketing and .2D pealing operations. Oh, natural frequency of the system is 680 Hz if you want to include that in your parameters. Color me curious.

I just can't imagine why every machinist wouldn't want a machinist's calculator of some sort.

Of course 'I' can't speak for every machinist but for myself, I don't trust the answers. I've been in this field long enough to know that software –even in very robust builds of FEA and CFD– only get you so far. Not to mention, getting GOOD results means, entering as many variables as one can – GIGO. I'm a bit skeptical of any software that doesn't include every possible variable within a system, and in that case, would rather fine tune the process at the machine. I then save the processes and unless one element changes, never have to do more than drag-and-drop in my CAM system. That or hook up a mic and have a go at things.

Regards,
Chuck

[BobWarfield]

Wow Chuck, a 100 HP gantry mill to go with that vibration analysis software too. You must have people to figure your feeds and speeds for you with all the expensive toys hanging around the Reliquary. You're definitely in a different world than 95% of the people I talk to.

But when you say, "I'm a bit skeptical of any software that doesn't include every possible variable within a system, and in that case, would rather fine tune the process at the machine," exactly what variables is it that you think you are missing here?

You are welcome to enter the manufacturer's recommended surface speeds and chiploads. All the variables relevant to the calculations being done are in fact there. And the calculations are not controversial--all the manufacturer's tech notes tell you to make them.

Chuck, if you can do the radial chip thinning and all the rest in your head, more power to you. If you can't, a calculator just saves you the drugery. If you don't consider radial chip thinning, you should, you'll get better results. That's one of about 2 dozen different things being calculated that you should be considering.

By automating that drudgery, it eliminates the need for you to waste time and leaves you with a better starting point on which to optimize. Honestly Chuck, if it claimed to really deliver optimal MRR that rivaled your trial and error or vibration analysis for your giant gantry mill I would have to charge more for it.

But hey, I'll leave you to your 100 HP gantry mill rather than lead the horse to water. I'm sure as you sit back in your Eames recliner and juggle the controls for the mill with the controls for the vibration analysis software, not to mention your pipe and latte, a calculator is more trouble than it's worth to you.

Sincerely,

BW

[Cmailco]

Wow Chuck, a 100 HP gantry mill to go with that vibration analysis software too. You must have people to figure your feeds and speeds for you with all the expensive toys hanging around the Reliquary. You're definitely in a different world than 95% of the people I talk to.

This machine actually belongs to a manufacturer local to me, one that I happen to work with on occasion; a producer of landing gear and large airframe components. Your question was, and I'll paraphrase without the sarcasm because there really is no need to be unprofessional here,

"Why wouldn't every machinist want your software or something like it?"

I'm answering that question as best I can. If using your software, I take the output as a starting point and adjust for best MRR. Conversely, with the tool manufacturer, I use the data as a starting point and adjust for best MRR. In short, I didn't gain anything by using your software.

VA software is just another tool used to that end, which takes a lot of the trial and error I described earlier, out of the process. With a machine tool capable of anywhere from up to 20k rpm or beyond, well there are a lot of options for cutting speed. You wouldn't want to spend all your time testing the latest tooling the old way, if you could do it in a couple of minutes with the software. So, maybe that explains why it's being used more and more these days.

But when you say, "I'm a bit skeptical of any software that doesn't include every possible variable within a system, and in that case, would rather fine tune the process at the machine," exactly what variables is it that you think you are missing here?


You are welcome to enter the manufacturer's recommended surface speeds and chiploads. All the variables relevant to the calculations being done are in fact there. And the calculations are not controversial--all the manufacturer's tech notes tell you to make them.

