Better Method? Small-ish bore with taper in C180 Copper.

This is an internal feature on a customer part in C180. The sketch is just a simplified area of the entire part for clarity.

The item is run from bar stock and parted when done. I'm removing most of the material with a name brand 14mm brazed carbide drill (because it was handy) then boring the rest with a 3/8" SCLCR boring bar (CCMT insert). I'm taking cautious light and shallow cuts (maybe 0.010"-0.020" DOC and 0.003"/rev ... and just guessing, but maybe 250 SFM or so) because in the past being more aggressive I snapped off the tip of a boring bar after it became wrapped tightly in stringers and jammed at the bottom of the hole.

There are about 100 of them in a batch and this operation is taking close to half the total time. I'm sure this isn't the most optimal way to get it done.

What are some better ways? It has been suggested to me that I step up the boring bar size to 1/2" and push it harder, but that doesn't leave much room for chips to accumulate and/or escape. I'm already looking at getting a solid carbide drill that's on size, and then I don't need to bury the boring bar down the hole. Maybe that's all there is to it?

Thanks for your constructive suggestions.

Drill to size and use a big centerdrill (offset like a boring bar)
to plunge the 60.

Booze Daily said:

Drill to size and use a big centerdrill (offset like a boring bar)
to plunge the 60.

Click to expand...

Well that's one I hadn't thought of doing. I'll have to try it out on some other things too.

For anyone familiar with C180, you know that this stuff likes to eat HSS for dinner so I'd be into a carbide centre drill. Do you think it would be happy about the side load? I think I might have a pretty big carbide centre drill sitting in a drawer that I've been saving for something special...

So, just to follow up and provide some closure to this, I had the opportunity to try this using a solid carbide 14.8mm drill today. Off the top of my head, I want to say it's a Sandvik CoroDrill 460XM. I can't spin the part at the recommended speed because there would be too much imbalance with the bar and chuck at that speed. But even at 3000 RPM it's pretty impressive. 0.014 IPR was the lower range of the recommended feed, and with those numbers it takes about 1 second to pop the hole in the part about 1" deep. The chips are perfectly formed and all you can hear during the cycle is the chips pinging off the inside of the enclosure.

The drill, combined with using a slightly larger boring bar and taking heavier cuts without fear of chip packing, probably halved the cycle time for this part.