[K-fab50s]

This is my first post on CNC Zone so go ahead, make the newbie cracks. :cheers:
I've already done the search and not come up with the answers I'm looking for, so here we go!

Setup info first:
I have a Proto-Trac 1745S that I've been turning 304 Stainless high misalignment spacers with.

The setup I've had the most success with turning the 304 is using Dorian VNMG-432-EG-DP25 inserts, turning the stock at 660 rpm, taking .015" @ 12.5 ipm passes for roughing, .005" @5.0 ipm finishing. I'm using one of Milicron's coolants. (forget which one, sorry - it works great on aluminum!) Most of the stock I'm cutting is between .625" and 1.250" in diam.

I have a nice surface finish, but this setup's hard on my tooling. I get about four or five pieces per cutting edge of the inserts before I start loosing tolerance. I also end up having a rolled edge on what should be a sharp point on the spacers. Right now I'm just going back and facing off the little rolled edge with a cutoff tool, but is there a way to avoid this or is it just the nature of the 304?

:stickpoke I'm getting stringers, not chips (once again - is this the nature of stainless?), they're generally slightly discolored to just starting to turn bluish. I've produced brown chips with a couple setups and it's not pretty... (too fast spindle speed and/or feed rates, right?)

I've played with speeds from 1100 rpm to 400 and feeds from to 5.0 ipm to 20.0 with cuts from .005" up to .025". I can't get tool life! (chair)

I'm guessing it's probably my choice of insert more than anything - my local tool supplier's been a bit of a help, but hasn't nailed it for me. Can someone give me some guidelines to start with? Insert, speeds/feeds and cut depth would be a great help.

I'm also getting ready to turn some 4130 and/or 4140 (not sure which one yet - gotta go do some more materials research). Biggest diam. will be about 6", smallest diam will be about 1".

On the few occasions that I have turned 4130 bar (1.250"), I end up with a torn surface instead of a nice smooth machined surface. I've run various speeds & feeds, but always seem to end up with similar results.

So how about it? Guide lines on speeds, feeds and depth of cut for the chromoly?

Does anyone know of a general chart (web site?) that would show the basics for me? Speeds/feeds/cut rates for different materials. I know it would be more of a guide line to start with, but so far I've been a trial and error operator, so more info would be great. (and probably less expensive!)

Thanks in advance.

[bennett71]

This might sound stupid, but is your on center or slightly above?

[K-fab50s]

This might sound stupid, but is your on center or slightly above?

I've tried to keep it on center or just a hair below.

[HuFlungDung]

Turning 304 SS is quite different than 4140. It largely has to do with insert coatings. The correct coating is absolutely necessary to get good insert life with 304SS. The material will weld itself to the wrong coating and begin to pull pieces off the cutting edge, commonly known as the built up edge phenomena. So consult your tooling catalogues as to suitable coatings for turning the 304.

The insert shape also has a lot to do with good chip flow. If the chip is piling up on the tool, such as it often the case with VNMG, it will wreck the tool. The VNMG is a negative rake insert, and does not have a positive rake chipbreaker to promote good flow in stainless cutting.

I don't know of any insert that does a good job of short-chipping 304, because those that do, force the chip to break on the side of the insert and this causes crating on the side of the insert.

Personally, I like to use Kennametal/Hertel Fix_perfect style inserts for turning 304SS. This unusual shape of tool (eight sided on edge) will roll the chip into a smooth spiral "cable" that may break between 3 to 12" in length. But, nice to handle, and they will fall down in the chip pan. I usually rough at about .05 to .1" DOC and .005"/rev feedrate with this tool. Surface speed, I keep down to about 300 fpm, as the heat buildup at the tip can be extreme with stainless. I use lots of flood coolant, too.

Iscar Cutgrip will also do an excellent job in 304SS. These also roll the chip up into a spiral cable. The correct coating is still mandatory for good insert life.

Turning C4140, use CNMG's to rough and finish with. There's lots of good grades and coatings that will handle it, and this is an economical insert shape to buy. Use the VNMG sparingly, it cannot handle much "plunge and turn", and should only be used where a tiny profiling feature demands it.

[bennett71]

Definatly use a positive cutter like HuFlungDung posted. You need to keep the insert engaged in 304 & always take a chip. I have had a lot of luck with wnmg inserts tin coated for stainless. I have machined a lot of inconel, stainless, precipitation hardened alloy 286 etc. in the past & it is not fun. Letting up on the feed with light cuts to prolong tool life can ruin an insert quickly.

[mrainey]

There's an interesting discussion about insert styles here (especially VNMG).


http://www.practicalmachinist.com/ub...;f=13;t=002020

[little bubba]

K-Fab First problem I see is that your talking about RPMs and IPM, I guess we can take a guess the inches per tooth based on the stated RPMs but running 660 rpms on stock from .625 to 1.25 inches in diameter is a big difference. First thing to do is start thinking in surface footage, RPMs mean nothing, your cutter doesn't care what RPMs the stock is turning, it cares about the linear velocity in which it is going through the stock. Same thing for the IPM, that doesn't matter, what matters is chip load, as in .005 per tooth or in the case of a lathe per rev.

