What's new
What's new

Need BEST PRACTICE for last thread deburring on machine

thetree

Aluminum
Joined
Apr 27, 2010
Location
mentor, ohio
Good Morning Everyone.
We make a number of steel parts that have a similar feature. They are mostly fine threads (1.00 - 1.5 diameter) up to a shoulder with an undercut. We usually end up with a last thread runout that is thin and hanging loose, either pushed out into the undercut or back into the thread. This "burr" can be up to 1/4" long and troublesome to remove.
Do any of you have the same problem and how do you handle it? I am spending a lot of time removing these by hand.

Thanks, Dan
 
i assume your undercut is a perpendicular groove to the shaft with no chamfer? i always have a 45 deg taper on my undercuts, then run the finishing tool back over the taper and then run the tool back over it again on fussy parts where minimum burr is required
 
Yeah it's not drawn with a chamfer and it's one of those companies who will reject for it. Also, small changes like that require 6 months of meetings and red line drawings and BS just to get it changed.
 
Use up the tolerance of your undercut and stay shallow. Im not sure what would happen, but what if you undercut after threading cycle?
 
the only other thing i could suggest then is if your on a mill turn to go in there with a little endmill or something and mill the end of the thread off in a way that doesnt stand out too obvious.
 
A pair of snips and a hand file while the part is rotating in the spindle after the cycle.
I'd like to know a sure fire way of deburring threads too. It can be such a P.I.T.A. sometimes.
 
A small 45 deg chamfer of height equal to the thread height at the end of the thread may work. It doesn't amount to change in drawing. Undercut / chamfering to be done before threading.
 
If you put a 30º chamfer on the undercut no one will even see it as a separate feature from the thread form, even on a comparator. Run the tool 2X once before the threading tool once after the thread is cut. It works for me.

Robert
 
Hi thetree:
This is a nuisance problem that all of us who do turning for a living knock up against over and over again.
Here are the solutions I (and plenty of others) have come up with over the years:

1) run the undercut, then the thread, then the undercut again, then the thread last pass again, repeating this sequence as many times as it takes to get a clean thread.
This works quite well on a great majority of steels, but has not been that successful for me on very ductile metals like 6061 aluminum or C110 copper.

2) make sure the chamfer at the trailing surface of the undercut is 45 degrees and not 60 degrees.
This makes the burred part shorter and easier to manage.

3) Higbee the last thread.
If you're unfamiliar with the term, it refers to a deliberate operation to remove the first (or last) thread by machining (usually milling) it away and is extensively used for threaded couplings of all sorts; fire hose couplings are a good example.
Clearly you need a live tooled lathe to do this and if you are using an axial live tool you have limitations on how you can mill it.
You need to use a tee slot or Woodruff cutter so the shank clears the threads and you can obviously only use it on fairly short threads.
With a radially oriented tool, you'd need to use a ball cutter and write a milling program that's a bit more involved than that for an axially oriented tool.

4) you could post process it away; handwork as you're doing now, wire wheeling or flap wheeling it away, tumbling, shot blasting etc etc.

Those are your choices; the nature of the run will decide which is the best fore a given circumstance.

I almost always do #1 and #2 first, because they're so easy to implement and they work well so often.

Cheers

Marcus
Implant Mechanix ? Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
Clarus Microtech

Oh yeah: make sure your tools for the threading and the undercut are SHARP!!
 
Some interesting solutions described here. I too have the same issue with a hardened 8620 shaft that I manufacture. I have tried the undercut, thread, repeat undercut, repeat last threading pass, and the results are improved but still not ideal. Usually I grab the offending burr with a small needle nose to remove as my cycle time per part does allow a small amount of time for manual removal, but a automatic solution sure would be nice. Nice to know I'm not the only one who fights this.LOL
 
I like the suggestions made previously but to throw out a bit of an "alternative" idea to the mix:

If you have a tool holder block available, you could put some sort of deburring tool (wire brush or abrasive flapper wheel) and feed it at just the right location and run the RPM up as needed after it's fed into location. It may require fabricating a holder to get just the right size and angle. At least then it can be done in the machine, and hopefully unattended.
 
After the "undercut, thread, repeat" to minimize burr, run a small deburr bristle brush in there to take off fine burrs.
Another option, thread mill the threads...
I have used both these on mission critical 316 SS parts that were not allowed any burr at all. (And we know how 316 likes to hang on):ack2:
My .02
 
You don't technically need live tooling to higbee a thread (or around my area we call it thread-clipping).
I've only ever done this when there was at least some sort of chamfer at the beginning and end of a thread.
Use a grooving tool with an insert wider than your thread, use G32 to control the tool to cut the same angle as your chamfer. Its kinda hard to explain but if you understand that G32 allows you to move the tool in any direction you want at the same threading speed and start point then you're pretty much good to create some code.
It is easier to explain if we use the front of the part as an example (but I have clipped both the front and back of threads).
I would paint the ragged-edge of my thread with a marker. Program the G32 to start away from the part and move towards the part in a straight line (to make sure everything was up to speed). Once my tool reaches Z0 then just move the tool at an angle that matches my front chamfer and off of the part. At this point I usually wasn't even touching the part... so I would adjust my offsets X down and Z in. And run the G32 again. Look at painted edge. Adjust offset. Repeat. Once I was happy with the higbee/thread-clipping I would take the numbers from the offset and use them to change my program numbers.
I think it only took me 45min the first time I did this... so its not that hard. And like I said before, I've done both the front and back of threads this way.
 
A) I'm certainly not seeing how a chamfer on the back end could be a problem.
The part of the thread that you wunna take away Shirley aint gunna have any holding power...
How and why are they checking to see if it is there?
Shirley there is no application for it.

B) If a simple chamfer aint allowed - a Higbie would be WAY more noticeable!

C) Can you thread roll it?


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

Think Snow Eh!
Ox
 








 
Back
Top