CALLING ALL INCONEL GURUS!!!!

[Jedi Mastercam X]

Good day fellow Mastercam padawans.!!!

 

i was wanting input/advice on some inconel

718 that we will be running. just some general advice on SFM for roughing, finishing, threading, insert grades, etc. we have run this material before and Houston machine shops are infamous for the machining of exotic materials. but to the those who are familiar with this alloy know that it is ALWAYS a pain in the rump!!! but still, insights from others never hurts. Here are the specs to get started. Thanks in advance chaps!!!

 

60HP Puma 18 Turncenter

 

All O.D. work and no high finishes required on surfaces. 63 or better.

 

Geometry on piece is complex with compound angles and such, so the use of Left & Righthand O.D. Tools will be utilized.

 

can anyone suggest a good base SFM?

How much rough cut per side to take?

How much to leave for finish?

SFM for 5-7/8" 8TPI Stub Acme O.D.?

Raw piece is 7.25" O.D. x 18.5" Long. After machining each operation, overall Taper is not bad.

 

we have made similar pieces on same materials, but again, i think that we are missing something cuz all the inserts we tried are just frying!!!.

we have went from 80 up to 120 Base SFM, .01-.015 Per Rev. on Rough leaving .02 overall for finish. 80-120 SFM w/.006-.008 on finish.

 

any questions, please ask. thanks again in advance gentleman and have a great day!!!

 

-R.

[Guest]

Ceramics to rough is probably a good start. If there is a lot of material removal going on, I like to use a 3/4Ø button to start.

 

Especially if it is not an interuppted cut.

 

A sulfer based cutting oil is probably a good idea as well.

[Jedi Mastercam X]

Thanks John. i knew aobut the Oil & the ceramics. Unfortunately we are not gonna have the luxury of swapping out the coolant with oil. do u know how these ceramics will react with a traditional coolant/water solution?

[Guest]

The ceramics you'll cut dry with mostly but they react OK with coolant it's the sudden tempchanges that freak out ceramics.

 

In my experience with inconel and other exotics water based coolant is not a good option. You will tear up tooling in this stuff anyway but you want to try to maximize edge life. I have found in the past water based just does not give you that.

 

Maybe someone will chime in with something they have used with good luck in the past but I have found anything short of oil does not really work well on this stuff.

[Guest SAIPEM]

You're going to need to cut REALLY SLOW.

There is no way around it.

 

You can avoid ceramics if you have some good PVD.

I use Iscar IC908 because I don't cut all that much Inconel or other High-Temp Alloys.

 

For 718 start out at around 52 F.P.M and cut it dry with a PVD insert. Work your way up in speed as long as your surface finish is acceptable.

Keep your depth of cut low.

Roughing should be no more than 0.03 deep leaving no more than 0.003 for finish.

Give yourself at least 2 spring passes.

I know it sounds too slow, but trust me, you'll see better results.

Keep in mind the machine you're cutting it on.

Feedrate should start out at around 0.008 for roughing and 0.003 for finish.

 

If you have CBN or Ceramics, pay attention to the coating and run the Surface Speed at about 70% of what the tool manufacturer recommends.

No water based synthetic coolants! Thermal shock is very bad.

 

You will chew-up inserts.

There is no way around it.

 

[ 04-18-2006, 08:40 AM: Message edited by: SAIPEM ]

[Jedi Mastercam X]

Hey dude! r u the NEW programmer @ Saipem/Sonsub?

[Don S at Barefoot CNC South]

Hi, I sent you an email with info.

[Guest CNC Apps Guy 1]

Kennametal's Kyon 2000 Series has done the best I've seen with this stuff. Their reccommended feeds and speeds are right on for RIGID setups. I did say RIGID right? , Oh, one more thing, don't forget the RIGID setup. I cut it dry last time I ran the stuff.

 

HTH

[Guest]

Now James are you sure about that?

 

Rigid you said right?

 

You need to have a rigid set-up.

[kinglouie V]

if you must use the water soluble coolant, hope it's some good stuff like blazer and you remember to ramp up the concentration. By any chance is this 718 cast?

[Jedi Mastercam X]

i dont think its 718 cast. just a solid round piece of 718 105 KSI. i dont have the cert. so i am not sure. thanks a lot everyone for the 411. i appreciate it.

[bhayden10]

We machine 718 everyday here. Mostly turning work. Our roughing is at .03 depth of cut .016 ipm at 980 rpm. (216 rv on a mazak)These numbers are when it starts at 1" od. Were turning it down to .625 .75 long. We are using iscar .048 nr 907 grade. We are running water soluble coolant very thick. Getting roughly 10 parts per corner. Very interested in what others are doing though.

jm2c

[N3526J]

We run a 718 Inconel job faster than I've seen anywhere.

 

Here's the recipe:

1) 1.25dia X 3flt Kennemetal Facemill (.25rad inserts)

2)Kennematal ceramic inserts: KIPR125RP43540

3)4584 RPM and 41.25 IPM.

4).100" axial cut

5)Full dia cut

6)Run dry!

 

Oh yes..

 

7)50 taper horizontal mill.

 

You will see the prettiest color of orange-red chips spewing off the cutter. The work doesn't get hot and you get great cutter life.

 

 

HTH

 

Dan

[j.nguyen]

Dan From Everett? Do We Know Each Other?

 

Jamey N.

[Guest SAIPEM]

N3526J -

That tooling setup won't help much on a Daewoo Turning Center.

[rsbeadle]

I have turned some inconell before and had trouble until I figured out that the biggest problem is surface work hardening. I ran around 300sfm with an "el-cheapo" stellram insert at .050 face off cut. The piece I was turning was a 14" cast square (yes I said turning a square) for a hydraulic cylinder end piece. I faced off about .200 per corner. The tip held up well but I had terrible edge wear .050 back from the tip due to the work hardened edge. I am not sure if it was 718 inconell or not because it was a farm job and we did not order the steel for it, but was supposed to be 718. hope this helps.

[N3526J]

Jamey,

 

Whats a email for you?

 

 

Dan

[4xxx4]

My last inco job was 718 and I ran some kennametal 5510 on it. cngp432 150fpm .04doc and .01 or so fpr for roughing. This worked well but frequent tool changes are inevitable. The parts I did started at about 250lbs and finished at 12lbs (yeh, I know....). We finished at 200fpm with over .01doc running a vngg3305 5510 and it ran sweet. Lesser doc will be in the hardened layer and kill your tool.

I tripled the coolant concentration!! Blasercut...

I also ran a 1.44 carboloy insert drill thru some slugs and it ran well at 200fpm with .006fpr

 

I hope this helps. I don't like reccomending Kennametal but this ran well/predictable.

 

My broinlaw likes the iscar wnmg432/433 for roughing and says it kicks everyones butt....

[Jedi Mastercam X]

Thanks for the input/411 4xxx4!!!! and to everyone else. we are gonna fire up this bad boy probably 1st thing tomorrow morning.

[j.nguyen]

[email protected]

 

Jamey

[Jedi Mastercam X]

thanks again for the input chaps!!!!