I'll agree with most of whats been said, 304 sucks, it does not like to break chips. I've been intermitantly running a losing job on the lathe in 304, and I cannot get the chips to break(I can, but insert life suffers tremendously), I'm getting only about 70 pounds of stringy fluffy chips per barrel. I've found that a rather positive insert works best for tool life.

I would toss the V series insert, rather weak, check out the thread in one of the posts above.

As for the 4140, if your getting a torn finish, then its probably annealed or what McMaster Carr calls prehard, 'may be up to 35C' but is always in the 26 range(not quite hard enough). In that case, let it smear all it wants on your roughing cuts, then let it rip(high surface feet) for a finish. A negative insert will also lead to a torn finish. I've found that turning the coolant off will usually result in a nicer finish cut on annealed 4140/30 and mild steels. For these kind of finish cuts you will want a harder not tougher insert or maybe even a cermet.

[K-fab50s]

K-Fab First problem I see is that your talking about RPMs and IPM, I guess we can take a guess the inches per tooth based on the stated RPMs but running 660 rpms on stock from .625 to 1.25 inches in diameter is a big difference. First thing to do is start thinking in surface footage, RPMs mean nothing, your cutter doesn't care what RPMs the stock is turning, it cares about the linear velocity in which it is going through the stock. Same thing for the IPM, that doesn't matter, what matters is chip load, as in .005 per tooth or in the case of a lathe per rev.

I agree entirely with the RPM versus surface velocity. The reason I stated RPM is that my Prototrac does not offer a constant surface speed spindle - that was another model.

The pieces I turn start out at either 1.000" diam and get machined down to .625" min. (in certain places, larger in others) or they start out at 1.125" and get turned down to .750". I have to find a spindle speed that covers the range. Once I hit the run button, it's step away and let the machine spit out the part. If I can find a happy medium, that would be good.

I also understand/agree with the feed per rev. I've done some calculations to determine the feed needed, but with the (obviously wrong) inserts I've been using, the finish I was getting with the numbers that I had - well... hence the experimenting with different spindle speeds and feeds.

Once again, my original post was looking for the basic starting points and then I'll tune to my machine.

Heck, if someone's kind enough to give me surface speed, feed/rev and the insert I need for turning 304, that would be wonderful!!

My original decision (wrong!) to use the VNMG was based on the profile of the pieces I am making. The diamond shape they offer allows me to profile my part with only one tool, get the 90 degree shoulder I need and cut the radius required for the ball joint to clear the body of the spacer. (see pic below)

I'll agree with most of whats been said, 304 sucks, it does not like to break chips. I've been intermitantly running a losing job on the lathe in 304, and I cannot get the chips to break (I can, but insert life suffers tremendously), I'm getting only about 70 pounds of stringy fluffy chips per barrel. I've found that a rather positive insert works best for tool life.

The comment I made about chips was more of a general question/observation. I'm usually machining aluminum and I get chips, not stringers. Obviously, from the answers I've seen, 304 is stringy. I can live with that. Once again, more of a query than me expecting to get chips. - making sure I wasn't doing something (else) wrong. :drowning:

I would toss the V series insert, rather weak, check out the thread in one of the posts above.

Gonna go talk to my tool guy either today or tomorrow. The info you guys have given me is exactly what I need and I thank you all for the guidance.

As for the 4140, if your getting a torn finish, then its probably annealed or what McMaster Carr calls prehard, 'may be up to 35C' but is always in the 26 range(not quite hard enough). In that case, let it smear all it wants on your roughing cuts, then let it rip (high surface feet) for a finish. A negative insert will also lead to a torn finish. I've found that turning the coolant off will usually result in a nicer finish cut on annealed 4140/30 and mild steels. For these kind of finish cuts you will want a harder not tougher insert or maybe even a cermet.

Cool. Once again, this is the sort of info I was looking for. Thanks!

As I've discovered, 304's a STRANGE animal to work with - especially when you're used to Al... I'm just trying to learn the basics of the stuff. I've been playing with a mill and lathe for quite a while now - totally self taught, btw. I've been trying to apply the proper formulae and such, but when you miss the boat entirely (wrong tool, insert, what have you), well, the math doesn't necessarily do much good.
Trial by fire has been a damn good teacher, but sometimes it's a (nuts)and you have to go and get help.

[InspirationTool]

IANAPM (I am not a professional machinist), but have you looked at 303 instead? I've heard its easier to machine, and it should work the same unless you need to weld the part.

-Jeff

[K-fab50s]

303 might be the answer
If...
I didn't already have a butt load of 304 in hand already...

Thanks anyhow.

