Anybody with experince of inconel?

Hi everyone, i am wondering if anybody here has any experince of machining inconel. I got a few different parts to make from this stuff which i've made before and was desperately hoping never to see again as it proved to be a real bitch to cut and took forever to do anything with.

I've tried out different grades of turning inserts from Seco and Kennametal which they reccomend for this stuff. Although the seco gear is by far superior it still doesn't seem to last that long at all and when it gives up it really does give up i.e. the insert breaks clean in half. This is doing the integrex 400y i look after no good at all and the turning tools are now under center height leaving a pip in the center of the bar after "edg fce" operations.

These parts are always small batches(7off for the upcoming orders) so i dont get that much opportunity to experiment with speeds and feeds. I've been told that its quite a narrow window between too fast and too slow for inconel and the best i seem to come up with is a surface speed of 30m/min at .2mm/rev feed and a roughing depth of 1.5-2mm. This is painfully slow especially as our supplier has minimum order quantities so im making all parts from the same bar and am having to turn 70mm dia bar dowm to 30mm for some bits!

Advice and suggestions from people who have also struggled with this stuff would be oh so greatly appreciated.

Even worse i got a fair bit of milling to do in some of these parts but because of the small quantities my manager is reluctent to try out any special cutters or inserts. I'm simply using coated hss ripper cutters and carbide end mills for finishing cuts and getting through absolutely shed loads of em. Seems like false economy to me but hey its his call, maybe he shouldn't have under quoted big time for this job.

Again input from anybody who knows anything about inconel would be very very helpfull.
Thanks.

There’s a PDF file here that should address machining Inconel (unfortunately I can’t tell you what’s in it – can’t open it at the moment due to computer problems!).

http://www.specialmetals.com/documents/machining.pdf

Source:-
http://www.specialmetals.com/general.htm

(Special Metals Wiggin Ltd in Hereford)

It (well, 718 for sure) is much more machinable in the solution annealed state than the hardened state.

There is a funny story about a UK shop making stuff for us after being warned up front about the heat treat issue. But they "knew better" and lost their shirt.

Like two expensive thread mills for each 1/2-13 blind tapped hole - not to mention enormous time over runs.

John

Thanks for the help guys its really good of both of you.

Asquith. The PDF file is really usefull. 33 pages in total with loads of speed/feed data for many machining operations without going too deeply into the metallurgy science, i never have tried to understand all that its a bit "rocket science" for me! Seems i've been using cutting speeds within those listed but at the upper end of the scale. Also, as i read it, i should be using heavier feeds and depths due to Inconel being prone to work hardening. I'll try slowing it up a bit and pushing in harder,

John. You were spot on, 718 and also the X750 we have are both refered to as being in the same material group in the PDF. It reccomends rough machining in the annealed state and finishing after precipitation hardening/ageing. However with the relatively wide limits on the parts we have and advised distortion of up to 0.07% we may well be able to finish the parts before heat treat and then pickle or powder blast them. I need to speak to the engineering dept to see if they think this may be a good idea, presuming of course this is not alredy being done. If it is annealed stuff we already have i'd say it would be pretty much unworkable once hardend.

Cheers guys, much appreciated.

We turn/mill a few Inconel jobs a month. Its mostly 625 and some 718 in the annealed condition. I use Kennametal CNMG-MS KC5510 to rough, 125-225 sfm. I run toward the lower side if I need to bring in a groover or another tool that may not hold up to the work hardening created at 200sfm. Feed .010-.015IPM/ DOC around .06-0125". Drilling under 13,5mm I use Guhring RT100, Firex coated drills, 60-80 sfm/ feed .002-.008 depending on diameter. Larger holes we just Walter indexable insert drills. SFM 125-200sfm, .002-.004IPR Feed. Pecking is the enemy of drilling 718 (like other work hardening alloys). I don't have high pressure coolant so have to peck sometimes in deeper drilled holes, but really try to avoid it.
I pulled up a program for an 1-1/4 OD Rod End Ball that we made.
Rough OD: 110sfm/.014IPR/.100"DOC.
Finish OD: 200sfm/.004IPR/FIN-X= .010
Drill, 1"dia: 195sfm/.0024 IPR (3/4" deep, no pecking).
Rough ID: 120sfm/.005IPR/.027"DOC(not much removal needed after drill)
Finish ID: 150sfm/.005IPR
Cutoff: 120sfm/.001IPR/no peck (goes from X1.2 to X1.0 so pecking not needed)

Much of this info may be part specific and vary depending of you finish part requirments. You were saying you were turning around 30m/min, I think thats about 100sf/min. If you have large diameter turning (38mm and up) and plan on seeing this parts coming back, you might consider ceramics. I used a Greenleaf WG300 round insert to rough a part from 2-1/4"(57mm) rod. I used 900sfm (274m/min). Down sides include programing to deal with the series Depth of Cut Notch that occurs, and the tool life is about 4-6 minutes of actual use per edge. But its spinning 7-9 times faster. I also increased the coolant concentration to 10-14% but that was mostly to aid drilling lubricity.

