Inconel problem

[Chap54]

I have been given the task of trying to make this inconel bracket. It's current state is that it has been EDM'd to shape leaving .010" per side to remove the recast layer. The part is roughly 6" x 3", heat treated inco  to about 45 rc. The part is .170" thick, with a bend about 2 " in on the long end at approx. 48 deg. I'm trying to cut about .010" off the bigger surface, and everything I try is just warping the part. I attached a file so you can see it. It was not my idea to leave the .01 stock all over, but it is proving to be a nightmare. The change to the process was made by an office manager with no consideration to what would follow. It's a long story but apparently I drew the short straw.............

 

So far I've been trying to hold it in a vise, using different face mills, 1.25", 2.0", and 3.0".  Any ideas would be appreciated.

51 m for forum.mcx-9

[TerryT]

what cs number are you using to figure out your feed rate with. 70's?

[AMCNitro]

Inconnel needs to be machined slow slow slow slow!  It work hardens very quickly.  Which tools are you using? Speeds and feeds?  Ive had best results with Kennametal Harvii 2, Fullertons and Walters also work well.

[Prodoggg]

You might want to try using a smaller dia. solid carbide end mill, 1/2" or so. Try running it at 100 to 140 surface feet feeding at about .002 per tooth. a small corner radius up to .015" will keep the corner from breaking down too quickly. Don't go with too large of a radius or heat may build up and cause warping and /or work hardening. We have had good luck with this approach.

[crazy^millman]

Get a hold of your ISCAR rep and ask for the 19 flute 3/4 endmill. 5% step over a .002 per tooth feed rate. 130 sfm and have a nice day.

 

Waterjet the Shape before even starting after I looked at the file.

[TerryT]

we use M.A.Ford endmills. They work great, usually able to keep cost under five bucks per endmill per part.

[AMCNitro]

Get a hold of your ISCAR rep and ask for the 19 flute 3/4 endmill. 5% step over a .002 per tooth feed rate. 130 sfm and have a nice day.

 

Waterjet the Shape before even starting after I looked at the file.

http://iscar.com/eCatalog/Family.aspx?fnum=3647&mapp=IT&app=216&GFSTYP=M&cat=4500168

 

That one? Interesting...

[jlw™]

Yes, that one is the shiznit. I have ran it in waspaloy and hastaloy as well.

 

Zcarb performs well too.

[Chap54]

Thanks for the input. Ron, the shape is EDM'd out leaving .010 stock all over. I'll get a hold of Iscar, and try some smaller tools as well.

 

Thanks.

[htm01]

should have wired it right to size

[Chap54]

should have wired it right to size

Well that is kind of how we ended up where I am now. The part used to be wired right to size, however that was without the customers knowledge. It worked well, but EDM was not allowed. They did it anyway ( this is before my time here) When the order came in again, the new Op Manager said we had to leave .010 because of the recast layer. All of this happened without any input from me. When the parts came back from EDM with .010 stock all over, it became my problem. Any process and fixtures we had basically went out the window.

[bd41612]

Well that is kind of how we ended up where I am now. The part used to be wired right to size, however that was without the customers knowledge. It worked well, but EDM was not allowed. They did it anyway ( this is before my time here) When the order came in again, the new Op Manager said we had to leave .010 because of the recast layer. All of this happened without any input from me. When the parts came back from EDM with .010 stock all over, it became my problem. Any process and fixtures we had basically went out the window.

 

That's why they get the big bucks.  They get you to work harder.  The more they see you struggle, the more they think they are getting the most out you.

[Chap54]

Thanks for all the input. Tried a dynamic path with a 12% stepover using a 1/2" endmill with a variable helix. So far it is working very well.

[Matthew Hajicek - Singularity]

You ever feel like you're Solidworks trying to find the solution to an overdefined sketch?

[MBuck]

Inconel is pretty thermally stable, isn't it?

Are they that tight of tolerance that heat treating is required prior to machining?

 

At the old job shop I was at, we made these Stainless steel parts about 2"x2" that were basically a hog out, that had some small (.0781) intersecting bores.

The owner used to get the cut stock blocks heat treated prior to machining, just because that's the way they had always done it.

 

I had a hunch one day and ran an untreated part and oversized one of the holes to ID it, then sent it in with the next batch of stock to be heat treated.

 

Owner got pissed when he found out that I did that, but after we inspected my part, we started heat treating post maching ops.

 

?

[AMCNitro]

Inconel is pretty thermally stable, isn't it?

Are they that tight of tolerance that heat treating is required prior to machining?

 

At the old job shop I was at, we made these Stainless steel parts about 2"x2" that were basically a hog out, that had some small (.0781) intersecting bores.

The owner used to get the cut stock blocks heat treated prior to machining, just because that's the way they had always done it.

 

I had a hunch one day and ran an untreated part and oversized one of the holes to ID it, then sent it in with the next batch of stock to be heat treated.

 

Owner got pissed when he found out that I did that, but after we inspected my part, we started heat treating post maching ops.

 

?

In my experience SS is nicer to machine AFTER its been heat treated, specially the precipitation heat treated ones.

[craigkalisch]

I know its kind of late in the Game but for Inconel try using 5 flute endmills for Inconel and SLOW!!! the Nickel gets gummy but not like Aluminum and is what beats up your tool and warps your part...