[Waynno]

Maybe asked before, But any advise would be greatly appreciated

I have a turning job hogging down some 4.5 dia x 4 length Inconel alloy 625

All turning, and boring, no mill work, Finished part some sort of fitting

Based on past experience, many many years ago, this is some tough
stuff on tooling:tired:

I have an abundance of WNMG 432s on hand

Machine, Older Mori SL-3 workhorse , strong coolant pressure

Please Advise good start point depth per pass....feed & speed

Any reasonable suggestion will be applied and appreciated

Wayne

[Boots]

Hi Wayne,
It's been awhile sence I have worked with this material. Although it is tough and dense and very heavy it is not hard. You can dent it with your teeth so it isn't very hard. Your speeds and feeds will be determined by the rigidity and power of your machine and the tooling you select. I have found that Hand Ground HSS works well. Carbide NO WAY... The tooling needs to be flexiable and carbide is not and will break and or chip. Slow is the key word with moderate chip loads if your machine will take it. You might have to experiment with the tooling edge on weather to make it a positive rake or negative rake. Positive will get you under the metal surface and negative will scrape it off but requires more HP. Good luck.....

[christinandavid]

Hi,

Don't know much about turning, but milled this crap for years (presume turning is easier - hope I don't offend anyone). As stated previously, carbide seems to be too brittle for roughing - as soon as your edge goes, you've had it - material seems to resist machining as soon as it gets hot. Have had best luck with high cobalt content (M42) high speed steel (coated is preferable, but not essential). Slow speeds (10-20 metres per minute) but push your depth/feed to the limit - you really have to bully the stuff to get a decent tool life.

Have machined some 'rapid prototype' inconel pipe fittings for a hydrogen power station project - it was basically layered inconel weld. That stuff was really abrasive - carbide rippers, new one each pass, no other option. I decided to redefine my datum for t'other end and accidentally rapided the chuck onto the bit I had just finished (a hard-won .05mm roundness tolerance), completely obliterating tool and ripping my (hastily made) fixture apart.

Component remained unaffected.

DP

[Waynno]

Thanks guys, Im working though this stuff slowly. It does appear
carbide is not the ticket for lasting tool life. I am getting 3-6 passes
per corner before it kills them

Its ironic, this stuff defies logic, it has the appearance of a tough stainless, but
I set up a 1.75 drill, run spindle at 60rpm and push the feed to the machines limit

neither the drill or stock shows any sign of getting hot or wear. Chips come off shiny
and the high speed drill lasts

go figure

Wayne

[christinandavid]

Nice one,

Had a brief moment of disbelief, thought you were talking about a 1.75mm drill!

Looks like you have ample coolant, which is a big factor...just wait 'til something goes off and gets hot and you may see a different side to the material... (evil cackle fades into background like end of 'Thriller')

DP

[Delw]

Round ceramics and then finish with carbide

[PixMan]

Ceramics do work great, but you need SPEED and FEED to use them reliably. You also often need different tool holders (or at least, other hardware for them) because the inserts tend to be thicker. I know of shops using Valenite's new WS-500 grade at speeds of 800 to 1200 surface feet per minute. It's a whisker-reinforced ceramic similar to Greenleaf's WG300 grade.

Inconels are an extremely tough material that work-hardens in a flash if your tool goes dull or you don't "stay in the cut" (dwell.) If you think 625 is bad, just wait 'til you're cutting some heat-treated 718.

It is very possible to machine this successfully using carbide tooling. Try using a PVD TiAlN PVD-coated sub-micron grade, such as Valenite VP9605, at a starting rate of 140sfm. I've run it at up to 225sfm in really soft 625 with an upsharp insert edge. I used their CNMP432 M2 chipbreaker in that 9605 grade and it gave life in number of parts rather than number of passes. Using "ramping" cuts helps reduce the depth-of-cut notching that occurs.

Your cutting fluid can have a big impact too. The machines I ran that material on used a chlorinated cutting oil, which is an EP (extreme pressure) additive, not chlorine for anti-bacterial properties. When I tried semi-synthetic water-based coolants, tool life was halved.

Hope this helps.