Unaccounted variables:

rigidity in fixturing
rigidity in workpiece
rigidity in machine tool: traveling column, rotating head 5-axis, trunnion, etc.,
natural frequency of the system: tool, holder, gage length, machine tool
tool holder type: BT, CAT, dual-contact CAT (Big-Plus), HSK

Now looking at GWizard,
I see that tool holders are selectable in the "setup" portion but have no affect on the output, though they are one more variable in machine tool rigidity.
A 100 hp mill cutting 6061-T6 aluminum with an HSK shrinker holding a 1" 3-flute end mill gets the same feedrate as a 35 hp CAT 40 mill performing a .75" axial x .7" radial cut. No consideration for gage length; this tool could be 2.2" out the holder, in a holder with a gage length of 6" or one with less than 3", the software doesn't care which, though it will have an affect on the cutting process.

1173 sfm, .0092 inch/tooth, 123.4 inch/min, 64.8 ci MRR... roughly half of what the 100 hp machine is currently doing, so no where near capacity for that machine.

Dial things down a little: 13k rpm Makino VMC, 1/2" 3-flute end mill, Nikken milling chuck, .5" axial, .375" radial, 1083 sfm, .0041 inch/tooth, 19.2 ci MRR.

This is a standard milling procedure in just about every machine shop. We're currently at almost 4 times the MRR in 7075-T6 and that's pretty common fare these days.

Again, is it useful to me? I'm trying to explain why it's not, not to be abrasive or to denigrate the work you've done –perhaps it might help you develop the software further.

Chuck, if you can do the radial chip thinning and all the rest in your head, more power to you. If you can't, a calculator just saves you the drugery. If you don't consider radial chip thinning, you should, you'll get better results. That's one of about 2 dozen different things being calculated that you should be considering.

By automating that drudgery, it eliminates the need for you to waste time and leaves you with a better starting point on which to optimize. Honestly Chuck, if it claimed to really deliver optimal MRR that rivaled your trial and error or vibration analysis for your giant gantry mill I would have to charge more for it.

No, I do radial chip thinning with my trusty T-89; have a program for it and everything, just fill in the variables and go. At least that's how I use to do it. Now I just develop cutting processes, record/store all the pertinent data and save those processes in the CAM system. I then recall them when needed... no need to test or recalculate anything. My library is rather extensive, though I still test tools now and then to develop new ones. I'd hope that everyone is using their CAM system in this way.

But hey, I'll leave you to your 100 HP gantry mill rather than lead the horse to water. I'm sure as you sit back in your Eames recliner and juggle the controls for the mill with the controls for the vibration analysis software, not to mention your pipe and latte, a calculator is more trouble than it's worth to you.

Never owned an Eames... any good? Lattes are not really my style but then, not many trendy things are. A nice Earl Grey every now and then fits me fine but a good porter or stout is like... ambrosia.

""The whole problem with the world is that fools and fanatics are always so certain of themselves, but wiser men so full of doubts."

~Bertrand Russell (the guy with the pipe)

Regards,
Chuck

[BobWarfield]

Bully Chuck, I like your response!

We do seem to be talking at cross purposes sometimes, but a little more comes across each exchange, and it's been a good dialog.

If using your software, I take the output as a starting point and adjust for best MRR. Conversely, with the tool manufacturer, I use the data as a starting point and adjust for best MRR. In short, I didn't gain anything by using your software.

What is gained are the calculations, such as Radial Chip Thinning, that you say you at least used to do on your T-89, as well as a number of other calculations such as ballnose effective diameter. I’m glad we’re now on the same page that these are useful at least if you don’t have some other way to deal with those calculations.

Unaccounted variables:

rigidity in fixturing
rigidity in workpiece
rigidity in machine tool: traveling column, rotating head 5-axis, trunnion, etc.,
natural frequency of the system: tool, holder, gage length, machine tool
tool holder type: BT, CAT, dual-contact CAT (Big-Plus), HSK

Now looking at GWizard,
I see that tool holders are selectable in the "setup" portion but have no affect on the output, though they are one more variable in machine tool rigidity.

A 100 hp mill cutting 6061-T6 aluminum with an HSK shrinker holding a 1" 3-flute end mill gets the same feedrate as a 35 hp CAT 40 mill performing a .75" axial x .7" radial cut. No consideration for gage length; this tool could be 2.2" out the holder, in a holder with a gage length of 6" or one with less than 3", the software doesn't care which, though it will have an affect on the cutting process.

