Machining Invar 36

[Kosta1234]

Hello everyone...

I need to know specs on machining Invar36.

The process is Milling

the job is 6metres x 3metres x 12 inches deep

If anyone knows what tools, speeds, feedrate, rake angles, depth of cut, best tooling for the job.

I would like to remove as much material as fast as possible.

If anyone can help me you can e-mail me at
kosta@ncprecisiontooling.com it would be much appreciated.

Thanks heaps

Kosta

[Kosta1234]

Hello everyone

I need to know specs on machining Invar36.

The process is Milling

the job is 6metres x 3metres x 12 inches deep

If anyone knows what tools, speeds, feedrate, rake angles, depth of cut, best tooling for the job.

I would like to remove as much material as fast as possible.

If anyone can help me you can e-mail me at
kosta@ncprecisiontooling.com it would be much appreciated.

Thanks heaps

Kosta

[Fish]

Hello Kosta,

That is one big piece of steel!! I know it is used when thermal stability is important. Invar doesn't expand as much as carbon steels when it gets hot. It has a pretty high nickel content which means it will work harden quickly if you don't have enough feed for the speed you are running. What machine are you working on? What RPM's, spindle taper and horsepower? I have worked on Ph stainless, but not Invar. I would bet that your local Iscar, Sandvik and Kennametal reps would have what you need. Try bringing them in with samples. It works here. If that doesn't work, let me know more about your machine and I can find out on my end.

Fish

Fish

[Kosta1234]

Hi Fish,

Just in reply to your response, the machine is a 5 axis machine, MAS BT50 spindle, loads and loads of power and plenty of feedrate available.

I have read up on the internet about invar and it seems to be very soft but very abraisive. A Nickel contenet of 36% dosent help either.

Any information about trying to machine this material is very much appreciated.

Regards

Kosta

[little bubba]

To me, high nickel content says ceramic. Here was my situation, machining A286 (between 24 and 36% nickel) somewhat similar to inconel(one of the trade names is incoloy) annealed to a 13C. The sandvik rep turned us on to ceramics, kennametal cutter and sandvik inserts. Cool, 100-130 sfm to 700-3000. Bought the kennametal cutter, read all the stuff on the internet, check out Kennametals web site, and MMS online did a VERY informative article in 1999, just search for ceramic, this was my saving grace. Anyway, we received our cutter and inserts, (RPGs) I tried all sorts of feeds and speeds that were recommended, and failed miserabley, cracked burnt inserts etc... Of course my logic said slow it down, lower feed, WRONG. Since it was soft, I needed more speed, 2" cutter, 12000 rpm, 6300 sfm, or 1nautical mile per minute. Worked great except you could see the color change(sparks that is) when it started a new cut. Double the depth of cut, wow, I just increased my tool life 4 fold, except the insert edges were breaking down at the edge of the cut, and still it was nasty starting a new cut. Back to the MMS article. 1)ramp, 2)keep the heat up. Ok, sat down and worked out a nice tool path that keeps the cutter in that part for the whole roughing cycle. . Had some problems with a little metal build up toward the end of the cycle, but I decided not to take out that last little bit. Roughing time of 17seconds, down from 24 minutes with carbide roughers, 2-3 parts per index, 8 indexes per insert, 6300 sfm 188-240ipm depending on depth of cut (almost constantly ramping) and radial depth. The biggest downfall is bad surface finish since the material is so soft, not a problem for what I'm working on, the other is a bit of buildup on the inserts, I just take them to a belt sander.
Honestly the Kennametal rep and their techs were less than helpful with our soft high nickel problem. It took the sandvik rep to sell us a Kennametal cutter, (the kennametal rep got his 'suggestion' back in pieces).
With the soft metal I would probably have had better luck with the angled insert cutters instead of the 'n' series 0deg. However the tradeoff would be the 'N' series is double sided (double the cutting edges), whereas the better shear insert is not (would that mean double plus tool life,????) BTW these are all 1/2" round inserts, running dry.


My suggestions on conventional cutting, (assuming that your material soft and high nickel behave similarly) is Carbide, M42 does OK in a bigger rougher (<50sfm)but useless otherwise. I've been using carbide roughers, half inchers, small radial, .13". .200 axial, 100sfm, .002-.004 per tooth depending on the corners it has to take, the tool life averages about 120 minutes, I usually pull them at 100 and grind a fresh radius on the end and get another 100 out of them. Smaller endmills are still bothering me, 400+ minutes on a 1/4 rougher, and still going strong. 1/8 finisher, 500+ minutes still going both running 90-100sfm. However I have to change my 1/4 finisher after about 25 minutes of run time, (starts throwing big burs). Here is the weird thing, I was running the roughers at 70sfm, I was being cautious after my initial failure at 200 and then 130sfm. I then worked up to 100sfm and increased my tool life time by about 40%, with the same feeds, really weird????.

Drilling, SLOW, CARBIDE and LOTS OF COOLANT(small peck steps). <.100" holes 5Xdia, .0003 per rev, .030 pecks, 30-40sfm. 1/4" holes, I've been fine with .003 per rev, over that I was breaking drills.

I hope this helps, I know the situation is a little bit different, but the soft hight nickel expierience might help you out a bit, none of the tooling manufacurers were much of a help, except for conventional milling, HIGH + HIGH +, its just like aluminum 'cept different. The valenite V590 cutters were great, 150sfm, .006 per tooth ( we went from 12 to 3 minutes on one roughing op and saved $1.50 in tooling) except if the tiniest little thing went wrong, you lost the cutter, no beef behind them, we were changing the inserts at 30min, but if something wasn't seated just right or (as I suspect) an insert wasn't up to snuff, you lost the whole thing, no sound difference, no squeel, nothing and the body of the cutter just wasted away, I guess they are made from the same thing as the interior door handles on mid '70s mustangs, somewere between crunched up tinfoil and mercury.