Newbie- intro. w/question

[gene rhodes]

Good morning! I am new to this web-site but have been reading the info from the threads for a while now. I have just started on the programming scene ( approx. 6 months ago) after 10 years of machining experience. I love this side of the wall and can only hope that this is where I continue to stay. We ( our shop) have recently installed the Featurecam program software to help bring us up to speed with our competition and it seems to be working quite successfully. The features that this program offers are quite extensive and extremely useful for what we do. I am currently the only one familiar with this software and that familiarity is rather new in itself.... but I love the challenge!! Nothing like being the "guinea pig".....so to speak!!
Anyway, I do have a question to "initiate" myself into this community. I was wondering if someone could tell me if there is a formula or something that will allow you to determine the proper SFM for a particular insert and what info is needed to obtain this. I know that some (most) insert boxes have this info on the back but I am wondering if there is a way to find this in the field.
Thanks and I'm sure I'll be back with more!!

[RICHARD ZASTROW]

Here's a helpful site I picked up here on the 'Zone.

http://www.kennametal.com/en_US/cust...ols_main.jhtml

Hope it works.

Dick Z

ps can't get it to fire, it's on the Kennametal site-you'll have to poke around from the home page. It's in the customer service aea.

[gene rhodes]

thanks Richard...that seems to help. Although I can't quite get a grasp on this Constant Surface Footage thing!! I understand the meaning and all, and understand the usefullness...but how is it that you can't get the RPM'S to end up at, say, 750 RPM's on a 2.5" part??? Without starting out at 150 RPM's!! The answer is probably right in front of my eyes but that just means this will be the one I remember because it frustrates me soo much!
My example is this.... I have a 2.5" part, hardened chrome rod, that I need to face-off. I know that using CSS will help keep the tool pressure the same thus extending the life of my inserts/tooling...in this case, this is essential due to the usage of a ceramic insert in order to cut through the hardened part of the material. This insert calls for a .003-.005" feed with the SFM's at 250 surface feed/min. I have tried to attain this only to have the RPM skyrocket to over 5000 (luckily it was dry-run first!) !! Is there just no way to achieve this until you reach center??? I have noticed that these particular inserts are breaking as the insert reaches this point....and releases tool pressure.
*note* I have only attempted a run on these parts without using the CSS feature.

[little bubba]

CSS really has little to nothing to do with tool pressure. More or less, its a productivity thing and a surface finish thing. Setting an RPM based on the SFM needed at max diameter will have turning too slow when getting near the center of the part, therefor not moving as much metal as you can, volume wise. Some materials, low carbon steels and even aluminum will have a noticeable difference in surface finish as SFM gets lower, or higher.

On to your problem, with the ceramics, I've never turned with them, only milled, but they are a different critter than any other cutting tool, as you are coming into center, even if you are hitting max RPMs, your SFM is approaching zero, not good for ceramics, you need to keep up the speed to keep up the heat, you slow down, the insert/material cools down, you shatter and insert. I've posted a good article here before, and its bookmarked on my computer at the shop. I think it was "practical applications for ceramics", an article on MMSonline. That article is what helped me immensely when ceramics were biting me in the ass.

And not to sound like a jerk, but spend some time figuring out CSS and make sure you have a good understanding of SFM(surface footage) or you are just going to keep getting bit. I'd try and answer your question a bit better, but I'm not quite sure what you don't understand, either way, you're a leg up for asking.

Good luck.

[gene rhodes]

hmmm...CSS has nothing to do with tool pressure? Then does SFM?? I don't really understand why this is giving me such a hard time! When you say "setting an RPM based on the SFM needed at max diameter..." Is this what determines your SFM? The max diameter? I guess I'm having more of a problem determining where it is that you determine such a feature. I know the formulas for determining SFM but the application is my problem. I'm the kind of person who HAS to know why....and sometimes that's my downfall. Our problem lies in the fact that, when these rods are cut ( in house) they are coming out no better than 3/16 out of square and the face is hardened due to the cutting operation. ( we use a "Savage Saw" to perform this) They are trying to fix the problem without fixing the problem, if you know what I mean! Due to the nature of things (economy), this is understandable. I am determined,until I'm shown a better way, to try to get these ceramics to face-off these rods! Am I wasting my time here?!?!?!?

[little bubba]

Gene, step back two steps, and start at the beginning. What you need to know is really simple basic stuff that from what you have said so far, you will understand.

You just need to start from square one, and then step up. Your trying to understand too many concepts at once, and yes they do all intermingle, but you always have to go back to basics. I can see how you could easily be confused. Example...

You're trying to design an internal combustion race engine from scratch, and your trying to figure out how the "lefty loosey, righty tighty" of the bolt that holds the engine into the car corresponds to the gas flow in the exhaust ports.

Since you seem eager to learn(I admire that) and didn't disappear after the first post, I'll type for a while, and hopefully it will help you out.

First thing, RPMs and feed in Inches Per Minute(or the metric equivalent) don't mean anything, they are fun to talk about and brag about, but as far as cutting metal, they don't mean sh!t.

1st thing, Surface Feet per Minute (SFM). You live and die as a machinist by this. The speed that your cutter is moving through the material. On a mill, your cutter is spinning, so you use the cutter diameter to figure your SFM, on a lathe the cutter is stationary and the MATERIAL changes diameter, and thankfully, most controls calculate that out for you. Easy to understand, the linear speed of the outer diameter. If you have a small tire on your truck, it needs to spin 1000 times to move you a mile, go to a bigger tire and it only needs to spin 700 times to move you a mile.

