ceramic milling diagnostics

[crabbass]

I am milling some Nimonic 263 parts.(High Temp Alloy, 49% nickel, 13%cobalt, etc.) Kennametal sells face mills and end mills with .5" round ceramic inserts in two different grades. I bought one of their 2" facemills with 3 negative flutes/inserts (for facing) and a 1.25" endmill with 3 positive flutes/inserts for roughing the walls of the part. If I could get these to work I could save hours of cutting time on each part. I used their starting guidelines for cutting speed and feed, depth of cut, converted feed to compensate for chip thinning, etc. I cannot get them to last!! not even for one part!! I have deviated the speed, feed, depth of cut in every way I can think of. (high feed, high speed, small cut) then (high feed, slower speed, small cut) etc, etc, etc. Unlike carbide, The visual wear on the insert does not change, It appears to have serious depth of cut notching, chips, edge buildup, and flank wear no matter what cutting paramaters are used. I am running dry (as recomended) with continuous air blast to help evacuate the chips (flames). Is there anyone out there using these products with success? Am I asking too much from my 20hp 40 taper machine at 7500 max rpm? I have the part fixtured verry rigidly to a solid plate mounted direct to the machines table.

[Superman]

Sounds like you have your work cut out for yourself

We are also going thru the same situation with Inconel 718
and found reasonable results using GEENLEAF tools for a mill / turn component

Sorry we're metric but currently have cutting speeds around the 600-750 m/min range, DOC approx 1mm, feed around the 0.09mm per tooth
the 0.5" round tips are giving the best results so far

All tips don't tend to last long , everything seems around the 3-5 minutes usage, so the more you

Every consideration to having the shortest tooling, any vibration is a no-no, so consider the tip "stuffed" if the occurs

It will be a long job, but look a Greenleaf technical data - it's the best info for the machinists I've seen so far.

[crabbass]

Once This is dialed in, if I can only expect 5 minutes of tool life, it would not be acceptable at all. Some operations are over an hour, estimated time with ceramic is about 20minutes (fairly large part 24" x 14" x 2" tall roughly) The carbide I use for roughing this job still looks fair after the entire cycle is finished. I havnt looked at the greenlee stuff yet, but your numbers are right where I tried starting, I cant go much faster (2400 fpm / 748m-min MAX on the 1.25" cutter). I still have a hard time understanding the principal of the ceramics. Kennametal said it "plasticises the material" It doesn't "cut" but rather "melts it and throws it to the side". Is depth of cut a large heat generating factor here? The first few impacts the cutters make when entering the material are cold, should a decreased feed on entry be used to help start the "melting process". Another side note is I am conventional milling (cutter full width) when facing, but I have been profiling the sides in a climb cutting direction.
thanks for your help

[Superman]

Appearantly, from the Greenleaf rep, you have to get temp up at the cutting action, if you have notching happening, not good, I think he said chipping was a better sign that you were getting closer

Conventional verses climb ? IMO climb would be better, if a tip goes down , it'll push away from the part, and the chip would have warmed up by the time the tip comes close to a feature on the part

Our rep has got us going on the 1.5" Excellerator with 3/8" buttons-3 flute with RPGN-32 tips
I went on leave when they started trialiing this tool, I would guess the feed would go up being a round tip ( a feedmill type of action ). Sharp changes of direction should be avoided ie fillet internal corners 0.06"-0.08" larger than tool radius
He's getting us to semi-finish the walls that the above tool clears to using a 1.5" excelerator- square tip -2 flute with SPGN-434 tips

-relieve the corners ( get rid of any heavy cutting the next pass would do )
-1 pass ( to remove the rad left by the previos tool )

don't currently know what stage we are up to now.
I hope this helps

Found these PDFs for reading
"MILLING 101" in ceramics
and
Ceramic grade WG-300

[Delw]

superman,

when ever your using ceramics we found your tips will last longer if you cut an angle on the piece your cutting then use the ceramic. both lathes and mills. having a sharp edge will destroy a ceramic before it even gets a few thousanths from the edge. Try it you will be very surprised of the results. I havent played with ceramics on mills that much however on face cutters we have had them do a big helix down to the part from center and cut out to the edge NEVER cut into the edge again as thats what breaks down the tips.

Greenleaf are good inserts.

[little bubba]

Milling with ceramics is fun. I did a butt load of it a few years ago on A286, took my roughing time from 24 minutes with carbide to 24 seconds. Tool life was 3-4 parts, so under 2 minutes before indexing.

There is an excellent article from 5 or 6 years back on MMSonline that really helped me out with ceramics, I've posted it here before and have it book marked at the shop.

Things I learned, I'd wager a guess that about 90% of your tool destruction comes when entering the cut, that has to do with heat, going in cold is what eats up your inserts, you want to ramp in with as small of a contact point as possible and probably a bit low on the feed just build up the heat.

Once you are in the cut, you need to stay in the cut, and as you've noticed the cratering, you have to constantly vary the depth of cut. As you've been in the cut for a while, more heat is building, so you may have to slow down on the spindle speed a bit and move up on the feed per tooth.

As for the actual toolpath, I highly doubt you are going to find a CAM generated path that will give you constant non stop cutting while varying the depths of cut. I spent a lot of time coming up with a ramping looping toolpath with constantly changing feeds to get all of my roughing done in one shot. Remember the majority of tool damage is entering the cut.

As for understanding ceramics, your right, it does plasticize the metal and push it away, you need to be running fast enough to heat the metal that much, but not so much it turns into a liquid and feed hard enough that you are pushing off the hottest metal, but not too hard so you are going into solid metal. The cratering (depth of cut notch) is from the surface of the metal cooling quicker, therefore harder and doing more damage to the insert.

Quick rule of thumb, they are the total opposite of carbide. You need to run faster on an interrupted cut(milling) than in a constant cut (turning). If the inserts start chipping, run faster. When your machine looks like its almost on fire and you think a helicopter is landing on your roof, you're almost running it fast enough.