Finer bore finish needed

[bikemutt]

With a lathe:

I'm taking about 0.0015" off the inside wall of an existing 0.260" hole in brass, depth is about 0.25", hole is open ended.

I started with a Micro 100 boring bar from Grainger as shown in the picture. I'm going in slow with lube and doing a spring pass on the way back out, the only thing I'd like now is a smoother finish. Not a NASA part, I don't have the ability to quantify the surface finish, just be nice to see more shine, less matte.

I've looked at other boring bars which appear as if they may be a tad more blunt, but nothing in the specs says they are designed specifically for finish cuts.

Also looked at the roller burnishers online but I have no experience with them.

Emery cloth for an outside I can imagine, not sure how I'd make it work on the inside.

Figured I'd ask the experts here for their suggestions.

Thank you.

 

[Terry Keeley]

No expert but I've sometimes had better luck taking light cuts in non-ferrous materials with very sharp (honed) HSS tools than carbide.

Also, I think brass might cut better dry...

 

[TGTool]

Stoning a small radius on the corner will help. A sharp corner is preferred for cutting to size like going in with that cutter since the square end cut presents less side pressure. A rounded end will create a smoother surface finish with the possibility of more springback.

 

[eKretz]

If you just want it shiny, do a quick lap on it. Timesaver compound is good and won't embed in brass.

 

[henrya]

All above are good — super cheap version is this:

Cut a slit in the end of a wooden dowel and put a strip of fine abrasive paper in the slit. Wind the paper around the dowel and place in hole with lathe running. Push in and out a few time and see. This is obviously not the answer if you have to make many parts.

 

[john.k]

If you have a million to do,use a ball burnish ...simply press a hard ball thru to size the bore.

 

[michiganbuck]

All above are good — super cheap version is this:

Cut a slit in the end of a wooden dowel and put a strip of fine abrasive paper in the slit. Wind the paper around the dowel and place in hole with lathe running. Push in and out a few time and see. This is obviously not the answer if you have to make many parts.

To add to henrya's suggestion the length of the abrasive paper or choth strip wrap on the slotted shaft makes an accurate size. and you can turn the strip around to use the other end. and tuck a piece under to get a fresh. area.

I used to use that method when the sunnens were busy, the part was too big or in a machine, or I had to fit something out on the floor.
But take care opening holes for size because saw Hack guys open a bore when it was a bug on a keyway that needed a file or a hone....and not a hammer to refit to a something to a shaft

 

[eKretz]

I use the strip of emery on a slotted stick method now and again also, but not in a .260" hole... My first choice would probably be a reamer. After that the lap. If I had a lot to do, the ball burnishing method mentioned by john.k is good too.

 

[FredC]

I see the first line you mention "on a lathe". I do a lot of production of brass parts with bored finishes. I always flood them with cutting oil. I have known people that when honing an edge on carbide think that rounding over the edge is the desired way. Wrong, if you ask me. I take a fine diamond hone and break the sharp corner with clearance going in the downward direction. I just want to see a line about .001 wide. Never have tried reversing the feed at the same setting seems counterproductive to me for precision or finish.
Finish pass for very small bores (.04 to .08) is about .001". Maybe .002 or .003 for larger bores.

These things are standard procedure for me and I always get good finishes. This is assuming the lathe you have is fairly tight. Even works on my old 9" South Bend, without flood cooling, a shot of cutting oil does the trick there.

 

[michiganbuck]

I do think that I could design a small hole hone device to go down to about .200".
likely use/invent a spring-loaded cone and a vitrified single AO or diamond abrasive 1/4 round.
I was once in charge of a manufacturing department that used cone-driven honing bars...and aided in the design of a few.

*You might call these guys to see if they go that small.

Small Hole Honing Tool | Single Stone Honing Tool | HONING

The single-stone honing tool is designed to process inner holes and improve the surface finishing on their internal walls.

honing-solution.com

I knew a fellow who made a fortune on a boat load of small parts, with honing a couple of tenths. They were so close to the wrong size that a number of passes made them good/spec. likely a Sunnen in a truck might be a decent business (no, he was in his shop and it was a military part he bid on fixturing and grinding the part so bid high , and won the bid.)

