SAFETY: Deburring on a Turning Center

[pwilson101]

At our shop, there is a practice of deburring some of the part on a turning center (from large VTL's to smaller horizontal turning centers) by applying emery cloth to an edge WHILE THE CHUCK IS SPINNING! So the operators arm is reaching over and onto the part while it is spinning in the chuck. This is undoubtedly a dangerous practice and a major accident waiting to happen.

I am looking for alternatives to deburring the part in the machine. I need to do as much work in the CNC as possible, as the operators are running multiple pieces of equipment. I don't want them to have to deburr outside the machine with a grinder, etc if at all possible (we are doing this now in-place of deburring by hand in the machine).

So, is there anything out there that is made specifically for this? I have seen brushes for milling machining centers, but I haven't seen anything for turning centers (although I haven't looked till now - I am new to the turning center department). Or any ideas on what I could "fabricate"?

Any help is much appreciated...

[pwilson101]

Oh, I left out some important information. The edges that need deburring are where a machined and cast surface meet. So I cannot simply program a radius at a transition point. The deburring tool would need to be able to deburr uneven, varying surfaces.

Thanks...

[ad64075]

Very true, reaching into a machine with a rotating chuck is dangerous. That's not to say I have never done it, but there is a "right" way to do it, as well. Instead of reaching the left arm over the part and spindle to hold one end of the emery paper and keeping the right arm closest to the body, simply reverse the order. Reach the right arm away from the body, therefore nothing will be rotating underneath it, and keep the left arm closest to the body. Admittedly, this takes some getting used to but is better that having a sleeve caught in a chuck.

Live tooling using a Scotch Brite Bristle Disc would be your best friend for this type of deburring. Do you have live tooling on your machines?

[pwilson101]

I'm looking at not reaching in there altogether.

And some machines have live tooling, others do not....

[pwilson101]

It seems like there should be something on the market that address this specific issue, considering how much CNC turning that goes on around the world....

[ad64075]

I agree! More often we face similar issues with large OD threads and having operators manually deburr them, which presents its own set of problems. We have researched solutions extensively and determined that most (if not all) applicable deburring tools require rotation (live tooling). On our live tooling machines we have already accounted for deburring, it's our standard lathes that cause grief.

[djr76]

If you dont have live tooling, what about a small air spindle mounted in turret, then plumb air through into the coolant system with a check valve to prevent air blowing back into the coolant reservoir itself. If you have spare "M" function relays, you can wire in an air solenoid to the the relay and turn it on/off via "M" code or turn it on/off manually with a ball valve.

[ad64075]

Originally Posted by djr76 If you dont have live tooling, what about a small air spindle mounted in turret, then plumb air through into the coolant system with a check valve to prevent air blowing back into the coolant reservoir itself. If you have spare "M" function relays, you can wire in an air solenoid to the the relay and turn it on/off via "M" code or turn it on/off manually with a ball valve.

I like the way this guy thinks...

Go Tigers

[djr76]

Originally Posted by ad64075 I like the way this guy thinks... Go Tigers

Thanks, Im a firm believer of "work smarter, not harder", hard work is for fools and mules.

[Delw]

There is NO reason to have to deburr a part that comes off a lathe. the part should be programmed so it has no burrs on each operation it does. it doesnt add anytime to the parts ran too accomlish this.
Of course there are some parts that just cant be done but there few and far between.

any time you put a chamfer on a part in a lathe you will get sharp edges on each end of the chamfer, do to the tool actually leaving the part for the next line.
what you do is before and after every Chamfer or angle you put a small Rad. like a .005 or less or even more if your print allows it, at every corner there should be a rad as well, even if your print calls for .003 max you can put small .001- .002 rad on it.

when running a rad, your tool NEVER leaves the part it always stays incontact with the surface.
try it you will be amazed at not only how much better the part looks but also how much less deburr time is involved. this works on all materials as well as nickle alloys.we used to do it on all titanium work because grabbing a tit part off a lathe with a small burr and coolant covered hands will cut you like a knife.

even on a Mill all parts should be deburred on the machine,

your customers will also love the parts more cause they are uniform. and you wont see deburr wheel marks.

using a file in a machine(with chuck) or emery cloth while the spindle running is very dangerous and shouldnt be done, but like all machinest we have brain freeze and think its easier, one day it will catchup with you.
it did me 2 years into machineing back in the 80's luckly it was just a small chunk of finger ( just the tip and 5 stiches) unlucky for me it was the night before opening day of deer season with a tag that was very hard to come by( took me 8 years to get) and it was my trigger finger. it was also the 3rd extra part of the order and the last part of the night.


Delw

[RICHARD ZASTROW]

Having a file stuck in your chest isn't a real good feeling either.

Dick Z

[Delw]

Originally Posted by ad64075 I agree! More often we face similar issues with large OD threads and having operators manually deburr them, which presents its own set of problems. We have researched solutions extensively and determined that most (if not all) applicable deburring tools require rotation (live tooling). On our live tooling machines we have already accounted for deburring, it's our standard lathes that cause grief.

Theres a few ways to deburr threads on a lathe. ( if you dont use those forming inserts)

turn od or id
cut thread to high limit
turn od or id again
finish thread to mean dia.
this will usually break the burr off and give you a nice clean burr free part.

one way we also done this is mount a round wire brush to a tool holder.
then
turn od or id
cut thread to high limit
hit with wire brush
turn od or id again
finish thread to mean dia.

there are many ways to do differnt types of materal, Brass and alum I use a fine brass wire brush. some times on small brass I use those black hard bristle brush's. the rest depending on how big the burr is, sometimes stainless wire brushs etc etc.

I got this idea way back when, when I had to deburr all out threaded parts cause the deburr guy went on vacation for a week. since I deburred threads on different hardness's of wire brushs I figured why not put on in the lathe.
they wont scar parts up because you move it with a feed rate and you can adjust pressure plus the Spindle is turning, this gives you a very nice clean even finish. also use collant ( very important.)

Delw