Nitronic 50 material?

[Mgrenier]

Hello all,

 

I did a search of previous posts and I need more info (if possible) about this material.

 

We never machined this kind of material and I have a few questions. We were wondering if this kind of material has a tendency to deform while machining or is it stable.

 

Also, if any of you guys can give me some pointers as far as what kind of tools should we use. and where should I start as far as speeds and feeds are concerned.

 

Any information is very appreciated,

 

Have a nice day,

[Harryman]

Cuts about like 303 stainless.

[chris m]

Nitronic 60 cuts like crap; no experience with 50

 

C

[Guest CNC Apps Guy 1]

It's a real bear to knurl, lots of pressure needed. Harry and Chris said it right though. It is a bear. Not on the order of the exotics (Waspalloy, Inconel, Rene, etc...) but still more difficult than most.

[Tim Johnson]

This should get you started. If you are machining cold drawn back off the speeds 15%.

 

 

STAINLESS STEEL (NITRONIC 60 ANNEALED)

 

1. TURNING

DEPTH OF CUT SPEED FEED

COATED CARBIDE INSERT-ROUGHING .100 400,500 .008

HSS .040 60 .007

.150 50 .015

.300 40 .020

CARBIDE .040 190 .007

.150 160 .015

.300 125 .020

COATED CARBIDE INSERT .040 -- .

.150 -- .

.300 -- .

 

2. CUTOFF & FORM TOOLS TOOL WIDTH SPEED FEED

HSS .062 45 .001

.125 45 .0012

.250 45 .0015

.500 45 .0015

CARBIDE .062 150 .001

.125 150 .0012

.250 150 .0015

.500 150 .0015

COATED CARBIDE INSERT .062

.157

 

3. THREADING THREAD DIAMETER SPEED 1ST PASS LAST PASS

CARBIDE UNDER 1" 65-100 .015 .001

OVER 1" 80-120 .015 .001

HSS UNDER 1" 8-20 .015 .001

OVER 1" 10-25 .015 .001

 

4. FACE MILLING DEPTH OF CUT SPEED FEED PER TOOTH

HSS .040 80 .006

.150 60 .010

.300 45 .014

CARBIDE .040 195 .007

.150 170 .010

.300 135 .014

INDEXABLE .040 240 .007

.150 210 .010

.300 165 .014

 

6. SLAB MILLING DEPTH OF CUT SPEED FEED PER TOOTH

HSS .040 80 .005

.150 75 .007

.300 55 .009

 

7. SLOT MILLING(ARBOR CUTTERS)DEPTH OF CUT SPEED FEED PER TOOTH

HSS .040 45 .004

.150 40 .006

.300 30 .008

CARBIDE .040 125 .004

.150 110 .006

.300 90 .008

INDEXABLE .040 155 .004

.150 135 .006

.300 105 .008

 

8. END MILLING-PERIPHERAL DEPTH OF CUT SPEED CUTTER DIA. FEED PER TOOTH

HSS .020 60 3/8" .001

.020 60 1/2" .002

.020 60 3/4" .003

.020 60 1-2" .004

.060 45 3/8" .0015

.060 45 1/2" .003

.060 45 3/4" .004

.060 45 1-2" .005

DIA/4 40 3/8" .001

DIA/4 40 1/2" .0015

DIA/4 40 3/4" .003

DIA/4 40 1-2" .004

DIA/2 35 3/8" .0007

DIA/2 35 1/2" .001

DIA/2 35 3/4" .002

DIA/2 35 1-2" .003

CARBIDE .020 220 3/8" .0005

.020 220 1/2" .001

.020 220 3/4" .002

.020 220 1-2" .003

.060 170 3/8" .001

.060 170 1/2" .002

.060 170 3/4" .003

.060 170 1-2" .004

DIA/4 140 3/8" .001

DIA/4 140 1/2" .0015

DIA/4 140 3/4" .0025

DIA/4 140 1-2" .003

DIA/2 130 3/8" .0005

DIA/2 130 1/2" .001

DIA/2 130 3/4" .002

DIA/2 130 1-2" .0025

 

