What's new
What's new

Inconel 600 Feed and Speed help

yoke

Hot Rolled
Joined
Sep 26, 2013
Location
PA
I am quoting a job that requires 18 cubic inches of material to be removed from a pocket with several posts.

I am having some trouble finding conclusive information about Inconel 600.

INCONEL® alloy 600 (UNS N06600) Ni 76.0, Cr 15.5, Fe 8.0 Description

The above link has sfm at 125 which appears to be higher than some other places I have looked. the same link has .007 per tooth feed.

I know Inconel has a tendency to work harden so it makes sense to take a healthy cut but that seems excessive.

I plan to use Imachining on this part. I was planning on using .5in 5 flt AlCrN coated cutter from Garr.


Are these numbers way off or should I trust them?
 
I don't have an answer specifically to your question but maybe this will give you some direction. Almost all my experience with the super alloys is on lathes with a little mill work and some with twin spindles and driven tools.
I've been turning Iconel 600 and Hastloy C-276 since the late 90s and added 625 and 825 to the bunch about 8 years ago. Of those alloys, 600 is easiest on the tools and could run faster, but also had the most tendency to tear (mostly with reamers and single point threading). My operators call it inky stinky.

For a given coolant fed carbide drill I would run the following parameters for different materials:
316SS - 200 sfm, .012-.014 feed multiplier (drill diameter X feed multiplier = IPR feed)
Inc 600 - 100-120 sfm, .009-.01 feed multiplier
Inc 625 and Hast C - 70-90 sfm, .007-.009 feed multiplier

I know it didn't answer your question sepcifically, but maybe was enough to give you something to relate to.
 
I was wondering how to answer this as well Mr BradleyK, You took the words right out of my mouth! Seriously tho , I think that is a great answer , We machine a lot of Inconel here as well , treat it like you would 316 or even a little tougher 321SS . Just my opinion (for what its worth ). Ed Good luck Yoke , also alot of times when I quote Inco , I just double the price , and still haven't got rich.
 
I would go with 100 sfm, and a super sharp cutting edge. Depending on your part geometry, hsm may hurt more than help. This stuff will work harden just by looking at it too much.
 
I ran the job and it went better than I could have hoped.

I approached the 18 cubic inch pocket by drilling a start hole .01 shy of the bottom. I programmed with Imachining.

230 SFM (calculated by the software, Tool had 150 SFM entered)
1800 RPM
31 IPM
Max cutting angle of 34 degrees
Min cutting angle 16.7
Chip thickness of .0025
DOC .625

Cutter was a .5in .03 corner radius 4 flute VRX from Garr.
finished with a square end .5 4 flute VRX.
Both cutters look like they could make more parts.
The finish on this part is stellar. I hope to see more of it because the money is certainly there.
Pocket run time around 55 minutes.

I wish I could post pictures for you guys to see as its a pretty neat part but this customer wouldn't like that very much
 
Thanks for posting with some real numbers and experience. I often go through the frustrations of trying to find good info on cutting the superalloys. Problem is when somebody figures out what really works, they usually keep it to themselves :)
 








 
Back
Top