 

[Conrad Hoffman]

It's really desirable not to mess around with 2nd operations if you can get the finish in the first pass. I'd start with a very rigid bar about 3/4 the size of the hole, HSS very sharp and with a small radius. I'm not a huge fan of reamers, but the right purpose-ground reamer could probably do this well. You can also drive a ball through the hole to smooth it out.

 

[PackardV8]

Surprised no one has mentioned the Sunnen valve guide hone as an option.

jack vines

 

[AlfaGTA]

This is my choice for small hole boring.....
This bar is 5mm OD ,will bore minim at.205" 20mm deep Other sizes available
Solid carbide and coated....Have used these in brass and works a treat...great finish.
One advantage here is that bar fits into a holder that registers the bar for length and clocked position, so changing tools does not screw up your setup.

Bar:https://www.sandvik.coromant.com/en-us/products/pages/productdetails.aspx?c=cxs-05t098-05-5220r 1025

Here is the holder, other styles available.

Sandvik Coromant

www.sandvik.coromant.com

Cheers Ross

 

[bikemutt]

So many great ideas, thank you!

I dug into the Micro 100 site and found a tool that's specifically made for finish operations. I'm going to give this a try first, then move through other options if it doesn't work out. This one has 0.5" maximum hole depth, should be more rigid than the 1" cutter I started with.

Ordered one from MSC today.

 

[Tyler337]

With a lathe:

I'm taking about 0.0015" off the inside wall of an existing 0.260" hole in brass, depth is about 0.25", hole is open ended.

I started with a Micro 100 boring bar from Grainger as shown in the picture. I'm going in slow with lube and doing a spring pass on the way back out, the only thing I'd like now is a smoother finish. Not a NASA part, I don't have the ability to quantify the surface finish, just be nice to see more shine, less matte.

I've looked at other boring bars which appear as if they may be a tad more blunt, but nothing in the specs says they are designed specifically for finish cuts.

Also looked at the roller burnishers online but I have no experience with them.

Emery cloth for an outside I can imagine, not sure how I'd make it work on the inside.

Figured I'd ask the experts here for their suggestions.

Thank you.

View attachment 374910

 

[Tyler337]

Sfm around 425-525 with a DOC at .02 for the finish pass with the biggest tool nose radius you can use. The bigger the better and feed at .005 - .007. Feeding slow doesn’t usually help for a good finish on brass. Too light of a finish pass won’t finish well on brass either. For example when I finish a groove on an od i don’t want my grooving insert spending a lot of time when finishing in z. The longer it dwells the more feed lines I see. I leave .007 - .01 DOC to finish the groove and sfm at 400 with a .0065 feed. I got the groove at a 22 finish. But this was on 13 chrome. So spin it slow, DOC at .02-.03 and don’t let your insert make contact on the brass for too long. If you can fit a wide grooving insert on a very Rigid bar then I’d give it a shot at .015DOC 450sfm at a .0075 feed. If ya get tired of trying to find the sweet spot just leave the id .005 small and use a small stick wrapped in some fine scotch bright and polish it to size and then you’ll get your finish.

 

[BOB-OO]

+1 AlfaGTA- the small Sandvik tools are the best I've used, never had an issue with a poor finish even in interrupted cuts.

 

[eaglemike]

Taking out .0015 isn't much. I used to hone brass tubing long ago with a Sunnen hone. Obviously if you only have a few, and don't have a hone, not worth it. We had some custom mandrels made. Worked really well. Don't know the job you are running, so just a thought.

 

[CarbideBob]

Tool number one is going to make a smeared cut unless modified.
You need more top rake to shear the material cleanly. A lot more or insane SFM.
Tool number two says top chipbreak but no specs on angle. .006 rad and tons of back clear so maybe shinny but full of feed lines?? Interesting to see how it does.
I'd grind this with lots of top rake (20 degrees) and 10 degrees of back rake, polished top to get a clean shear and chip flow.
This not an option for most who do not have the stuff to do it and you would not want me to quote a one piece run.
One can do the flap thing on bores this size. The core will be small and size control a pain.
IME big rad tools do not work so well here.

 

[WakelessFoil]

I have heard guys get better finishes with HSS steel tooling when it comes to softer materials.

May have already been said but choke up the boring bar as much as you can to reduce any flexing.

Hope this helps.

-Justin