[One of Many]

303 might be the answer
If...
I didn't already have a butt load of 304 in hand already...

Thanks anyhow.

The insert and proper speeds and feeds may be the best answer.

I have found when material tears out on the finish, it is often due to the material welding itself to the cutting edge and there for becoming the new cutting edge, all be it a poor one at that. Wax cutting wax so to speak. Sulfer based cutting oil has worked OK for me in this regard, but it does not always relieve 100% of the problem. Inserts are nice, but I would rather grind and hone my own edge for PIA materials that work harden so easily.

DC

[little bubba]

K-Fab, you asked for a starting point in 304, I'm just taking an educated guess. You don't have constant surface speed, so I would start out at about 500-550 SFM based on your maximum diameter. Then, since your running a fairly long skinny part, feed of maybe .008-.012 per rev, DOC of .015 to .030 depending on what kind of deflection your getting. On that same note, since your not really hogging, you could probably get away with VN insert, though I would make sure to get my hands on an insert that had a good positive chipbreaker, maybe 15 degrees, to overcome the -5 degrees in the toolholder, also make sure that you get an insert with no T-land. This should make for a nice low force cut that will keep the deflection down on your smallish parts.
I guearantee you will get stringers from this, but sometimes it unavoidable.

[K-fab50s]

K-Fab, you asked for a starting point in 304, I'm just taking an educated guess. You don't have constant surface speed, so I would start out at about 500-550 SFM based on your maximum diameter. Then, since your running a fairly long skinny part, feed of maybe .008-.012 per rev, DOC of .015 to .030 depending on what kind of deflection your getting. On that same note, since your not really hogging, you could probably get away with VN insert, though I would make sure to get my hands on an insert that had a good positive chipbreaker, maybe 15 degrees, to overcome the -5 degrees in the toolholder, also make sure that you get an insert with no T-land. This should make for a nice low force cut that will keep the deflection down on your smallish parts.
I guarantee you will get stringers from this, but sometimes it unavoidable.

Thank you. This is exactly the sort of information I need to get my starting point figured out. I'll be able to tune from there. I didn't get a chance to talk to my tooling supplier today, but have full intentions of sitting down with him tomorrow and discussing this more with him.

As far as the piece being long - no, not really. The bar stock sticks about 1.5" out of the end of the chuck. Very little deflection. Most of the spacers are only .750" to 1.000" in length.

I have one more question. I keep seeing "DOC" in turning related posts - would you like to fill me in on this? Diameter Of Cut? Distance Off Center? Like I said earlier, self taught. Never worked in a machine shop, don't know any machinists and such - so I'm pretty stupid to some of the terms. (and not afraid to admit it. Ego in such instances just gets you in trouble.)

Stringers aren't a problem. I've got a 55 gallon jug full of stainless coils. Sharp suckers! - I use welding gloves and long reach needle nose pliers to pull them out after each part's been made. Learned real quick how sharp they are a couple years ago. Nothing like AL!!!

[little bubba]

DOC - depth of cut, radial value, not diameter. I would say that 1.5" sticking out on a part that is going to .625 is getting in in the spindly range. I wouldn't want to take a .120 DOC on it, which you should be able to take if your part was 4" in diameter, and sticking out 2inches.

Who is your 'tooling guy'? Some sales reps are really good, others have no clue but can spew out amazing amounts of crap from the catalog. I sat in a Kennametal presentation a few months back and there were a couple of guys who had just purchased a new Mazak Lathe and had no clue about machining, they were making some parts on a manual lathe and were asking all kinds of questions about RPMs. They were asking why they were breaking inserts when turning a 4" diameter at 400rpms but at 2" diameter they were making good chips. This rep is going on and on about chip breakers and grades and material and this and that, but didn't have the machining background to explain to them that its not RPMs but surface footage. If you knew what you wanted, he could quote you the chip breaker and grade off of the top of his head though.

On the flip side our Sandvik rep is a fricken genious, well actually they say its not what you know, its who you know. If he's not 100% sure of what you need he'll get on the phone and has a contact that will know or who knows somebody that will know, and then he'll get the info for you.

If you have the former instead of the latter, from my expierience, you want an insert that is halfway between hard and tough, maybe leaning a bit toward s the hard. No negative t-land or primary. You want positive, though probably not as positive as you would use for aluminum, maybe a 5-10 degree positive primary angle to add some edge strength, leading back into a more positive chip breaker, though your probably not going to break the chips anyway, so that doesn't matter. I'm sure there are more people on here with lots more expierience than me so, I may be totally wrong, but from what I know now, that is what I would go with. For what its worth a couple of weeks ago I was having insert drill problems in 304. Kennametal suggested X insert, it was worse than the one I was using that was totally wrong, so they set me up with another set of inside and outside inserts, worked like a charm. However their original suggestion worked great on the "backup" drill as a boring bar, 400 minutes of tool life per corner, I can live with that. Just some thoughts to keep in mind.