I haven't cut any Inconel since the 80's, cut it for many years, Aerospace Industry, the best insert I ever ran into was from SECO, grade HX, simple as that, it would just cut and cut and cut and cut and....... well you get the idea!came in every geometry even in topnotch cutting tools!!

Don't know if Seco offers it any more!
LOW FEEDS and LOW SPEEDS

here is an eBay link to some HX grade inserts
Seco HX grade inserts on eBay

These Seco inserts might not be too bad. Was turning L-605 Ni Cobalt last week and the local Seco rep happened by with his CP200P grade. Didn't quite have the best geometry for the application on him. But, it proved a little better than the KC5510.

The Seco gear i used in the past was CP200 grade but with no "P" at the end. I found it lasted twice as long as the kennametal stuff(not exactly sure which grade). The good news is i have changed machines, still on an integrex but one that is in much better condition and which the foreman doesnt like to put inconel on.

Our inconel bits should be coming through in the next couple of shifts so i'll be able to tease the poor guy who filled my shoes for a shift or so, at which point i'll pass on everything i've heard here. Thanks Guys.

Low speeds, low feeds, BUT! Don't let the tool "rub" i.e.,keep a positive feed going where you keep a chip forming. I don't know if that makes sense if you haven't done it but you'll know what I mean when you see it. The idea is to prevent work-hardening.

This thread brought back memories of my aerospace days..Inconel, Waspalloy, Rene 141, blegh!

I just bought my first boxes of Seco inserts. 2 geometries in the CP200P (they say they improved the CP200 and are adding a "P" until the old inventory is used up) and 2 different geometrys of the new TP2500. I'm going to test them out against the equipment we're currently using as worthy test subjects arise. The TP2500 kept going where my Kennametal quit in a larger 17-4 H1150 part...at 100sfm faster I might add. When I get a obvious result like that, I have to lift an eyebrow and think there might be something here.
We should start a post highlighting different tooling, speeds, feeds, etc to display potential options with tooling in different materials as they come up.
Thanks for mentioning Seco, I have high hopes for improvement.

we machine inco 718 day in day out nasty stuff and yes very slow to machine.
typically 25/30m/min at .25feed/rev for finishing 0.25mm DOC.
Rouching we use greenleaf ceramic 270m/min at 0.35mmfeed/rev 2.00mm DOC

Sandvik have just released some new coating grades which we are currently trialing with positive results so far. mainly extended tool life. Sandvik are also working on different types of cutter approach when creating slots.

hope this helps

Man, it sure seems like Seco has gotten a lot better.I always hated thier stuff.It was always cheaper than anyone else but only lasted about half as long as any other brand.Anyhow in part to your thread.For the milling on Inconel I always use a Cobalt endmill.Its a lot slower cutting but lasts a lot longer due to not being brittle and chipping like Carbide endmills.

SF, When I posted my last posts, I had hopes that this new TP2500 grade would be the one size fits all. I definately felt the same as you before...cheap Seco inserts used by cheap shops. During my testing thus far, The Seco is outperforming my Kennametal for roughing certain materials: Nitronic 60, and 17-4 H1150 are the most notable with 3-5x's increase in life and about 10-15% increase in sfm. It could be that I'm using the wrong Kennametal for those applications as well, thus thhe drastic tool performance difference. 321ss and 347ss are the "meat and potato" material here and the Seco insert I'm testing does not hold up to the Kennametal (CNMG432MS 5510) as well. I'm waiting for the next worthy high temp alloy test subjects to come through and I will try the CP200P

Hey Jimmy check this link out I just found it.Looks good. Kennametal insert

That's funny. The article states that "hi-temp alloys are generally limited to 150-200 sfm" (which Jimmy said he runs them at w/ 5510's) and that these KC-5510 inserts "can be run at 300-400 sfm"...Jimmy, did you try 'em at THAT speed? lol, did they melt? I've only turned a few inconel parts, but I used Greenleaf whisker-reinforced ceramic, like Bushman, for roughing; Seco for finishing.

I machine (Integrex 400IV-ST)a variety of High Temp Alloys (Inconel, Monel, Titanium, Zirconium, Nickel, Renae 41, and more Hastelloy than I care to). We exclusively Kennametal 5525 Grade for OD and ID turning, grooving, and threading with excellent success.