Second side burr on lathe - Suggestions

[wishin4snow]

I have a part with a tight tolerance bore 0.1375" +.0003 / -0.000. I bore the hole to size on first side to keep it concentric with the OD. On second side, I face off the part from the center out to help get rid of the part off ring. I then use boring bar to put a chamfer on the back side and try to draw the burr out but no matter what I tried, I still get a small burr that stops the pin. I was looking for suggestions because I have quite a few to run. I was able to get a reamer 0.1375" that I run through the hole on second side which definitely helped however I did have to stone the reamer to keep it from oversizing the hole. I was just looking for other tips incase I can't get a reamer the size I need on future parts. Material is some weird "Carpenter Consumet Electrical Iron Rod"

Code
G0 X.127 Z.1
G1 Z-.025 F.008
X.132 F.001
X.1376 Z-.005 ( I taper onto the size to help blend the transition)
X.157 Z.005
G0 Z.1

 

[Labrat]

Any chance you can cut the chamfer before you bore to size?

 

[Kingbob]

Take a finish facing pass with the boring bar, it can be .0005 doc, then pull out your chamfer. That burr can sometimes be from a slight discrepancy between the facing and boring tool.

 

[guythatbrews]

X.132 F.001

Try approaching much closer to the finished bore size before starting the chamfer lead in. Like X.137. You just have to really watch you don't undercut the bore.

What is your tool nose radius? It must be near zero to even hit the part starting at z-.005 with no tool comp.

 

[Ox]

I'd git a 1/4", 60* incl, single flute countersink.
(sharp = HSS)

Then I would go in @ X0, go to depth, and then walk it out in X+. This is going to be the least likely to roll a burr inside. Just need to make sure that you have the tool retarded enough to make sure that your cutting edge is hitting, and not your clearance. This is a good app for glass 1/2 empty. (negativity is your friend over positivity)


Also, as your tool wears and starts to roll a burr, you can edit your code or offset U.04 W.02 and go aggin.
(or in this case W-.02)


----------------------

Think Snow Eh!
Ox

 

[MCritchley]

dive your boring bar in a few tenths just before it will intersect with the chamfer you will be creating on opp2. In effect, you would create a very small counter bore like .020" long

The chamfering opp will leave a burr that might only be a tenth, the little cbore will allow the pin to slide over it.

 

[Omega]

https://cogsdill.com/products/deburring-tools/burraway/

Not sure if it will open up the hole slightly, I have only used them on open + - .005 holes....I'd give them a call and ask.

 

[604Pook]

https://cogsdill.com/products/deburring-tools/burraway/

Not sure if it will open up the hole slightly, I have only used them on open + - .005 holes....I'd give them a call and ask.

Those look neat. Do you really need the multiple sizes when being used in a lathe seeing how you can just adjust you X offset to run it along the wall of the ID?

 

[SeymourDumore]

Code
G0 X.127 Z.1
G1 Z-.025 F.008
G01 X.132 F.001
G01 X.1375 Z-.005 ( I taper onto the size to help blend the transition)
G03 X.1475 Z0 R.005 (Radius out, not chamfer!!!)

There, I've fixed it for ya.

Not sure why is everyone fixated on chamfering and expecting no sharp edges ...
If you chamfer, you end up with not one, but two sharp edges in fact.

 

[guythatbrews]

There, I've fixed it for ya.

Not sure why is everyone fixated on chamfering and expecting no sharp edges ...
If you chamfer, you end up with not one, but two sharp edges in fact.

Well, sometimes a radius is not allowed, just as sometimes a chamfer is not allowed.

Personally I think chamfered parts look better, so, if allowed, I chamfer. If the burr won't go away, well, then radius.

It certainly does help to wrap a small radius before or after the visible chamfer, or both, as needs be. Some controls with auto any-angle chamfering and auto corner radius make this reall easy.

I really wouldn't use a cogsdill or heule type tool for this. It's just not needed.

 

[wishin4snow]

Thanks Guys, You gave me some things to try.
Before posting, I did try the countersink tool method but that didn't help.
The boring bar is a sharp nose radius.
I also tried generating a small radius into the chamfer but that didn't help. Rather than Line, line, Line. I tried Line, radius, Line, Line. I did not try a full radius but could give that a try next.

 

[guythatbrews]

Take a very close look at your boring bar. The tip may be gone.

I never use a sharp tool unless absolutely required.

 

[cornerRad]

Flexhone it with a 600grit or higher. Will take the but right off without changing size

 

[guythatbrews]

Flexhone it with a 600grit or higher. Will take the but right off without changing size

I have not had good luck with flexhones and burrs with a corcumferential lie.

For example, on a cross hole the sides of the holes it gets, but the other edges it's very hit or miss and mostly miss.

Wishin4now there is no reason why this should be such a big problem. I think something is fundamentally wrong. Like maybe a chipped tool or above center.