9. END MILLING-SLOTTING DEPTH OF CUT SPEED CUTTER DIA. FEED PER TOOTH

HSS .030 40 3/8" .0005

.030 40 1/2" .001

.030 40 3/4" .002

.030 40 1-2" .003

.125 385 3/8" .0007

.125 535 1/2" .0015

.125 535 3/4" .0025

.125 535 1-2" .004

DIA/2 30 3/8" .0005

DIA/2 30 1/2" .001

DIA/2 30 3/4" .0015

DIA/2 30 1-2" .0025

DIA/1 25 3/8" ----

DIA/1 25 1/2" .0005

DIA/1 25 3/4" .001

DIA/1 25 1-2" .0015

 

10. THREAD MILLING

SPEED FEED PER TOOTH

HSS 45 .0015

CARBIDE

INDEXABLE

 

11. DRILLING SPEED DRILL DIA FEED PER REV.

HSS 45 1/16" .001 DIA/63

45 1/8" .002 DIA/62

45 1/4" .004 DIA/62

45 1/2" .007 DIA/72

45 3/4" .010 DIA/75

45 1" .012 DIA/83

45 1 1/2" .015 DIA/100

45 2" .018 DIA/111

 

12. SPADE DRILLING SPEED DRILL DIA FEED PER REV.

HSS 35 3/4"-1" .006

35 1"-1 1/4" .007

35 2" .010

35 3" .013

CARBIDE

 

 

 

 

13. INDEXABLE DRILLING SPEED DRILL DIA FEED PER REV.

426 3/4" .0016

426 1" .0024

361 1 1/4" .0031

361 1 1/2" .0031

361 1 3/4" .0031

295 2" .0039

 

14. REAMING SPEED DRILL DIA FEED PER REV.

HSS 30 1/8" .003

30 1/4" .003

30 1/2" .004

30 1" .006

30 1 1/2" .007

30 2" .008

CARBIDE 40 1/8" .003

40 1/4" .004

40 1/2" .006

40 1" .008

40 1 1/2" .009

40 2" .010

 

15. BORING DEPTH OF CUT SPEED FEED PER REV.

HSS .010 65 .003

.050 50 .005

.100 40 .012

CARBIDE .010 165 .003

.050 130 .005

.100 115 .012

INDEXABLE .010 195 .003

.050 155 .005

.100 135 .012

 

16. C-BORING & SPOTFACING SPEED DRILL DIA FEED PER REV.

HSS 50 1/4" .002

50 1/2" .003

50 3/4" .003

50 1" .003

50 1 1/2" .004

CARBIDE 110 1/4" .002

110 1/2" .003

110 3/4" .003

110 1" .003

110 1 1/2" .004

 

17. TAPPING SPEED PITCH

10 7 OR LESS

12 8-15

16 16-24

20 OVER 24

 

18. COLD FORM TAPPING SPEED PITCH

20 7 OR LESS

24 8-15

16 16-24

20 OVER 24

[Tim Johnson]

Sorry, this chart looked better on my monitor

[Mgrenier]

Thanks alot guys, that info will become very handy in a very near future.

 

BTW, the material will be casted. Hope everything goes right.

 

Thanks again and have a nice day,

 

P.S. Any additionnal info is welcomed.

[chris m]

quote:

---

the material will be casted

---

OUCH

 

The skin of the casting on our Nitronic 60 castings is a bitch to cut. Don't tickle it, take a healthy DOC to get under it ans keep the SFM down [350ish] and you should be OK

 

C

[Jack Mitchell]

http://www.goodwinalloys.com/data3.htm

 

Looks like between 31% to 47% nickle/chromium content.

 

This stuff is bad news; once machined (assuming a valve or pressure pump) you can stand five feet back and still witness that nickel/chromium wave - it's unmistakable.

 

Good luck with this - I might suggest 1/64 Tnr for turning with light cuts & aggressive feeds.

For milling?

Get a bad case of the stomach flue if at all possible.

 

" notoriously stiff alloy with a high hot strength " actually shows that the author has a sense of humour.

