Hole Burnisher

[jeff]

Does anyone have any experience with these?

We have a repeat job that requires a thru hole size of .3747/.3742 with a 64 micro.

Reamers are a pain to constantly hold size, and of course jig grinding is not an option because the boss says it's too expensive.

Approximately 50 holes per month, in 4340 PHT material about 1-1/4 thru.

[tozmaster]

I have used these in the past, it was on thru holes in an aluminum casting.

Once set, pre burnish bore size also an important factor, but once it was set up and going we ran thousands of parts without any issues.

Is your 4340 heat treated?

I have heard that with heat treated steels up to a reasonable HRC like 45-47 they work even better for surface finish in the 8 to 16 realm.

[jeff]

it's 4340 PHT which is 28-32 Rc

[djstedman]

Call me crazy but that doesn't sound like it should be that hard to do with a reamer, we have done some burnishing here and from what I remember, it tended to be a hell of a lot more of a pain and expense than finding a way to get it to work using reamers or boring. We have one job running in 300M @ 52-55Hrc (basically the same alloy as 4340) where we are doing .1968 +.0004/-.0000 and we run the same carbide reamers for hundreds of parts..

 

In our case we drill .. then mill leaving only about .002 / .003 for the reamer, then ream again with a second reamer and then a third reamer and we use Moly-D for lubricant rather than coolant..

 

By doing that we have one job running in 300M @ 52-55Hrc (basically the same alloy as 4340) where we are doing .1968 +.0004/-.0000 and we run the same reamers for hundreds of parts.. the first one takes the brunt of the material and ends up having to be changed out every 50 or 60 parts.. but the other two tend to last for quite a long time.

 

Things to consider if you cant get your reamers to maintain size.. Do you Mill the hole? or just drill it? How much stock is being left in the hole? Have you tried adding a second and or third reamer? and what's your source of lubrication for the reamers?

[MIL-TFP-41]

We use them all the time. Cogsdill. Best off talking to them to get the pre-burnish hole size and finish requirements. You will be amazed that the finish you get and the longevity of the tool. We run with just water soluble and have yet to run into a problem.

Your process is gonna most likely look like this tho....

Drill

Ream

Burnish

Gonna have an extra toolchange....but if it makes the process better and more reliable...then its worth it.

[tozmaster]

+1 ^^^ What JMC said, only I would add a countersink if allowable between drill and ream.

[jeff]

Things to consider if you cant get your reamers to maintain size.. Do you Mill the hole? or just drill it? How much stock is being left in the hole? Have you tried adding a second and or third reamer? and what's your source of lubrication for the reamers?

 

Currently we just spot face, carbide drill with a 9.2mm OSG drill (so about .012" being left for reaming), chamfer, and ream by hand on a Bridgeport with a cheap Morse HSS reamer.

Lubrication is a cutting oil, I think it's tap magic.

 

Is .012" too much for a reamer? I've always tried to leave about .015" for reaming. Maybe that's why it's such a pain to have consistency.

[Rstewart]

Currently we just spot face, carbide drill with a 9.2mm OSG drill (so about .012" being left for reaming), chamfer, and ream by hand on a Bridgeport with a cheap Morse HSS reamer.

Lubrication is a cutting oil, I think it's tap magic.

 

Is .012" too much for a reamer? I've always tried to leave about .015" for reaming. Maybe that's why it's such a pain to have consistency.

 

The amount left for reaming is proportional to the Dia. I usually leave somewhere around 7% of the hole dia. example: .277" hole * 7% is .019"

[jeff]

My concern with a burnisher is that it work hardens the material? The parts are already 28-32, what Rc can I expect after burnishing?

[jeff]

Just noticed our boss is buying us .3745 reamers for this job.

That cuts our tolerance down to +.0002/-.0000

Nice.

No wonder it's hard to keep the no-go pin from going in!

His logic, is that it will cut smaller once it gets dull and wears down.

[Oppiz]

His logic, is that it will cut smaller once it gets dull and wears down.

