Poor finish on boring bar operation. Brass and thin walls

[EyeEmTrash]

So I am making what you can call a screw on lid for a part on the lathe. It is made out of brass. The walls that are closest to the opening are only .03 thick. The finish is coming out pretty bad. It's not all that rough but you can visibly see the lines. Does anyone have a fix for this? I have tried using the same boring bar for both ops, a rough bb and finish bb, different inserts, .001 feed and .005 depth of cut and a bunch of other feed combinations, I adjusted the spindle speed some. To no ends as they all have the lines. Am I missing something? Any tips?

I forgot to mention, the finish on the rest of the operation is fine. The walls are a bit thicker in those parts. Is it chatter?

Edit: So I think the problem was that the chamfer/radius was too big. I lowered it and it came out really clean. If the problem comes back, I think I will run the ID operations first and then the OD. I appreciate all of the tips but like I said my job says its okay with the lines. I don't want to get too complicated by wrapping it and everything else as that will be too time consuming. Thank you all for the help!

 

[charlie gary]

Got a picture? There are many ways to envision "the lines".

 

[EyeEmTrash]

Got a picture? There are many ways to envision "the lines".

 

[EyeEmTrash]

Got a picture? There are many ways to envision "the lines".

my job says its fine so its not the end of the world if I cant fix it but its bothering me and I would like to be a better machinist.

 

[EmGo]

Because it's so flimsy it's vibrating like hell. Anything you can do to constrain the part will help. I'd probably just make a little cardboard mold and pour wax all around the outside, like a cylinder. That might still be too flimsy but anything you can do like that will fix the problem. There's some really low-temp melting metal that people used for that a lot. Cerrobend ?

 

[FredC]

Try a .001 depth of cut on your finish path. I have a general rule of .003 on ODs to get get precision and close tolerance. On IDs with small boring bars .001 usually works best. You are not sticking that boring bar too far out are you? It is on center?

Edit additional info:
On boring bars for that kind of work I do use carbide and sharpen the front to a keen edge and put the smallest possible corner break on the point with clearance in the downward direction. A larger radius on the corner would be your enemy.

 

[EyeEmTrash]

Try a .001 depth of cut on your finish path. I have a general rule of .003 on ODs to get get precision and close tolerance. On IDs with small boring bars .001 usually works best. You are not sticking that boring bar too far out are you? It is on center?

Edit additional info:
On boring bars for that kind of work I do use carbide and sharpen the front to a keen edge and put the smallest possible corner break on the point with clearance in the downward direction. A larger radius on the corner would be your enemy.

I have tried a .001 DOC, still had the lines. No the boring bar is barely sticking out. I have used inserts with a .015 radius and down to as small as I have. Still no luck. But I will stick with a lower DOC and smaller radius insert to minimize the problem. Thanks

 

[dandrummerman21]

I have never turned a wall that thin in brass.

But the idea that "anything can help" is valid.

So my suggestion, that may not actually improve anything, but wouldn't hurt to try, would be to wrap a couple big rubber bands around it. Will reduce "singing". If it is more "flex" related, then it may not fix it. But worth a try??

 

[charlie gary]

That looks like chatter in your bore. When I turn thin wall stuff (.007" or thinner), I try to do the inside work first when there's a lot of material to support what's going on. Then I leave large amounts of material on the O.D. and take a finish cut with a light feed rate (.001"-.003" IPR). Sometimes features dictate turning the outside first, and when that happens I typically rough the I.D. within about .005" of the finished size and then take my last cut with a dead sharp tool because the nose radius of the tool should be smaller than the thickness of the cut.
Others have mentioned putting something on the O.D. to lend support against the cutting forces. I've had good luck with Bondo. It is easy to use, and when your done you can remove it with heat or paint stripper.

 

[EmGo]

I have tried a .001 DOC, still had the lines. No the boring bar is barely sticking out. I have used inserts with a .015 radius and down to as small as I have. Still no luck. But I will stick with a lower DOC and smaller radius insert to minimize the problem.

This is a case where a really SHARP hss tool MIGHT help.

