What's new
What's new

Best Way to Deburr Back Side of 1/8" Hole in 4340???

Nerdlinger

Stainless
Joined
Aug 10, 2013
Location
Chicago, IL
Cross drilling an 1/8" hole in 7/8" round 4340 straight down in Z. I spot before drilling so the top side of the hole already has a nice chamfer but the back side is all burry. Should I just use one of those spring-loaded EZBurr, BurrAway, etc. or is there something else that's better??? :scratchchin: Thank you!
 
Cross drilling an 1/8" hole in 7/8" round 4340 straight down in Z. I spot before drilling so the top side of the hole already has a nice chamfer but the back side is all burry. Should I just use one of those spring-loaded EZBurr, BurrAway, etc. or is there something else that's better??? :scratchchin: Thank you!

Yup. That will work. You will end up with a bit of shape to the back chamfer but it should match the front chamfer.
 
I am very :skep: about a spring loaded chamfer dooing anything in this app, but if you doo go that route, please report back!.

I would just flip it over and hit it with a 1/4" multi-flute chamfer tool in a cordless drill if it was me.



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

Think Snow Eh!
Ox
 
I use BURR AWAYS all the time...get the ones like this with the blade its stronger...if theres a tall wall I do both sides the BURR AWAY is by far better than the BURR OFF style....I use for inside pipes...I beams...square beams...etc

New-in-tube-cogsdill-burraway-tool-750-type-b-blade-4-photo.jpg



 
Ez burr has nice options. Harvey has some options too Harvey Tool - Carbide Back Deburring Mill

I might expect a little kaboom if you try to take off a 4340 burr with a Harvey 57110 -- .087" shank, 1" neck length. maybe it'll work a treat :scratchchin:.

I use BurrAways, but one downside to them is you need some room on the backside for the pilot. You can reduce the pilot length, but only to a certain point. Assuming this is a CNC lathe job, you'll need to drill deeper to make room for the pilot.

I'm with Ox --hit it with a countersink in a handheld drill. 5 seconds.

Regards.

Mike
 
Run it in the 4th axis.. Might be overkill for this particular job, but
I did have a job where I had to drill cross holes through some threads,
deburring 10 or so wasn't bad by hand, but deburring hundreds of threads
by hand, F'that.. Rolled it over and deburred with a sharp endmill.

Those springy deburr tools are awesome, but I'd be a little scared at
that hole size..

As already been said, cordless drill and a countersink.. You can NEVER
have enough cordless drills in the shop.. Ream, Drill, Tap, Chamfer, they
even work in a pinch with some small abrasives if need be.. I'm small time
and I've got at least 6 drills floating around here, they get used constantly.
 
I've used a pin or drill shank in a vee block on the Bridgeport.
Stick the hole over the pin and chamfer.
 
Now there is one other option, if you are in a 4th or in a Y axis lathe, and this works especially well on rounds:

You can index to 270* and come in from the side with an endmill. You may need to play with the size of the mill 'till you git what'chew want, but it will de-burr w/o cutting way deep on the apex. It may push some back in the hole tho?

In some applications, it is a good alternative. I guess it would depend on the ratio of the hole and the bar/tube size.


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

Drainin' the Swamp!
Ox
 
It turns out we had an 1/8" burr away tool that, so far, has worked great! I perfectly smooth chamfer that didn't do the old, "take one fuzzy 90-degree edge and turn it into two fuzzy 45-degree edges." It's just a matter of life now so we'll see!
 
Hmmm, I do like solid carbide deburring tools over brushes and spring-loads dealies and i see they have one of those with a 1" neck length....the programming would be more "fun" than a burr away but whatever. I just might give it a try if the burr away doesn't hold up. Thanks!
 
I am very :skep: about a spring loaded chamfer dooing anything in this app, but if you doo go that route, please report back!.

I would just flip it over and hit it with a 1/4" multi-flute chamfer tool in a cordless drill if it was me.





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

Think Snow Eh!
Ox

In my shop all those off-line secondary ops that, "just takes a second" always adds up to piles of nearly-finished parts that are waiting for that last op so I alway try my darndest to let the machine make it as complete as possible.
 
Regarding 4th axis. There is a blind hole at 0 degrees then indexes to 90 degrees for the cross hole that goes through. i can't insert to 270 to deburr the backside of the hole that was drilled at A90. because there is another part in the way. At A0. I tried coming up against the back side of the hole with a 3/8 end mill that was alread on the tool list but it looked kinda shitty. Maybe a smaller em would have worked but so far the burr away is working like a champ.
 
For the record the 1/8" Burr Away has worked beautifully. About 400 pcs in and still going strong. I figured no one here would know what a chamfered edge would look like so I attached a pic and made sure to hold my phone in landscape mode. Thanks for the help!

Chamfer.jpg
 
Well, I must say - I for one am impressed!



and made sure to hold my phone in landscape mode.

That's impressive too!
Now - any chance you an send any of that my wife's direction?




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

Think Snow Eh!
Ox
 
glad It worked for ya....another tip with those...I run really slow RPMs and those last a couple of years....I run coolant and dry....as long as its slow it will last doing any material...and on cross holes I rapid to hole...feed down past hole with spindle off...turn on spindle....feed up and back down for chamfer....turn spindle off....feed out to above part...rotate hole 90 or 270 or whatever...repeat....and I do top of hole as well by feeding down once at rapid spot and back up then spindle off feed down....always spindle off when traversing thru holes...only spin on chamfers
 








 
Back
Top