Insert Life in Large 15-5 Stainless Turning

We do a significant amount of 15-5PH stainless steel CNC turning in the 8” to 25” diameter range. Parts are either bar stock or forgings that are usually hockey puck shaped. For OD roughing we use a CNMG 432 Iscar grade IC907 and run it at 325 SFM, 0.1 DOC, 0.01 IPR. Generally, we rotate the insert after 25-45 min of time in cut. All the turning is done in large slant bed lathes with flood coolant.

I am not convinced this is very efficient and think we could achieve a higher surface footage and much longer inserts life. I wanted so see if anyone on this forum had any experience with 15-5 and what kind of SFM and insert life they were able to achieve. Are the numbers we are running reasonable or could we do a lot better? Sandvik rep recommended trying a 4425 grade, I have also heard good things about 2025 and 2220. I plan to buy some samples of these inserts and give them a shot but wanted to get some other opinions.

Any experience or advice would be greatly appreciated. Thanks

Ask your reps for the freeby sample packs. Ingersoll has packs of 3 and each insert in the sample has a different chipbreaker.

CNMG432's are so common your grandma probably has a pack on her nightstand (sorry Bobw ).

Bottom line: if the rep won't give you a tool to try, he doesn't deserve your business.

Sandvik 2220 is definitely a lot better than the old 2025 in terms of tool life.
I'm not sure how IC907 compares to these. I have 1 pentacut tool that uses IC908 and that's a pretty good grade.

If you've got a good grab on the part and the HP required, I'd look at higher DOC rather than higher SFM. Heat from too high SFM is #1 killer.
DOC is free. You might be able to get away with a bit more feed too, but forgings can be funny and if its interrupted cuts keep the feed lower.

SND said:

Sandvik 2220 is definitely a lot better than the old 2025 in terms of tool life.
I'm not sure how IC907 compares to these. I have 1 pentacut tool that uses IC908 and that's a pretty good grade.

If you've got a good grab on the part and the HP required, I'd look at higher DOC rather than higher SFM. Heat from too high SFM is #1 killer.
DOC is free. You might be able to get away with a bit more feed too, but forgings can be funny and if its interrupted cuts keep the feed lower.

Click to expand...

I agree SFM seems good to me. Feed could go way up-double probably, but I'd start at .016". And DOC could also be double. (Assuming you mean you're taking the diameter down .2" per pass with .1" DOC).

R

I think the easiest way for better tool life is to crank up your feed. .010” isn’t much for a large lathe. Upping the feed will have the insert engaged less in the cut and will help insert life. Not to mention increase your metal removal. I sell Walter inserts for my tough applications as I’m a distributor sales guy. Their NRR chipbreaker which is a heavy duty chipbreaker that only comes in single sided turning inserts would be my first choice. I think you could run .030” IPR in 15-5PH. Or if you want the conventional double sided CNMG the RP5 chipbreaker will serve you well and you should have no problem running .020” IPR. I think 280-300 Sfm is a good speed. PM ME I’ll get you some FREE inserts to try out if you like.

personally with that much material coming off I would consider 1/2" round ceramics. typical SFM would be around 1000 cuts easy .200 per side feeds could be up to .015ipm, then us a cnmg for picking out the rads/corners and finish unless you have a big tol.
we ran inco with whisker ceramics at 850-1000sfm and up to .015IPM usually around .100-.150 doc.

Ledyard said:

We do a significant amount of 15-5PH stainless steel CNC turning in the 8” to 25” diameter range. Parts are either bar stock or forgings that are usually hockey puck shaped. For OD roughing we use a CNMG 432 Iscar grade IC907 and run it at 325 SFM, 0.1 DOC, 0.01 IPR. Generally, we rotate the insert after 25-45 min of time in cut. All the turning is done in large slant bed lathes with flood coolant.

I am not convinced this is very efficient and think we could achieve a higher surface footage and much longer inserts life. I wanted so see if anyone on this forum had any experience with 15-5 and what kind of SFM and insert life they were able to achieve. Are the numbers we are running reasonable or could we do a lot better? Sandvik rep recommended trying a 4425 grade, I have also heard good things about 2025 and 2220. I plan to buy some samples of these inserts and give them a shot but wanted to get some other opinions.

Any experience or advice would be greatly appreciated. Thanks

Click to expand...

.
some materials give abrasive wear to inserts and tool life is never very high. and if material has large hard spots of slag sudden tool failure can be a problem, this can give random problems
.
insert DOC often tied to vibration and hp limits of machine. obviously severe tool and part vibration can give sudden tool failure
.
feed rate usually use what inserts made for. a large change and if chip doesnt break up and is long wrapping around part it can easily be a big problem
.
often reliability is highly sought over a slight increase in cutting rate and then experiencing a random 2% sudden tool failure rate and the problems or damage that might occur. that is trying to save $100. labor or tooling and it costing $200. or more the long term data can say its not worth it. sure try stuff but record long term data of any problems. for actual machining times including any problems that might occur.
.
tool salesman will always sell you more tooling. watch for random problems increasing tooling costs rather than actually saving tooling costs over the year. often high reliability is cheapest rather than dealing with problems.