But when the part is really thin, or really long, it wants to vibrate. You'll see guys with a lead hammer pressed across the top of a shaft, or stuff tied around the part, or all kinds of tricks to try and dampen the vibrations.

Sometimes it even works

 

[michiganbuck]

Just a guess here...run the machine at 200 rpm and wrap upholstery thread along the OD, Double wrap would be quick to install, with the start stuck with a tab of masking tape..and place a rubber band over to lock the thread. Then go back to turning RPM,
Turn/bore with a very sharp HSS tool bit,..
Good to draw the radius (small section of) at 10x scale, and draw in your tool bit edge to see what clearance looks like in the radius of the part.
You might try 10* side clearance and 5* top rake
Drawing the action will tell how to install the tool clearance in an ID part, often The clearance needs an adjustment to the arc of the part..and a secondary to avoid any rubbing.

looks like 100SFPM might be a decent try.
Sharpen the bit with a 60gt (or finer)wheel the hone the edge with a fine stone.

We used to wrap a snake of children's modeling clay around a grinding job..but you cant do that with lathe speed..unless you hold the part still and tree-pan with the tool bit rotating.

 

[sfriedberg]

That's an absolutely classic chatter pattern. I have seen woodturners with special wobbly tools for turning that very texture.

 

[EyeEmTrash]

That looks like chatter in your bore. When I turn thin wall stuff (.007" or thinner), I try to do the inside work first when there's a lot of material to support what's going on. Then I leave large amounts of material on the O.D. and take a finish cut with a light feed rate (.001"-.003" IPR). Sometimes features dictate turning the outside first, and when that happens I typically rough the I.D. within about .005" of the finished size and then take my last cut with a dead sharp tool because the nose radius of the tool should be smaller than the thickness of the cut.
Others have mentioned putting something on the O.D. to lend support against the cutting forces. I've had good luck with Bondo. It is easy to use, and when your done you can remove it with heat or paint stripper.

I like that idea and I'm a little upset that I didn't think of that. I also realized the chamfer/radius may have been a little too big, so I lowered it and the first part that came out was line free!

 

[charlie gary]

I like that idea and I'm a little upset that I didn't think of that. I also realized the chamfer/radius may have been a little too big, so I lowered it and the first part that came out was line free!

There's nothing to be upset about here. If you knew the answer to every challenge, you'd be the person running the show. Be happy you were smart enough to ask a question and get lots of good feedback.

 

[AlfaGTA]

My go to on thin parts like that that want to vibrate is to leave the OD thick and finish that ID.
Further modeling clay works well to dampen the part and prevent chatter.
Form the modeling clay around the part.
Form it into a cylinder around the part.
Easy to apply, easy to remove, cheap.
Fits all kinds of shapes.
Cheers Ross

 

[Scottl]

Because it's so flimsy it's vibrating like hell. Anything you can do to constrain the part will help. I'd probably just make a little cardboard mold and pour wax all around the outside, like a cylinder. That might still be too flimsy but anything you can do like that will fix the problem. There's some really low-temp melting metal that people used for that a lot. Cerrobend ?

Or even tape on a wrap of heavy rubber around the OD. Better yet, bond on some lead roof flashing with a heat removable adhesive such as jeweler's wax.

 

[rjwalker1973]

Or even tape on a wrap of heavy rubber around the OD. Better yet, bond on some lead roof flashing with a heat removable adhesive such as jeweler's wax.

Great ideas

 

[rjwalker1973]

Does your machine have SSV? Sometimes it can help . Also do you have the option to bore the ID first?

 

[???]

One offs I would finish the ID with my thumb and forefinger lightly holding the part. Super sharp tool, small DOC. Not recommended if you have two thumbs . I have also made a Delrin sleeve to lightly press over before.

 

[MCritchley]

How much stock is on the OD?

As others said I’d do the inside first then finish the OD

One thing I’d add is a threaded plug that has a tight fit in your bore. The plug will stiffen that part up considerably.

You might also get away with shoving a tapered silicon plug in the bore to stiffen it up.