Deep hole boring on a lathe

I have a 3" diameter piece of 6061 I need to put a 3/4" hole down the middle. I will be 8 1/2" deep. Using a 5/8" boring bar it chatters no matter what I do, Using HSS honed to very sharp and taking small cuts makes no difference.

Surface finish on the hole is important and it needs to be within .001" of .750". I have never had to do a hole this small and this deep. Were the hole something like 2" diameter, I would have no problems. How do you keep a 5/8" boring bar from bending????

Laverda said:

I have a 3" diameter piece of 6061 I need to put a 3/4" hole down the middle. I will be 8 1/2" deep. Using a 5/8" boring bar it chatters no matter what I do, Using HSS honed to very sharp and taking small cuts makes no difference.

Surface finish on the hole is important and it needs to be within .001" of .750". I have never had to do a hole this small and this deep. Were the hole something like 2" diameter, I would have no problems. How do you keep a 5/8" boring bar from bending????

Click to expand...

Solid carbide? Did you slow the rpm way down?

Bore it for a couple of inches, then finish with a reamer.

Drill it .030 undersize then ream it.

And do you really need it within .001 over 8-1/2"?

I would do it by drilling to within .010 of finished diameter, being careful minimize drift with sharp, balanced grind drills, preferable machine ground. Frequency chip clearings. Through the center coolant would be nice. Then bore about an inch deep .001 of the final diameter and then ream with a sharp reamer using frequent chip clearings. The initial bore is the accurately center the reamer. As you get deeper, the odds are that the hole will drift from the drilling so take it easy on feed. A left hand twist reamer will help push the chips ahead of the reamer.

Tom

Laverda said:

I have a 3" diameter piece of 6061 I need to put a 3/4" hole down the middle. I will be 8 1/2" deep... How do you keep a 5/8" boring bar from bending????

Click to expand...

You can't keep it from bending and chattering.
5/8" diameter and 8 1/2" inches overhang is almost 14:1 lenght-diameter ratio or 14xD.
Anything over 4xD is not recommended for normal steel boring bars.

If you have deep pockets:
Solid carbide boring bar maybe up to 6-8xD and 500 usd or so
Dampened solid carbide boring bar 14xD if you really push it. 2000 usd or so...

https://www.sandvik.coromant.com/si...s/global/technical guides/en-gb/c-2920-23.pdf

Laverda said:

How do you keep a 5/8" boring bar from bending????

Click to expand...

..and vibrating. At that depth? Generally, one doesn't.

Hole isn't REALLY that deep, given you are only working shiny cheese, but you are actually into self-supported / self-guiding tool territory.

For a lathe, search on "gun" drills and "balanced" boring heads.

Piece of cake for a hor-bore, but only if it was a "through" hole, not blind.

Tight budget, you might have to settle for reaming and roller-burnishing to hit size and surface finish spec "sort of" cheaply.

Even a good drillpress can do that, and generally faster and cheaper than the lathe, most especially IF.. you have spare stock enough to make the hole FIRST, then turn the OD and other features concentric to it on a mandrel at HS, center divot at the blind end.

2CW

Drill to within 1/64'' of finished dia, single point bore first 2 to 3'' deep to finished size, complete job with a simple tool makers reamer made from silver steel / drill rod.

Limy Sami said:

Drill to within 1/64'' of finished dia, single point bore first 2 to 3'' deep to finished size, complete job with a simple tool makers reamer made from silver steel / drill rod.

Click to expand...

.. or .. hold even that half-bore alignment area a tad undersized, put a "pilot" on the reamer, and have lower risk of a disjoint in finish.

Guess you might check the tool bit clearance..Hold it to 5/8 radius gauge(if the bore is over 5/8),bit at center line of gauge and with a loop see clearance all the way down to the heal. That it is very sharp..That you tool post is back a little on you saddle better center there so not rocking forward. Perhaps your top rake 10*, side cutting edge perhaps 15/20* off 90. slow feed , high rpm perhaps try 700 ?, depth of cut minimal.. that all very basic so likely you tried all..

be sure you don't feel chatter in the tool post?? knock a shim under the front of the boring bar pushing it up tight in what ever holder at the lead edge of holder..Hand/bolt a heavy lathe dog on the out end of the boring bar if it is long that way..

Agree with bump larger the bore as much as is safe with drills and reamers.. 3/4 reamer might give better finish with coolant flood in the drill press. Yes best to test the reamer in a scrap to be sure +-.001

Yes could go the other way. boring bar but end in the 4jaw.. out end of boring bar on a live center. and hold the part in a cross vise..Tricky to get it straight and dead on center that way...