Nitronic 40

[K2csq7]

I have some parts I did in the past, but we ended up turning the material off the faces. Parts are about 40" X 40" and we have to take a bit more than 1" off the face(s). I had a Sandvik rep in here with a couple face mills and maybe 4 different grades of inserts... Nothing remotely efficient came out of that... it worked, but slow as $^&$ and the inserts got eaten by the dozens...

Our machines are Daewoo ACE's (horizontals) with (i think) 30 horsepower.

Turning the material off took about 12 hrs/part ... we have 3 of them coming up in the next few months. The material is not hard at all, but EXTREMELY abrasive.

 

Any ideas on some heavy duty tooling that I can demolish this material with?

TIA

[jeff]

I've machined Nitronic 60 in the past, and I don't remember having this issue.

Not sure how different the 40 is from the 60 though.

From what I recall, it's like 4150 pht.

Sorry I can't give you more help.

[strabe]

I too have machined N60 but not 40. What kind of insert life did the lathe have? I'd look at what grade those inserts were and see if you can find something comparable for a face mill. Good luck.

[K2csq7]

The inserts in the lathe didn't have that great of life, but they were big SNMG 644 IIRC. The DOC was a little more than .300 and his feed was up near .018 ipr.

The one thing that did work well for me was drilling with inserted drills, up to 2" dia, coolant thru, but it was nearly impossible to get the chips to break...

I also tried running the tools dry and that didn't seem to help.

I did some comparing 60 to 40,

40 has a bit less nickel, but more manganese and chromium...

[Hardmill]

What kind of tools did the sandvik rep use ??

They have some good stuff and should have had you up and running

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[gcode]

Did you try Sandvik button cutter (Coro200)

 

I've had good results using them in hard stuff with Ø.75" insert and .1 to .15" depth of cut and 40% radial stepover

 

An Iscar Feed mill might be a good choice too

[K2csq7]

The inserts (still have em all broken & beaten in my desk lol...) R300-2060M-MM and R300-2060M-PM <<< .750 buttons

 

it was a 4" face mill RA 300-102 R38 20M was the cutter.

 

Couldn't get more than 125" without trashing the edges....my WOC was like 3.75 and DOC was .1875

 

 

40" X 40" and we have to take a bit more than 1" off the face(s)

 

Thinking I need like a 10" facemill, I have 30 HP.... The part weighs close to 6K lbs..

I wish I could plunge it of, but I'm guessing the retracts with this material would kill the inserts real quick...

Need Mcam to be able to hop up and away from the material on the plunge retracts....

[jeff]

You'll need more than 30hp to push a 10" facemill lol.

Maybe try a different type of coating on the insert?

[K2csq7]

You'll need more than 30hp to push a 10" facemill lol.

 

 

Do you have any unobtainium I could coat em with?

 

Maybe I need some oil instead of coolant...

I am going to ask my boss if I can take a 5hr. field trip to the forging house in PA to steal some of their secrets

[K2csq7]

Talked to the guy at the forging house... says they run old 8" facemills dry with square TiN coated inserts, bit less than 100 SFM, and about 3-4 IPM... and it works like crap... . He asked that if I find anyting to let him know :lol:.

 

The actual spec on the material is ASME SA-336, FMX-11, annealed... AKA **$*#*#^^*$%@&*$#(^@&*^$@#%

[Kris Bennett]

I cut Nitronic 50, Nitronic 50 High Strength, and Nitronic 60 quite often... Using that Sandvik R300 button cutter try using the S30-T grade.. Most of the Sandvik reps are just learning about it as it is very new.. Run about 325 SFM with about .008 chip load per tooth.. And as deep as your horsepower will allow.. NO, I repeat, NO coolant... The thermal shock is what is killing your inserts..

I've also had a lot of luck with Walters facemills with the insert on 45 deg.. Also, NO coolant..

[K2csq7]

Thanks kjb5150

[Jeremy Herron@DBS Solutions™]

We use the Sandvik R300 button cutters too Keith 1/2 I.C. inserts grade 2040 flat top insert. I think about 600 sfm and .008 f.p.t. and Dry. I will double check speeds, feeds, and edge prep on the inserts in the a.m. and let you know for sure though.

[Jeremy Herron@DBS Solutions™]

R300-1340E- MM 2040, 600 sfm .008 fpt .125 doc 45% stepover air blast. We get about 45 mins in cut, but I am milling out peices that have been brazed into a gas turbine cover so they are extra hard with a lot of nasty interruptions.

 

HTH

 

[Jeremy Herron@DBS Solutions™]

double post. Doh!

[K2csq7]

The gold ones... I've still got the used ones in my desk... (3/4" i.c.) (had a 4" face mill on trial...)

45 min!!!!!! 600SFM!!!!!!!!!

I couldn't get more than ~10 mins. in the cut before they were toast (wet or dry)... and my sfm was only ~100 (did try higher, maybe up to 400) The abrasion wear was/is (lookin at em now) horrible, looks like someone held em up to a belt sander....

IIRC my W.O.C. was like 85% and D.O.C. 1/8 - 3/16"

[Jeremy Herron@DBS Solutions™]

I will call some of my gurus tomorrow.