Inco 625

[headhunter]

Hoping to get some help from somebody who has worked with this material before. I'm quoting a part out of Inco 625. I've never machined Inconel before, so I'm learning as I go. I have several holes to drill and tap, and ream, and a few counterbores to mill. Mostly in the 1/4" to 1/2" diameter range, but I do have a couple of holes that are .070 diameter X 2.1" deep. Whats a good starting point? HSS, or carbide? I'm guessing carbide. It's got a high nickel content, so I'm guessing work hardening is going to be a factor.

[K2csq7]

.070

I'd look into EDM...

 

Drilling inco is a PITA.... the successful window if feeds/speeds is small, carbide is a must... You should be able to mill it fairly easily, I would use an endmill (or 6 lol) to ramp the c'bores.

Workhardening as you predicted is a factor, you must push your endmill fast enough to get one flute past the previous... It's almost like the material "moves" out of the way of the cutting edge and scrapes the backside (relief grind) of the flute.

As with all superalloys, rigidity of machine & fixturing is paramount.

[mkd]

a buddy machines it daily. he swears by guhring carbide drills. no center needed just drill from solid.

he gets hundreds of holes per drill.

he just texted me his parameters: 50sfm @.0015 per rev.

1.5 times the diameter peck.

 

don't even think of running a tap in your CNC; thread mill only

[headhunter]

Great! thanks guys. I'll see what I can do with it.......

[Pilot Plant Supervisor]

I just had to drill 2MM holes 3.5" deep in Ti. I had the Guhring rep come in and we used a gun drill. I was impressed, 21 holes with one drill and you could hardly see any wear with 30X. That's 73.5" of Ti!!!. Anyway, the rep said he has had good luck with the gun drills in Nickel based alloys. Through spindle coolant 1000psi is a must for this to work though.

[Brando]

guhring series 5020, has 80mm flute, if you have about 750+psi thru spindle coolant it will work no problem, ive used them extensively in our horizontals, make sure you read the manual on how to use them its not at all like a regular drill

[Rotary Ninja]

Drilling 2.1" deep with a .070" drill isn't going to be a cakewalk with any drill. You'll need to keep an eye on the drills. There won't be much warning when a drill starts to wear and is embedded 2" deep into your part. We used to drill .020" holes in 718 Inconel Castings. The drills were so small the coolant pressure alone would break the drills if you had it up too high. The parts had I believe 80 holes. We ran two drills per part. You might get 10 parts just fine then break a drill off in the next three parts. So figure on replacing the drills before you think you need to to keep from scrapping parts. Cheaper to buy more drills than more Inco.

 

As far as milling, you'll want to take probably a .010" finish cut. Inconel doesn't like a light cut to be taken on it. I've tried to take .001" off a part, and after five .001" passes removing no material at all taking another .001" pass takes .004" LOL. It's because like K2csq7 said, it seems to push away and rub against the relief of the flute - wearing the hell out of your tool. A larger cut prevents this.