turning a286 (~50Fe 25Ni 16Cr)

[bookwurm99]

at work we are machining some bolts out of a286 rod and we need to part them off of the rest of the rod. need speeds and feeds to use so we can speed things up. we are doing about 1000 of these fasteners (first time working with this material). we are currently turning the profile on both ends on cnc machines and doing the parting off on a manual lathe. the time that it takes to part off these has the profiler sitting around waiting for the bars to get parted off. i have already looked in machinery's handbook 27th ed. for a286 or anything similar to it in composition but have been unable to find anything close to it. want to be able to do the parting off on a cnc but don't have any idea what speeds and feeds to use for carbide TiN or TiAlN inserted part off tool with flood coolant. have asked people at work and at my cnc class but they don't have any idea where to start. we will also be threading these after the partoff. please help.

[bennett71]

Is it precipitation hardened also. This stuff is nasty & work hardens just by looking at it. I once had to cut 42 6" dia. slugs of this stuff & the best carbide band saw blades we could find only lasted for three parts. Then they had to be faced in the lathe & tool reps I had come in asked me what is this crap! The solution was ceramic inserts. These are expensive, but well worth it if you add tooling to the quote & do a lot of parts. We machined with no coolant as the key was to let the heat out with the chip. It was pretty scary watching red hot chips flying off it but it worked great. Maybe a tool rep will give you a sample insert to try

[little bubba]

Did a whole bunch of milling on A286 a while back. Ceramics where the only way we could move a lot of metal fast. Took our roughing time from 24minutes with cabide to 24seconds with ceramics. 11700 rpms with a 2" cutter, feeding between 200 and 250 ipm. It was like the 4th of july in the shop.

Other things I found milling it, is that uncoated carbide held up better than coated carbide, and it really likes that carbide to be sharp.

Look for speeds, feeds and tool geometries for inconel. Its fairly similar, just a bit less Ni. One of the trade names of A286 is Incoloy. No matter what you call it, its a miserable material to work with, especially if you aren't familiar with it.

[pepo]

Use the same feeds,speeds and tooling you would use for Kryptonite.

[bookwurm99]

Use the same feeds,speeds and tooling you would use for Kryptonite.

where can i find kryptonite at? i thought krypton was destroyed or something like that.

[pepo]

Didnt Gene Hackman have some?

[bookwurm99]

i'm talking about kryptonite in THIS world. don't think they'll have any at ebay or anything like that '(checks just in case)'. nothing yet. the closest thing, unbihexium, hasn't even been discovered yet. http://en.wikipedia.org/wiki/Unbihexium

[Les A W Harris]

at work we are machining some bolts out of a286 rod and we need to part them off of the rest of the rod. need speeds and feeds to use so we can speed things up. we are doing about 1000 of these fasteners (first time working with this material). we are currently turning the profile on both ends on cnc machines and doing the parting off on a manual lathe. the time that it takes to part off these has the profiler sitting around waiting for the bars to get parted off. i have already looked in machinery's handbook 27th ed. for a286 or anything similar to it in composition but have been unable to find anything close to it. want to be able to do the parting off on a cnc but don't have any idea what speeds and feeds to use for carbide TiN or TiAlN inserted part off tool with flood coolant. have asked people at work and at my cnc class but they don't have any idea where to start. we will also be threading these after the partoff. please help.

Material condition? solution treated, 180 to 230 Bhn. 25/95 ft/min, .002"/.004" per rev, tool material T-15, M41-M47, C-2 carbide.

Material condition Solution treated & aged, 250 to 320 Bhn. 20/80 ft/min,
.002"/.004" per rev, tool material T-15, M41-M47, C-2 carbide. That was back in the 1980's, basically start at the slow speed, heavy feed, lots of coolant, Try speeding up part at a time till it fails, then back off a tad. Since that ancient time carbide's and ceramics have come a long way, back then, a sharp, honed T-15 tool would beat carbide. How about your tool supplier, for a recomend?

Threading; Under 1", SoluionTreated, 3 to 12 ft/min, .010" 1st pass---.001" last pass, .002"/.004" per rev, tool material T-15, M41-M47. 1.0"--6.00" dia, 4 to 12 ft/min, others the same.
C-2 carbide. 65--85 ft/min.----80---95 ft/min.

Solution Treated & aged, under 1.00" 2 to 8 ft/min. 1.00"---6.00" 3 to 12 ft/min.
C-2 carbide. 45-70 ft/min,----50--75 ft/min.


Les H.

[stustev]

I think I would saw the parts to length at twice the length of one part plus the part off tool and .020. This would give you .010/part to finish face. You don't say what size the part is or what size the lathe is. With the parts short you would have no rpm limits like you would have with the bar. Chuck the blanks and do 1 part on the end of each blank, bore jaws and do the second part and then part them off.
Does your lathe have constant surface speed? You will need it. Sharp high speed steel part off tools will probably be the best. Keep them very short and very sharp and a high positive rake. You will need the constant surface speed to get the surface speed high enough when parting off. As the tool reaches the center the surface speed gets so slow and this material is so quick to work harden - you don't want ANY rubbing. You will need as much speed as your lathe will spin at the very end of the cut. Once you start, do not stop or hesitate in the cut.
Lots of coolant in this type of cut using HSS will be best. If you go to carbide or ceramic then I think dry would be best.
You will want as small a tit as possible on the end of the part. Pay very close attention to the center height of the part off tool. I would think from 0.0 to 0.003 in. above center would work the best.
Use the previous post's recommendations for speeds and feeds to start.
Sharp tools are the first requirement. As soon as the tool shows any sign of dullness you must change it or sharpen it. In a 1000 part run you will learn where you should change tools to prevent tool breakage. In one job I did it was so predictable that one part more would break the tool every time.
Please post the results.
Stuart

[victor-arcp]

My company recently accepted a job with machining A286 that has been harden. I will be running it on 2 Mori Sieki Duraturns. I think the parts are about .5-.750 in dia we will be doing ID skim pass of about .02 to bring these parts to size. I was wondering if there are any recommendations on speeds and feeds for this material. Any help would be appericated. Also recommendations on tools. Ceramics, Carbides, etc. Chances are we might be using either Sandvik boring bars or PH Horns not sure until I get the parts in this coming Tuesday.

[03clipse]

I have been running A286 for years. Long enough to get good at it.
Turning
Iscar WNMG 432-TF Grade IC907 Rough 400-500 SFM .012 FPR .12 DOC
Sandvik WNMG 432-QM grade 1105

Cut-off Manchester .125 wide M93 grade 150-200 SFM .003-.005 feed

First I would call my tool rep and get him in here. My Sandvik Rep worked with me untill 2:00 AM for a week. They are very good to deal with

[victor-arcp]

Are the Iscars for turning? What are you using for ID work?