Anybody have experience HSM super alloys? looking at a production job made of Invar ( FeNi36 ) never cut this alloy but have cut other alloys with mixed results looking to take a new/better approach on this job. need to do both turning and milling. The part is small made of 1.750 rd stock. The plan is to bar feed in Samsung lathe then mill in Doosan DMN both new with in the last year.
4 Likes
I’d say check with Titan, he’s done quite a bit of crazy materials, see if he’s done this one…
3 Likes
Let’s tag him and see what he has to say. @Titan what are your thoughts?
3 Likes
I’m hoping to get input from anybody who has experience with this good or bad. Titans input would be great but if somebody else has knowledge on this I’ll listen to them also. Thanks
5 Likes
I’d say use Sandvick prime turning tools, Inventor and Fusion have been undated for it, and adaptive bothways using Imco endmills. If you need recommendations, they are good about recommending the right endmill for the material, and may send you some tools to try out…
3 Likes
You may have already researched and found this, In case you had not found this information, here is something to start from. http://www.invaralloy.com/invar-machining.php
3 Likes
Invar is very gummy. The various amounts of iron nickel are the killer… so RIGIDITY is going to be your best friend. Is this a production job for the shop? Short run? Prototype? I’ve ran a ton of HRSA over my career. I find when I’m in doubt I actually run a destiny variable 6 or 7. Flute raptor I wanna call it. Reason I’m doin that is because you have to take a chip load!! Don’t run the cutter too easy and “rub” the flutes. Chip loads will be small. Less than a thou. More flutes will help also because the SFM across the workpiece will be slower also. Think 316L. In my milling experience light step overs of less than 8% of the dia. Should keep you out of trouble. Also! Get that damn chip OUT!!! Whatever it takes flood coolant. Thru tool if you get fancy endmills from helical. Or air blast never tried that one tho.
As far as turning. I’ve hade probably the best success with kenametal. I saw prime turning as a suggestion, if you have A RIGID set up go for it. If you can program for it and understand the cost and concepts. If you’re not gonna invest. Standard turning methods work. Check your cutters SFM start on the low small chip load. Check the inserts for odd wear. If you’re not seeing any. Step up the machine cutting parameters until you achieve a chip to chip time your comfortable with that maintains your customers tolerance.
If you have any other questions just ask! I’ve been doin work for GE and Honeywell FM&T for 11 years now. Solid 85-90% HRSA. Prototype and short run.
4 Likes
we machine it in annealled state, about ~160 BHN hardness. CNC CookBook’s G-Wizard Feed & Speed Calculator will have parameters for milling, drilling, turning, boring, etc. G-Wizard will give you feed & speed, plus tool deflection values for different DOC and or WOC. Cutting SFM is low, around 180 SFM with carbide tooling. Monitoring tool wear is a must. Invar36 likes TiCN / TiAIN coated tools.
Tom www.amsmotomachine.com
2 Likes
Interesting… Do you anneal the material yourself? Usually Invar is annealed to relived any “cold work stresses”.
Also what applications are you using Invar for on a motorcycle?
3 Likes
it is supplied to us in the anneal state. I own 2 machine shops - one specializes in hi-performance engine components such as 5-axis CNC ported cylinder heads, CNC diamond honed cylinders, etc mostly for high end import engines, and Harley Davidson motorcycles. My other machine shop does prototyping and small batch industrial work. A lot of simultaneous CNC 4 axis mixed with the normal 3 axis work; plus CNC lathe ops. Jobs range form oil & gas industry to aviation…although this week’s project is manufacturing 20 hot-rod throttle bodies for Dodge Hemi. Invar is similar to Inconel, which we also machine; they both have very low coefficient of thermal expansion. The Invar we machine is typically for laser/optical components. The inconel components we machine is typically for a German based company that manufactures large DMLS 3D metal printing machines. Tom www.automotivemachine.com
2 Likes
So. I call BS. Invar is NOT like Inconel at all. Invar is Iron and Nickel based. While Inconel is Nickel Chromium! They cut totally different. I know I’ve handle Inco 624, 718. This last week actually! Made some hubs with an internal spline cut by wire. It’s not easy stuff to get thru like Invar. Invar is way closer to 316L stainless. Invar has better CTE (thermal expansion) than 300series stainless.