 

In my 30+ years in this trade I can't think of a time when a reamer cut undersize. Is wire edm an option?

[djstedman]

First, I assumed you were putting the hole in on a CNC, if you are then personally I wouldn't even consider attempting to ream holes on a Bridgeport anymore.. not that its not possible.. It just doesn't make sense to remove the part from the machine.. then put it in another machine for reaming..

 

Also, though I'm sure I will be told by many people the myriad reasons I'm wrong and that this shouldn't work since it goes against pretty much everything I was ever taught by all the old timers I started in this field with.. leaving only a couple of thou in the hole will greatly increase your reamer life and help maintain hole size.. Since were using reamers in the CNC and on most of our jobs we need to maintain tight positional tolerances we generally will drill about .01 under to remove most material.. then mill and leave about .002 which gets us our positional location, then chamfer and finally ream for size.

 

If possible most times I prefer to buy carbide reamers.. for a .3745 reamer its about $50.. and it will pay for itself by not having to mess with it and through extended tool life.. I tend to agree with the other poster .. if anything reamers will pretty much always cut to size or a little over.. I would want a .3743 reamer.. I am sure you could find them and it would make your job a whole heck of a lot easier since it would essentially double your tolerance over the .3745 reamer your currently using.

[brandon b]

Sounds like your boss has the same logic as mine. At least you probably have good holders. I have 20 year od worn out collet holders , I've usually got a thou or two of runout ( if not more) so he tells me to just put tape on the low side of the remear and stick it back in the holder... Lol

[Guyinthedesert]

I would leave about .006, then go in with a carbide reamer. It should be a no-brainer.

 

Did you indicate the reamer in? I wish I had a nickel for every time someone came up to me and said "Reamers no good, it's cutting o/s at the top". Then I stick an indicator on it to find .004 runout. Response from idiot set up guy, "Is that too much?"

 

If it's still giving you trouble, ream it .002 u/s and have it honed.

[jeff]

I would leave about .006, then go in with a carbide reamer. It should be a no-brainer.

 

Did you indicate the reamer in? I wish I had a nickel for every time someone came up to me and said "Reamers no good, it's cutting o/s at the top". Then I stick an indicator on it to find .004 runout. Response from idiot set up guy, "Is that too much?"

 

If it's still giving you trouble, ream it .002 u/s and have it honed.

yes, it was running less than .0005"

Not sure how much stock we were leaving in the hole for that carbide reamer, but the tip is now dull and looks like it was rubbing.

I'm not the one who ran that reamer.

I have a quote in for a burnisher.

Thanks everyone for the input!

[scooke4073]

Google Ballizing.

 

I have used ball bearings (in aluminum) and they work really well. Put a program stop, load the ball bearing into the hole, and press it thru with the machine (used a dowel pin held in a collet chuck)

[jeff]

Google Ballizing.

 

I have used ball bearings (in aluminum) and they work really well. Put a program stop, load the ball bearing into the hole, and press it thru with the machine (used a dowel pin held in a collet chuck)

 

That would be nice if I was the person running it.. .but unfortunately this has to be idiot-proof.

[huskermcdoogle]

but unfortunately this has to be idiot-proof.

 

There is no such thing.

 

You sir should know better...

[brandon b]

For ballizing , How much material are you leaving for the ball to push thru?

[FROZEN]

Komet makes reams that they grantee to work. They not cheap, but worth every penny.

[scooke4073]

For ballizing , How much material are you leaving for the ball to push thru?

I would typically ream it to within about .001.

[jeff]

Komet makes reams that they grantee to work. They not cheap, but worth every penny.

 

Looks like they have some nice products, thanks!

[brandon b]

 

I would typically ream it to within about .001.

ok. With your mill how fast is your feed rate for pushing the ball thru?

[scooke4073]

ok. With your mill how fast is your feed rate for pushing the ball thru?

It's been a while but it was around 10 ipm if I remember correctly. There isn't really much load to worry about....it goes through nice and easy.

[brandon b]

I'll have to give it a shot one of these days. Pretty much The same for aluminum. Stainless. Titanium ...