Best tooling / machining strategy on turning all thread into dog point set screws

[doug925]

Good morning all.

I have a RFQ for 300 pcs of the part show in the pic.
The customer is asking me to quote the labor only, and he is supplying 4 each, 12' sticks of 3/16-16 allthread.

Turning the dog point, chamfering and parting off are easy....
Though, after 20+ years in the trade, I still do not know a decent strategy for chamfering preexisting threads, and NOT roll a burr into the starting thread. Once a burr is made, the only way I know to get rid of it is to spin a nut (or thread chasing die) back across the burr to remove it.

So, Practical Machinist, I ask:
What tooling or cutting strategy should be employed (in this case) to prevent a burr from being formed?

This will be run on a bar fed Genos, C axis machine.

Thank you in advance for any help you all can provide.

Doug.

 

[ewlsey]

They already helped you by chamfering at 60 degrees instead of 45. I'd just chamfer with my parting tool and maybe hit it on the convolute wheel to take the sharp edge off the thread.

 

[WILLEO6709]

why on earth would you buy allthread? turn the od of round bar, thread after, cutoff, and slide a drive slot in it. I would think post threading would take the most deburring out of it.

 

[Milland]

Sharp a tool as possible for generating the chamfer to minimize burr generation, plunge cutting should help.

Do you have any way to set up a small powered tool on your machine? If you can get a small (~2") fine SS wire wheel to push into the front/end of the thread prior to parting off that should take care of any remaining burrs.

 

[doug925]

why on earth would you buy allthread? turn the od of round bar, thread after, cutoff, and slide a drive slot in it. I would think post threading would take the most deburring out of it.

Willeo,

I agree with your approach to the job; however, I have to quote the job based on the customers request. I will quote them on turning them from round, but I need to consider the best way to handle this as requested.
Besides, I need to learn how this might be best accomplished for my own edification.

Thanks,

Doug.

 

[doug925]

Sharp a tool as possible for generating the chamfer to minimize burr generation, plunge cutting should help.

Do you have any way to set up a small powered tool on your machine? If you can get a small (~2") fine SS wire wheel to push into the front/end of the thread prior to parting off that should take care of any remaining burrs.

Milland,

I can rig up a wire brush in one of my axial live tools. Thanks!

 

[DDoug]

Look at the contact area (in the collet) of all thread, and then
look at the contact area of solid material.

Explain it to the customer, feeds and speeds will have to be reduced greatly to not mar the tops of the existing threads in the collet.

"reduced feeds and speeds" = higher price.

 

[Kyle Smith]

Though, after 20+ years in the trade, I still do not know a decent strategy for chamfering preexisting threads, and NOT roll a burr into the starting thread. Once a burr is made, the only way I know to get rid of it is to spin a nut (or thread chasing die) back across the burr to remove it.

Best way I know is to "tell" them you used the all thread, then run them out of barstock.

Coming from the largest Ø to the smaller Ø helps, instead of the conventional opposite approach. In example, for the end with the dog point start at major Ø and turn towards the dog point.

 

[Limy Sami]

Doug,re damaging the althread - has that lathe got a subspindle? .....if it has, can the subspindle slide in relation to the collet or chuck, ...in the same way a carriage on a manual lathe does when threading?

 

[art.h]

why on earth would you buy allthread? turn the od of round bar, thread after, cutoff, and slide a drive slot in it. I would think post threading would take the most deburring out of it.

Because as the secondary you have no right to change the basis of the order. While I agree your choice of methods makes more sense, without the express permission and new/altered dwg. and PO you would be violating the agreement. and no matter how trifling this could be used against you in any future legal matters.

 

[Mtndew]

why on earth would you buy allthread? turn the od of round bar, thread after, cutoff, and slide a drive slot in it. I would think post threading would take the most deburring out of it.

It's customer material.

 

[triumph406]

I've never damaged a thread in a collet yet, we do a lot of parts using all thread, never been a concern.

 

[John Welden]

No Bid. There has to be better jobs you could be doing than this kind of crap?

 

[Milland]

I've never damaged a thread in a collet yet, we do a lot of parts using all thread, never been a concern.

I have to agree, that's a decent sized part with minimal work done to it, the threads shouldn't be damaged from appropriate collet grip.

 

[Limy Sami]

No Bid. There has to be better jobs you could be doing than this kind of crap?

If the price is right John ????? ..a $ in the pocket is still a $ in the pocket, ......and it may as well be Dougs as the next guts.

 

[John Welden]

If the price is right John ????? ..a $ in the pocket is still a $ in the pocket, ......and it may as well be Dougs as the next guts.

Some dude supplying all thread for this job has to be some cheap ass that doesn't have a clue.

But if the price is right, you're right.

 

[Mtndew]

No Bid. There has to be better jobs you could be doing than this kind of crap?

Unless it's a VERY good customer and he needs them right away.
We take shit jobs all the time from one of our customers but only because they give us millions a year in work.

 

[FredC]

That 3/16-16 thread threw me for a couple of minutes, looked at the drawing and 3/8 -16 will not be so bad. It has already been mentioned that cutting from the od towards the center on chamfers minimizes bur not sure why but that matches my experience. Machining existing screws is done all the time for oil field fasteners, many times when it would be easier to make them from scratch.
http://www.practicalmachinist.com/v...-mills-and-lathes/threading-5c-collet-333689/
We used to make a 5/16 long 5/16-24 dog point screw 10,000 pcs at a time we had the all thread rolled then form tool profiled, drilled, broached the allen, and cut off on a screw machine. We deburred them with the fixture pictured on a wire wheel. Only took a couple of hours to do all 10,000. For 300 pcs I would not bother doing them on the machine with a wire wheel, if using a sharp finish tool and cutting from the outside in on your finish cut is not good enough drill a flat bottom hole in a piece of steel and burr them by hand it will only take a few minutes to do both ends on 300 pcs. The already rolled threads will have a slight micro hardness from rolling on the surface of the threads that will make them easier to machine and minimize the burr anyway.

Added a photo of set pcs used to set up the screw machine when the job repeats.

 

[Limy Sami]

Unless it's a VERY good customer and he needs them right away.
We take shit jobs all the time from one of our customers but only because they give us millions a year in work.

Exactly, and by the same token I've had plenty of good customers that became good - simply because I was to take on something others couldn't do in time or who thought the job a waste of time etc etc etc.


Mind you I've had som A holes from that work as well, ..but they didn't last long

 

[david n]

Doug
You're gonna have problems no matter what in that 304SS crap................you have live tools, use them. Put a chamfer mill in a radial tool?