Inconel 100

[cmichaud]

Hi All

We're machining (or trying to) some Inconel 100. Does anyone have any hints/tips? From what we've learned so far we have to turn it at about half of what we would run inco718. We're running the inco 100 at 55sfm .009/rev .07 doc. Using Sandvik button tools H13A grade. We've tried a bunch of other Sandvik and Iscar stuff and nothing is helping. I was hoping that we could go faster but it may just be the nature of the beast.

 

Any help or advice would be greatly appreciated.

 

TIA,

Craig

[Slick]

Do you have VoluMill? If not, it may be a good time to speak with your reseller.

We have been experimenting with "Highspeed" toolpaths but are still running in to cutter life issues. We have been up to 200 SFM in inconel with smaller cutters, 5/8" and lower. But if you haven't experimented with it I would advise to sticking with what you know without a rep supporting you.

 

On the programming side, make sure your entry and exits are not banging the cutter on corners (if you've watch volumill online you can see how it removes the corners of material). This is huge for tool life you will want to draw these in most likely.

[cmichaud]

Hi Slick,

 

We do not have Volumill, but thanks for the advice. We've been working with a few tooling reps and not many people seem to have cut this stuff. Most people are saying try this and good luck haha.

 

The part is a turbine blisk for the hot section of an engine so it's mostly 5-axis simultaneous (sp?) machining. Turning it has been bad enough, I'm almost scared to see what milling it will be like.

[Slick]

Keep an eye on this thread, I have someone looking in to it, if I hear anything more I will let you know.

[Slick]

Here are some proven numbers for production:

 

Roughed at 80 s.f. with .0031” chipload using an .625” dia., 5 flute, .06 bull, .875 loc stubbed in a stub holder. Depth of cut was .450” with a .200” step over.

[Teh Bear without Brains kinda idiot]

look toward Hanita Varimill .

especially new type Varimill II or supervarimill do not remember the exact name

Good for this stuff .

Tried it on monel was good

[cmichaud]

Thank you all for your suggestions, I'll be giving them a go on Friday when the job hits the mill.

 

I'll be sure to post what results I get with any tools we try.

[neurosis]

Have you looked in to high speed roughing using ceramics? I am not familiar with Inconel 100 but have seen 718 roughed with ceramics and it is simply freaky to watch. It turns the Inconel to powder and looks like a flame thrower.

 

 

[Superman]

We got limited success with "GREENLEAF" ceramics in Inconel718

Turning

RNGA-43 CS1500 Ft/min, 0.0035"/tooth, 0.02" DOC

CNGN453 T7A--CS1500 Ft/min, 0.0018"/tooth, 0.02" DOC

 

Milling

cutter = WSRP-60001.2 -3 flute

tips = RPGN-32 -S8000 F0.0012"/tooth, 0.04" DOC

cutter = WSSP-70001.2 -2 flute

tips = SPGN322 -S8000 F0.0012"/tooth ( take out radius of 3/8" tip )

 

Note--

-no heavy cutting in corners

-tip must not notch ( sometimes means you have to speed up & get it hotter at the cutting edge )

-chipping means you are close

-tool life is close to 5 minutes--get as much done in that 5 minutes

 

Get a rep in- these tips are not cheap

[cmichaud]

Thanks for all of the info guys. Am I right in assuming that you can only rough with ceramics and not finish because of the high heat? We haven't really used ceramics milling or turning but if we get more of this Inco 100 it looks like we won't have a choice.

 

Thank you to everyone for their suggestions.

[Goldorak]

for the end-mill , Niagara is by far the best

 

we cut a LOT of inconel here and niagara stabilizer mill always beats the other brand

 

ez Hanita vari mill can produce 4 part , the stabilizer will produce 50 part with a faster cycle time...

 

180SFM 10% WOC 30 to 40IPM full depth in dynamic mill

[Goldorak]

i forgot to mention that your milling setup must be as rigid as possible

 

we archived this speed setting on an Okuma MC-V4020 with a cat-50 spindle, and the end mill is mount as short as possible

[Teh Bear without Brains kinda idiot]

looks like you use Hanita Varimill not in proper way

I use it with lower feeds and heavier cuts

[Goldorak]

i had to admit that i don't do extensive test with the Hanita varimill, since our niagara distributor is only 2mi from here and he offers excellent prices ans service

 

 

but i followed the manufacturer recommendations for both end mill for SFM , i just played with the WOC

[j.nguyen]

Guessing the blade is a forging and volumill would be better suited for a block. The ceramics would beat the hell out of your machine. Conventional though the skin will save on tool life. The Hanita Varimills have worked great for me but have never used the stabilizer? Guessing you nest a bunch of them on a fixture to turn them and now milling the ends?

 

Jamey

X4

[cmichaud]

Actually all the blades are already attached to the hub. It's a one piece turbine, about 11" in Dia. We have had some luck with the Stabilizers in different materials so we'll probably give those a go the first time around.

[calnet42]

I can't find Inconel 100, but I did find IN-100

in the Pratt book, it is AMS 5397.

9.5%cr,15.0%co,.17%C,4.75%ti,5.5%al,3.0%mo.

machinability of 8%

 

(inco 718 has machinability of 16%)

 

sounds like you are in thek for feeds+speeds..

[cmichaud]

That would make sense, the cusomter told us it was an Inconel casting but the material on the print says IN-100. Thanks for the info, looks like it'll be a lot of tools and time.

 

Is the Pratt book available online? It seems like whenever there is a materials question the Pratt book saves the day.

 

Thanks for your help!

[calnet42]

I've never seen it online.

I Got mine from my Dad, who worked there for >20 years...