Jig grind 4340

We have .175" through holes on 4340 Rc 56 with .010 stock. Tried high speed spindle on our Moore #3 with CBN mandrel. Any suggestions to speed things up?

Why leave so much to grind? Is position that bad?

No, position is fine. Just the way we recieved them. Client probably left more for HT.

Might be possible to plunge a carbide endmill at that hardness and get rid of some excess material. Wouldn't be fast but faster than grinding. What is the finished hole call out? What kind of gaging?

The finish is .1877 +.0003. Carbibe won't cut this Stuff and all you do is burn up bits and time when you try that. We are thinking slow it down with a slower spindle and choke up on the CBN but just hoping I'm missing something. Usually these tiny holes need higher speeds but these super metals are just harder than hell. These new aerospace alloys are so durable, you can't even grind them...in a reasonable amount of time.

I would choke up on the CBN point but keep the speed up. It may seem abusive but push it hard to within a couple of thou, make it sing loud, then ease up so that your hole will be cylindrical. Can you get a coarser CBN point? I used to grind 8mm and 2mm holes in 416 and 440C for days on end. The 416 was comparable in hardness and that is how we did it, though we did not have that much grind stock. It will seem hard on the machine but the Moore can take it. The 8mm hole had about 5-6 thou to go and eventually could do one in less than 5 minutes including loading. Tolerance was +.0002, gaged with Deltronic pins. Once you got the hang of it you were stuck there forever it seemed.

Rough them out with plated diamond?

Hi Jerry:
In your first post you said 4340 at 56 RC.
4340 is neither exotic nor is 56 RC very hard.
It's got a bit of nickel and chromium in it so its a bit shittier to grind than plain carbon steels, but not overwhelmingly so.
However at 56 RC it'll hardmill just fine.

You should be able to interpolate those holes within half a thou of position and diameter easily with any decent CNC mill and a bog standard 5/32" or 4 mm TiAlN coated carbide endmill unless they're really deep holes.
Leave a thou on for the jig grinder and you're good to go.

You might even be able to mill within honing distance and then just hone them the last twitch (assuming they're through holes), but if you want them dead nuts on location, jig grinding is safer.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Thanks to everyone for tge input. Its much appreciated but we have it moving now. Slower speed spindle and cuts like butter.