surfacing hastelloy

[somename75]

So I have a job possibly that would require me to machine off around .08 in hastelloy, with a ball endmill. The surface that needs to be cut is about 8" x 20" or so. I was going to throw 1/2 ball endmills at this but was wondering if going around 160 sfm, and .002 per tooth would be a good place to start this quote from. I dont know how much benifit I will get from the chip thinning so I am scratching my head as to get a baseline on this. Also, from you guys that have worked with this stuff, what kind of tool life should i expect out of a varimill type tool?

 

Thanks much

[K2csq7]

Soooooooooooooo much of this depends on rigidity of your machine & workholding. <<< I can't say enough about that.

A literal night and day difference.

If you can surface for 20 mins with a ball end mill, you're doing REALLY good IMO.

Keep your expectations low.

[somename75]

shat, this is quickly becoming a no quote. Even with a .05 axial and .015 stepover, you still think it will suck that bad? Thanks by the way for the help

[mkd]

what about a ceramic insert tool.

we've all seen the youtube videos of cutting inconel dry at stupid high RPM....

[somename75]

that is something i might have to consider for this, who does the best work when it comes to ceramics? Sandvic?

[mkd]

i would ask the customer for a trial run before giving any hard quote.

 

be sure what you can do with your equipment......first

[K2csq7]

If you feel confident your machine & workholding will be "SOLID", I would not be afraid.

Can't win if ya don't play, right....

 

Maybe you can call a material distributer & pick up a small chunk to "play" with....

[T_MALENA]

If you try the ceramic route - try the Kennemetal ceramics. tried greenleaf, sandvik, keyocera & kennametal. The Kennametal worked best. I recorded a video where I had it cutting hardened Inco at 18k rpm & 200ipm feed. Also I pushed it to 30k rpm & 350ipm just to see what would happen. Tool was a 1.0 dia button style with 3 8mm dia ceramic inserts. Doc was .02 & radial width was .5 And a cold air gun.

Rigid setup!!

 

I dont have access to the FTP, is there another way to post a video for all to view?

[Rotary Ninja]

I have cut a lot of Hast X and K2csq7 is giving pretty good advice. Your tooling, no matter what you use is going to take a beating. Maybe rough with a bullnose with a .050" stepover leaving .010" then finish with the ballnose? If you can get the surface on an angle, to cut with your ballnose at about a 30 degree angle to the material you will be better off. This will get you away from the center of the endmill and give you better tool life and less breakage. The biggest endmill you can get away with will of course allow the biggest stepover.

[Matthew Hajicek - Singularity]

You could take most of the material with a high feed, then take the last few thou with a ball. I use Fraisa solid carbide 6mm, 4mm, and 3mm high feeds for roughing between closely spaced tapered ribs. I run the 3mm at 12000 RPM and 227 IPM, .0024 step down in hardened H13, leaving about .003" for finishing. They last several hours at that rate too.

[somename75]

thank you all very much for helping out a noob, Im gonna ask if they have a scrap one laying around for me to play with, they quite likely do

 

once again

 

thanks much

[CAM-mando]

I would talk to Greenleaf.

http://www.greenleaf..._-1_10103_10090

 

Also if using ball tools I think you should consider fixturing the part at a 15° or so incline relative to the spindle C/L.

[TK-32™]

If you try the ceramic route - try the Kennemetal ceramics. tried greenleaf, sandvik, keyocera & kennametal. The Kennametal worked best. I recorded a video where I had it cutting hardened Inco at 18k rpm & 200ipm feed. Also I pushed it to 30k rpm & 350ipm just to see what would happen. Tool was a 1.0 dia button style with 3 8mm dia ceramic inserts. Doc was .02 & radial width was .5 And a cold air gun.

Rigid setup!!

 

I dont have access to the FTP, is there another way to post a video for all to view?

 

youtube would be the easiest to share the video.

[Guest CNC Apps Guy 1]

Yeah that stuff beats the crap out of tools no matter what, so, go ceramic if you want to make some money on the job. Personally I like Kennametal stuff. I used the Kyon stuff for turning Stellite back in the day.

 

DO NOT shy away from it. If you guys can do this type of work, good things will come. You'll loose some hair along the way but it's so worth it. 99.99999999% of the shops out there will no bid it.

[Rotary Ninja]

Yeah that stuff beats the crap out of tools no matter what, so, go ceramic if you want to make some money on the job. Personally I like Kennametal stuff. I used the Kyon stuff for turning Stellite back in the day.

 

DO NOT shy away from it. If you guys can do this type of work, good things will come. You'll loose some hair along the way but it's so worth it. 99.99999999% of the shops out there will no bid it.

 

Where is the Mother Ship located? Because here in Indiana I have seen more work with Hast X, Inconel, Rene, Waspalloy, etc than I have anything else. Five out of the seven shops I have worked at specialized in exotic materials. Just curious because around here getting that kind of work is very competitive.

[Guest CNC Apps Guy 1]

The mother ship is residing in Southern California at the moment. 'Round these parts seems like if it's not Aluminum, most people no-bid it. Even Ti, a lot of shops shy away from which is ludicrous. Ti is like butter.

[Rotary Ninja]

Yeah, I don't know what kind of butter you use, but ours is a little softer here I'm thinkin'

 

Where I am at now aluminum is the norm too. Might as well be cutting Balsa Wood.

[Jeremy Herron@DBS Solutions™]

I prefer ntk for ceramics, but realize that you cannot finish mill with them, only rough to within about .040, You can finish turn with them all day, but I would not try to finish mill any surfaces especially if you have an FPI or post process metallurgical inspection.