Surface speeds and chip loads are totally different between Inconel and Invar…
2 Likes
Thanks for all the Input I love that one can ask a question like this and get the responses we got. Not everybody is going to agree but even then the banter seems more friendly then in other places. We have talked to our tools reps ( got some free samples coming ) seems like with the right tooling and machines this shouldn’t be that big a deal of course you never know until you have actually machined it in your machines. This project is still a month or so out before we do first article I’ll give you a up date on how it went when we get that far. Wish I could be more active on hear but like most days I got a lathe to run and another to set-up back out to the shop BOOM!!
3 Likes
Marcus, take a chill pill. I was only referring to Invar & Inconel having releatively low coefficients of thermal expansion and useful in high temp app. Invar has one of the lowest Thermal Coeff. Re-read my reply - I never implied they machine the same… There’s no need for your to rudely “call BS” to epxpress your obvious experience with Invar or Inconel. The forum should be a place to share your experience, as well as mine with out the need to inject inflammatory “mine is bigger than yours” language 
I’ve been successfully and profitably machining Inconel, Invar and 316L SS for many years, and was only sharing a bit my own experience, however if you still feel it is necessary to “call BS” and attack others so that you can boast of your own knowledge, then I’ll be glad to leave the forum. I only came here to help folks - not to be treated rudely by some one such as yourself who is rather immaturely quick to inject inflammatory language. Generally, when I have a difference of opinion with a fellow forum member, I respectfully ask for further clarification - who knows? I may actually learn from them, rather than insult them. As an example, I’ve already learned many things about you … and your experience. Thanks for sharing.
2 Likes
Scott, in addition to G-Wizard Calculator, this site may prove helpful:
www.hightempmetals.com/techdata/hitempInvar36data.php
respects, Tom-AMS
2 Likes
@MarcusMadrid @Tom-AMS
Lets please keep it on course. I believe both of you have some valuable knowledge and wisdom that I would love to learn more about. Both of you are a valuable resource. And let’s not let a little misunderstanding ruin an awesome post. I’m very grateful for your positive input but let’s keep it positive.
Your fellow Machinist,
Travis Sherwood
3 Likes
Thank you …I agree. This is a great place for gaining / sharing machining info
2 Likes
I am so sorry for the delay, I am posting below.
3 Likes
Thanks for holding it down, I didn’t see this and just received a text to look at it. Posting below
3 Likes
@ScottCarpenter @MarcusMadrid @Tom-AMS
Hey, sorry guys for the delay. I missed this and then just got texted from one of my guys saying the thread was getting a little out of hand… all good. We are machinists and definitely can get carried away… Truthfully, I have done a little INVAR36 but not much. 36 is the percentage of Nickel which is hard, but it also has Iron, which makes it easier to Machine than inconel.
Now, Inconel, I do have a ton of experience. Inconel is Nickel based with Chromium… which makes it Hard… Truth is, sometimes harder is actually better, since it breaks a chip better than gummy material. Kind of like 6061 AL is way easier to Machine than 7050 AL… because 7050 is Gummy and doesn’t break a good chip.
Much of this has already been discussed above… I have always challenged myself, and learned early on, that their is always a tool for the job. In this specific case, I would reach out to Kennametal and ask for their aces… and get them to guarantee some tools…
As far as Machining HSM,
It’s going to be tough but you definitely can go faster than what the Machinist handbook says… take lighter cuts with an endmills like the HARVI 3.
Maybe 5%
But go full depth… maybe 2 X Dia…
Maybe 175 SFM and .003 - .004 ITP
This is actually slower than I go in inconel 625 but is still much faster than others ask…
The chip is thinner, which allows it to break easier…
From there just play with the feeds and move forward. Again, I don’t do a lot of INVAR36 but know a little and I think this is pretty safe. Tell your Kennametal Rep I suggested it and if you run into trouble, I am sure they will give you a free tool maybe…
I run Inconel all day everyday and the HARVI3 kills it…
In Titanium we are actually at 400-600 SFM at a .0047 - .0053 IPT
As far as Turning, it’s a little closer to the recommended but you can still get pretty creative. Talk to the reps and ask them to guarantee some inserts…
Good Luck!!!
5 Likes
My bad for my attitude guys. @Titan @Tom-AMS @Rumpelstiltskin
I’m just very passionate. 
Good luck with job!!
3 Likes