What's new
What's new

ID Grinding Titanium Carbide, advice needed.

jspivey

Aluminum
Joined
Nov 18, 2018
Location
Southern Illinois
Hello all,

Does anyone here have any experience grinding Titanium carbide? Tomorrow at work, I am going to have to start ID grinding some parts that came from the manufacturer with bores about .02 under size (Miscommunication between my boss and the manufacturer). The bores are approx 1.8" dia and about 1" deep. The setup I have to work with is a Dumore tool post grinder with 32,500 rpm spindle running a 3/4" diamond wheel from Falcon Tool Company.

Basically, what should I be looking at as far as spindle speed on the lathe, feed rate, and depth of cut. I have looked around online and haven't been able to find much. While I have a little bit of grinding experience, this is definitely way out of my comfort zone. Any advice would be greatly appreciated.

Thanks,
John
 
If the bore goes through, wire EDM. This sounds like a really time consuming project. I would guess 60 -100 rpm, .0003 - .0005 doc, .01 - .02 IPR but don't know how rigid your Dumore grinder is. I would use flood coolant if at all possible.
 
Thanks to both replies. Unfortunately the bore does not go through, so wire is out. Thankfully I do have flood coolant available. I don’t know how rigid the grinder will be either, as I’ve never used it before, but I am trying to stay optimistic. I’ll report back some results when I can.
 
You may want to do the roughing passes starting inside the bore and coming out.
Then finish going in.
The reason here is that the wheel is going to wear a taper and if all passes inwards your hole will have that taper at the bottom.
You don't say which mix TiC but this stuff loads most wheels fast. A very soft stick is your friend.
It also chips out like crazy if your wheel grit too low. (you are in what we call low speed grind but not much to do about that) .
If critical watch out for that opening to the face under a microscope.

Rotation wise I'd be as slow as your lathe can go. 30 RPM would be fast for me.
DOC and feed limits set by the spindle power.

Assuming you can dress/true the wheel and re-chuck accurately you may want to consider a rough op on all parts and then go back for a finish with a fresh wheel.
Missing is the tolerance on the finish hole so my world may not be yours and all the above nonsense from some loonie guy on the net...:willy_nilly:...:typing:
Lots of coolant, I hope it just turns out to be dead easy.
Bob
 
Bob,

Thanks for all that info, definitely a big help. I don't know what mix of TiC it is, but I may be able to find that out tomorrow from the boss. I'll also have to look again at the wheel grit tomorrow, but I'm fairly sure it's not super course. Thanks for the tip about plunging into the bore at the bottom, makes perfect sense that taper could be a problem otherwise.

I have to make an arbor for the grinder, and once that is done, my plan is basically just to see how it goes and go from there, whatever "there" ends up being. I'm hoping for dead easy, but who knows. As for tolerance, I remember now that the bores finish to 47mm nominal and calls out H7 for the tolerance. So a little less than a thou to work with.
 
Thanks to both replies. Unfortunately the bore does not go through, so wire is out. Thankfully I do have flood coolant available. I don’t know how rigid the grinder will be either, as I’ve never used it before, but I am trying to stay optimistic. I’ll report back some results when I can.

(X) OD feed outside and travel onto the bore will cause the leading edge to break down and put a radius at the bottom of the bore.

(*) A very small feed to the OD and taking stock on the way out reduces this wheel wear/edge break down..

Because the full wheele is in the feed a very very small feed, like a tiny feed and spark out then travel.

Like Bob said you may have to fresh wheel if thh corner gets to large a radiud.

Blue up the last .003 - .005 to see straiht bore.

Likely this feeding to the OD can only be done wet.

Arbor should run near dead on and be short so less wip.
 
+1 for in-feeding inside the part, then feeding out of bore. That's how I do any grinding that's up to a shoulder.

I've never had to work with this material, would it be possible to bore in the lathe with a diamond tipped insert or some other insert above carbide?
 








 
Back
Top