On a lathe, CSS, say 100 sfm, at a 4" diameter, 100rpms(rounding), so you are facing, get down to 2" diameter the spindle has sped up to 200rpms, gets closer to the center, 1" diameter, 400rpms, 1/2" diameter, 800rpms, 1/4" diameter, 1600rpms, 1/8" diameter 3200 rpms, 1/16" diameter, 6400 rpms, 1/32" diameter, 12800 rpms, 1/64" diameter, 25,600 rpms, 1/128" diameter, 51,200 rpms. Notice as you approach the center line, your RPMs to keep up your surface speed is increasing drastically. As you approach zero you are approaching infinity, I would love a spindle that could go infinity RPMs, but, doesn't exist, and if it did, I wouldn't want to be near it. So.. there are codes to limit your MAX rpm.

Now I'm guessing you understand feed per tooth/rev and depth of cut (DOC), since you haven't expressed a problem with that. So per your box of inserts or other source, you have a SFM, you have a DOC and feed per tooth(mill related, same thing) or rev. That is what (mostly) will determine tool pressure.

So, now lets say you are running X SFM, Y feed, Z DOC, Your tool pressure will be a given amount. Say 100lbs, again, #s pulled out of my ass. Now you double your SFM, your tool pressure will be the same, BUT... it will require more HP. This is the difference between instantaneous force (pressure) vs, work per time (HP). Easy to confuse and not the easiest thing to understand, but the pressure on the tool for a given DOC and FEED will be the same regardless of how fast its moving through the material.

Now I shouldn't have said that since this is where things start to spiral out of control. A higher SFM can change tool pressure several ways, chip flow, a higher heat in the material from a higher SFM can mean a smoother lower force chip flow, also coatings that come into play at higher temps can make things all KY like and let the chips flow easier, lower tool pressure. Of course this all falls apart if you run your insert too hard or too fast and simply destroy it. Geometry plays a strong role in this also.

Now you are messing with ceramics, so the whole HEAT and CHIP FLOW are even more important. A ceramic insert is basically a fricken lego, and ceramics react in the complete opposite way that HSS or carbide do, read the article I suggested, its a PIA to find, if you can't find it I'll post it in the morning when I get to the shop.

I hope some of that made some sense to you.

[g-codeguy]

Good morning Mr. Rhodes. I will attempt to address a couple other questions you had. In the 1st post you asked "if there is a formula or something that will allow you to determine the proper SFM for a particular insert and what info is needed to obtain this."

There is no formula, but there is technical information on the SFM range for a given grade of insert...in a family of material...in the insert company's catalog. Use this section to find out the correct SFM for your insert in the type of material you will be running.

Example: In the back of the Sandvik catalog is a material cross reference list. Not all materials are listed. Pick out one close to what you are running. 8620 is listed as belonging to group 02.1. Go to the turning technical section. Say you are wanting to run a GC4225 insert at F.01. Looking across the page under the 02.1 group you will see that it lists 3 different feedrates. .004 at 1500 SFM, .016 at 1000 SFM and .031 at 710 SFM. Notice the faster the feedrate, the slower the SFM

Take these numbers with a grain of salt. They are in the business of selling inserts. Most tests they run are based on a 15 minute insert life. I run 8620 at 950 SFM F.01, 52100 at 900 SFM F.01. The other programmer does larger parts, and runs at a higher SFM with the same feedrate or higher. If I ran his SFM on the smaller parts, my tool life would go down, yet his tool life is good. Don't know why, just know that is the way it is.

In your 2nd post you asked, "how is it that you can't get the RPM'S to end up at, say, 750 RPM's on a 2.5" part??? Without starting out at 150 RPM's!! "

That is because you are programming G96S250M3 at the start of your operation. Do this instead. Say you want to start facing at X2.55. 250 SFM at that diameter is 374 RPM. Program like this:

INDEX POSITION
G97S374M3
T0101M8
G0X2.55Z0
G50S3000
G96S250
G1X-.065F.004

Now the RPM is correct for the starting position. Also notice that the G50 is your friend. No more 5000 RPM as it cuts to the center.

You also asked if there wasn't a way to achieve higher RPM without going to the center. Sure. Increase the SFM.

One thing to consider if rough facing a different material at say F.01 is to slow the feedrate down as it approaches center. I normally switch to F.004 at X.2. Your insert will thank you.

You asked "Is this what determines your SFM? The max diameter? " Absolutely not. Grade of insert and material are the major determining factors. Sometimes you may need to change from the desired SFM because of chatter or to get a certain finish, as an example. Normally a higher SFM will give you a better finish in steels. Especially the soft ones. Increasing the DOC on soft steels will usually give a better finish.

Only job we use ceramics on does not face to center so I can't help you much there. Other than to agree with a previous poster. Your SFM is dropping way to low as it approaches center. Ceramics love heat.

EDIT: Couple more thoughts. Is the cut an interrupted one from the saw cut? Not good if yes. What DOC are you taking? Keep it shallow. Maybe .020/.030 DOC.

[gene rhodes]

thanks for the info guys...I will copy this info to my C drive to use as future reference. I am learning more and more that running and programming are COMPLETELY different animals!! the floor experience has helped quite a bit but I still have a TON to learn. On top of all this, they've got me proving posts out as well!! I have been successful with 20 machines so far, but not without a few headaches along the way!! New programmer, new programs, new program format, new posts... hard to build a rep. that says " man, he knows what he's doing" with odds like that!! But hey, what's life without a few challenges along the way, right?!?!?!
Anyway, thanks again and I'm sure you'll be hearing from me soon......I'll let you know how this worked out for me....