 

 

Regards, Jack

[Harryman]

Try angled roughing passes to come out of the cut from below the skin. This method is working great for me on plasma cut 304.

[Jack Mitchell]

It's unusual to see a casting as opposed to a forging on this type of material; still rather expensive either way.

 

304SS is a little bit tough for me when it comes to milling and turning.

303SS is gravy in every sense of the word; actually, I prefer this material to mild steel or the like.

 

Of course these are merely my own opinions and should not necessarily be taken too seriously.

 

Regards, Jack

[Mgrenier]

quote:

---

assuming a valve or pressure pump

---

It is not, it seems like a cover of some sort and it has about 85 pockets in it. I am starting to get scared about this job.

 

Thanks again for the info.

[chris m]

Just keep the surface speed down and use inserted cutters wherever possible. The mat'l is pretty tough so just don't get crazy aggressive and try to use multiple roughing tools to get some tool life

 

C

[McRae]

I just finished a Nitronic 50 Job. SFM for turning was in the order of 300sfm and feed was normal per the chip breaker of the insert. Material work hardens so keep this in mind. Surface Finish comes up Beautiful and the approximate run time differential was 4 times that of carbon steel (keep an eye on your schedule and don't lie to your customer by underestimating the time to finish the job)

 

Milling, drilling and tapping - think Hastelloy C or equiv for cutting characteristics. Metalurigically this is more like a modified 309L stainless and if you are going to weld this stuff, there are galvanic corrosion possibilities so just be careful and do your homework.

[McRae]

Tim Johnson 2002 - Please indicate the source of the information that you have presented. I am looking for similar data sheets for other material groups and that looks quite comprehensive.

 

Thanks

[chris m]

quote:

---

Surface Finish comes up Beautiful

---

What were you finishing with Andrew? My finishes always have that highschool-kid-Camaro look [really wavy] when I turn Nitronic 60

 

C

[Tim Johnson]

Andrew,

 

I created that information based on the Machining

Data Handbook. I drew it up looking something like the handbook showed, and the hss speeds in it are actually pretty close. The carbide speeds and feeds are for the most part obsolete. The actual speeds and feeds start from different sources. The carbide end mills come from Niagra cutter carbide book,(not the complete book, those speeds seem to be off), the drill speeds are a combo of Precision speeds and Gurring feeds, the carbide insert speeds start from the manufacturer. When I run new material I make a new list and adjust as I learn the real speeds and feeds. I pretty much started this 1 1/2 years ago.

[Jack Mitchell]

quote:

---

created that information based on the Machining Data Handbook.

---

Machining Data Handbook is available from the Machinability Data Center - Institute of Advanced Manufacturing Sciences, Inc.

111 Edison Drive, Cincinatti, Ohio 45216

 

ISBN 0-936974-02-8 (2 volumns)

Check them out for a newer release please - mine is the 1980 edition

 

Regards, Jack

[Jack Mitchell]

Martin,

 

You may or may not have experience with these types of materials; I’m not sure about your background, given the question that you initially posed.

 

This will be a very expensive workpiece.

Just relax and take your time, if your supervisor questions the amount of time required to learn this material then bye all means offer him the opportunity to do the job.

 

Hastelloy and nimonic alloys are rather difficult learning curves for almost anybody on this forum.

 

 

Regards, Jack

[McRae]

Chris,

 

Used conventional Turning tools and created some deep screw profiles using a side and face tool. We also ground some bearing fits.

 

Sales promised a delivery based on carbon steel and I am the villian because this thing has a compairitive machinability coefficient of .2 - so after 4 weeks, I now list to the left from the selective A$$ chewing that took place.

 

Jacks learning curve - I'm there man...

 

Tim - Thanks for the information. My set MDHB is pretty much to keep dust off of the book shelf for the same reasons you indicated.

[chris m]

I toooooold you that it was gonna be slow

 

Damn its tough being right all the time

 

 

We turn all of our bearing and seal diameters so the slow feed / light DOC is the primary reason behind the Bondo bucket finish, non-critical dims usually look better because we take more stock and run more feed.

 

C