Incoloy a286

[Ballnose Bill]

Hey guys we just got a fairly large job turning 10" diameter approximately 10" long a286 Incoloy. I have done some searching and from what I am seeing it looks like this stuff should be roughed in right around (200-300 SFM ) with a .100" doc and .01"IPR. As for finishing I am guessing (400-600 SFM) with .01" doc and .0025"IPR we may have to slow down a bit to achieve the 16 finish on a diameter. The tolerances are +/-.001" on the bores which I don't see a problem with but it does have some flatness and parallelism requirements within .0005"these are a bit; if not alarming, at least they do stand out. My guess at this time is we will have to fixture and grind at least one of these surfaces to meet the requirements. I guess what I am asking here is, there doesn't seem to be many threads regarding this stuff, does anyone here have experience that they would like to share with me? Also I am definitely curious as to whether roughing it down with ceramic would be worthwhile. I definitely will call on my tooling supplier but right now I am just tiring to draw as much knowledge as I can and this place definitely has a wealth of it. Thanks in advance.

[mkd]

don't have any experience with ceramic, but carbide should do well for milling and turning.

 

tried to surface grind a dog bone part years ago. tendency to curl overpowered double sided tape and wheel turned it brown.

no bueno...

[djstedman]

I have done milling in A286 before.. never had the chance to try turning it, its a tough material thats about halfway between cutting titanium and cutting Inconel, totally able to be cut with coated carbide though.. its very strong stuff .. need to have as rigid of tools and setup as possible, also had a LOT better luck using roughers on this stuff than finishers for some reason.. breaking the chips increased tool life and feedrates..

 

I was cutting right around 225 SFM and it worked fairly well.. main issues we had was trying to hold perpendicularity side milling our mills would go to hell and start tapering fairly quickly..

 

Our parts were pretty small that we were doing, but from what I recall they stayed fairly stable with minimal movement from material removal..

[DODGERFAN]

Last time I worked with A286 was about 15 years ago, it was on a chucker.

Drilling a 1/2 inch hole, you would need to put ALL of your muscle into it.

Tough stuff.

[John_F_44]

I like to use a semi finisher for this type of material and surface requirements. The semi finisher would leave about .002 per side for the final finish tool. Would use a SFM of around 550 and a feedrate around .0015 IPR for final finish pass which will get a 16 finish or better. The use of a semi finish tool extends tool life on the finisher and makes close tolerances repeat extremely well. I run the semi finish tool rather quickly at 550 SFM with anywhere from a .008-.01 feedrate. This will also help keep flatness and paralleism within .0005.