FFS Tom... stop! with the random tool failure bullshit. OP has a reliable process, just looking for improvement.

What brand of lathe? Rob has more experience than me on lathes for sure, but if it is a Haas you aren't going to get his feedrates/doc. I've had good luck with LNMX inserts in a Haas, but not sure what (if any) offerings you could find for a stainless grade (we were doing 4140ph with them)....

Consider also stepping up to a larger radius... 433 insert. Maybe even go up to a 543 insert and really increase your feed/DOC.
A harder grade on your barstock will help with being able to increase SFM but that harder grade may not like going through the first layer of a forging (depending on quality of the forging). I normally use Sandvik 432 MR 2025 in 316 hex barstock... 380 sfm, .01 feed, and keep the nose of the insert below the hex flat diameter (anywhere between .05-.15 DOC when measured to the corners of the stock). Whenever I run round stock I use 433 MR 2015 (harder grade) at 450 sfm and .013 feed. I cannot use the 2015 grade in the hex material because it gets beet up and chips out.

Any salesman should be willing to give you a free sample. Of course the bigger the customer the more free stuff you'll get.

Have you tried using the CNMG tools that use the other 2 sides of the insert?
Nice big lead, could possibly crank the feed up a little.

DMF_TomB said:

.
some materials give abrasive wear to inserts and tool life is never very high. and if material has large hard spots of slag sudden tool failure can be a problem, this can give random problems
.
insert DOC often tied to vibration and hp limits of machine. obviously severe tool and part vibration can give sudden tool failure
.
feed rate usually use what inserts made for. a large change and if chip doesnt break up and is long wrapping around part it can easily be a big problem
.
often reliability is highly sought over a slight increase in cutting rate and then experiencing a random 2% sudden tool failure rate and the problems or damage that might occur. that is trying to save $100. labor or tooling and it costing $200. or more the long term data can say its not worth it. sure try stuff but record long term data of any problems. for actual machining times including any problems that might occur.
.
tool salesman will always sell you more tooling. watch for random problems increasing tooling costs rather than actually saving tooling costs over the year. often high reliability is cheapest rather than dealing with problems.

Click to expand...

Tom, did your spreadsheet tell you to say that?

Because the OP doesn't have those problems.

Ledyard said:

I am not convinced this is very efficient and think we could achieve a higher surface footage and much longer inserts life.

Click to expand...

You mention that they are forgings. Is the insert life the same all throughout the turning process? Or do they fail quicker when you're making your first pass.

Mtndew said:

Have you tried using the CNMG tools that use the other 2 sides of the insert?
Nice big lead, could possibly crank the feed up a little.

Click to expand...

I second this, but only if your machine is tough enough to handle it. We use CNMG543 100 degree holders for roughing and you can rip right through the metal, sometimes stopping up the chip conveyor. We can get up to a .375 depth of cut at a feed of .024 IPR in 4340 at 400 SFM. In our larger lathes we run an Iscar COMG 646 in a 100 degree holder for depths up to .415 with a feed of .034 IPR and 450 SFM. The chips coming off of it look like Fritos.

When I used to chuck parts, we turned TONS of D2 every night. D2 is 12% chrome, 1.5% carbon, with Manganese, Molybdenum, Silicon & Vanadium. Tough stuff, and very abrasive.

I don't remember the exact insert, but we used Kennametal CNMG432's, I believe it was grade KCK10, and ??? chip-breaker. Doesn't really matter. We had a 25hp Okuma captain lathe, and some SOLID workholding.










750sfm, .012" ipr feed, and .450" DOC per side.


Let that sink in.


Tool life might have only been 10 minutes time in cut. But in those 10 minutes, it was RAINING chips inside the machine. $$$$$$$$$$$










I don't have a ton of experience with 15-5, but I can't imagine that it's 2x or more tougher than D2 to cut.

That being said, Iscar 907 is a fantastic finishing grade. It has a very hard substrate, and will offer awesome tool wear. But it wouldn't be my first choice for bulk material roughing. It has a PVD coating that's not going to offer a whole lot in terms of thermal resistance. In short, it's going to get hot before other coatings - namely aluminum oxide - will.

Unless you just have crappy workholding, there's no reason you shouldn't be taking .250" DOC per side, and probably .012-015" ipr feed.



I've gotta say, I think Walter's WSM10S grade may be the perfect tool for this. If I were using Seco products, I'd probably try TP0501/M6.

Iscar probably has a better insert for this too, but to really gain anything, you've got to start getting aggressive with your cutting parameters.