Help? They want to give me Inconnel 718.

[Chad 73]

Thier looking at taking a one piece inconnel job. Looking through old posts i see water solubles are no help and low speed seems to be the starting point. I have a high speed mikron that has an oil mist, Is that enough? The other option is a weak a$$ mitsubishi with the water sol. I'm thinking about 700 RPM at 4.2 IPM with a data flute or maybe OSG Carbide. Will rough with a 1/2 but half to finish with 1/4 inch ball endmill. How does this sound to those that cut this stuff? I've got a feeling this will cost more than they quoted it for. Please help.

[Thee Dragracer1951]

I believe inconnel is cut at close to 35sfm. That would be 267rpm for your 1/2" rougher

You're WAY too fast...

[john316]

.

 

I'm with dragracer on this one. You haven't said if it's hardened or anealed, but you will need to run it slower than what you have. The configuration of the part will make a difference too. Inconel has a tendency to warp if it has a flat shape to it. If you only have one part it is better to err on the side of caution than to go too fast and scrap the part.

 

.

[Chad 73]

I believe the part is anealed and did consider running the 1/2 slower Guess i forgot that part. The part is actually cylindrical and hollow. Will be doing 4 axis work on it. I'm considering filling the center with some aluminum to take out the vibration from being hollow too.

[Storkman]

Good luck, it is nasty. Keeps the speeds down with a decent chip.

[john316]

.

 

What's your diameter and wall thickness.

 

.

[?Mark]

With a good brand of carbide em you want to go between 75 and 90 sfm in inconel 718 and about .0015 ipt for a 1/2 dia.

 

hth

[kccadcam]

We've had GREAT success running Mitsubishi

High Feed Mills in roughing 718 Inconel.

Mitsubishi AJXU12R0204 - 2 inch dia.

running 250 RPM, 30 IPM, .030 DOC

Excellent insert life....

[Chad 73]

Part is about 3-1/2 diameter with a wall thickness of 7/16. I'm only milling 1/4 deep though not through.

[kinglouie V]

roughing with cobalt "corn cobb" roughers preferred from my perspective. no light chip load.

[terry5357]

quote:

---

I've got a feeling this will cost more than they quoted it for.

---

Isn't that always the case, what chaps my butt the most though is when the owner quotes the job with some hairbrained scheme that wouldn't work in a good dream, When they come and tell you what they had in mind, its always some stupid plan that makes you think "man were you on crack when you took this job?"

And then after they realized they underquoted BIG TIME they expect the programmer to bail them out, and when you can't work a miracle, its the programmers fault the company is losing money on that job. Yes I am a bit bitter about that particular senario..........and what makes it worse is they come and ask you what would be a good strategy and when you tell them, you get the "yea man that will work", then when the job gets quoted its like they never even mentioned to you. Thats the kind of suff that makes me HATE my job at times...............Good lick Buddy

[Tom L]

Chad,

I have to wonder if we are serving the same customer. We just ran cylindrical and hollow

718 Inconel parts. Also 4th axis rotary. Ours are 6” dia. We made a steel arbor for the part to slip fit.

Used a nut on the end and also used the tailstock. We used 3/4" Guhring Firex coated rougher.

 

Mark is real close to where we ended up, we ran 100 sfm @ .0013 cpt with .235 doc.

Water soluble coolant was not a problem. I went the route of the ball mill to re-create

An O.D. but it proved to be very time consuming. Tolerances allowed me to use a standard 3/8”

Carbide endmill doing a 3D contour with .100 stepover.

 

hth