True story, and as I have said, I would not expect your MRR to be any where near what you can get to by exhaustive testing for the last little bit. However, what if you’re doing a job where it doesn’t make sense to do the exhaustive testing?

Also, if you know for a fact your machine is capable of considerably more, the tuning parameters are there to apply that to your machine profile. As we will see shortly, we're closer to your Makino example than you may think.

But, even if you start with radically tweaked numbers, they still ought to be adjusted for the particular cut you are taking for radial chip thinning and all the rest.

Lastly, it shouldn't surprise you that there is a plan in place to leverage that date on tapers and so fourth. It's a plan I think you would appreciate, but I can't say more just yet. Suffice it to say I collect taper and other info for a reason and they are not placebos. The teaser would be to ask, "What if 1000 machinists could collaborate to make this data really specific and really potent?"

1173 sfm, .0092 inch/tooth, 123.4 inch/min, 64.8 ci MRR... roughly half of what the 100 hp machine is currently doing, so no where near capacity for that machine.

Dial things down a little: 13k rpm Makino VMC, 1/2" 3-flute end mill, Nikken milling chuck, .5" axial, .375" radial, 1083 sfm, .0041 inch/tooth, 19.2 ci MRR.
This is a standard milling procedure in just about every machine shop. We're currently at almost 4 times the MRR in 7075-T6 and that's pretty common fare these days.

Chuck, if I do what you said you would do and enter the manufacturer’s data, you might be surprised at where I wind up.

For the Makino and an OSG endmill, I get an MRR of 45 vs your 60 after optimization, within 33%. That’s all adjusted. Not bad for a couple of clicks. If I had time on the job to optimize further, or if I just created some profiles in the Tool Crib based on experience through hand tuning, I would be dialed right in.

And, I can then change the cut parameters, readjust for radial chip thinning, ballness effective diameter or whatever, and I’m still tracking your better numbers. If I can get that close to a hand optimized profile algorithmically, well hallelujah!

That very well might not be useful to you, but it is to many machinists.

No, I do radial chip thinning with my trusty T-89; have a program for it and everything, just fill in the variables and go. At least that's how I use to do it. Now I just develop cutting processes, record/store all the pertinent data and save those processes in the CAM system. I then recall them when needed... no need to test or recalculate anything. My library is rather extensive, though I still test tools now and then to develop new ones. I'd hope that everyone is using their CAM system in this way.

This one I find fascinating. I wish you would write about it in depth in your blog, because I suspect others would find it fascinating as well.

The part I am hung up on is that it seems to imply some limited number of cut depths and widths, as changing them effects everything (as does changing the material you’re machining, but many shops limit themselves to relatively fewer materials).

But perhaps I am jumping to a conclusion about what you mean. If all you’re doing is keying in the chiploads and sfm’s from your manufacturer’s catalogs, or perhaps as tweaked by your experimentation, that’s fine and well, people certainly do that, and you can do that with the calculator as well.

However, those numbers still need adjustment for the specific cutting conditions (ballnose, radial chip thinning, yada, yada) or else we’re back to only having numbers that are limited to some set up cut depths and cut widths.

That would seem to me to be extremely confining from many perspectives. Hence, I suspect I just don’t get what you’re trying to tell us.

"The whole problem with the world is that fools and fanatics are always so certain of themselves, but wiser men so full of doubts."

~Bertrand Russell (the guy with the pipe)

Regards,
Chuck

I will see your Bertrand Russell (poor chap, he can have a consistent incomplete universe or an inconsistent complete universe, but never both) and raise you George Bernard Shaw:

"The reasonable man adapts himself to the world; the unreasonable one persists in trying to adapt the world to himself. Therefore all progress depends on the unreasonable man."

Cheers,

BW

[neurofen]

interesting vid.