Thread notation drawing 5

[dizork]

Design - shaft partialy threaded with external thread 1/2-20 UNJ.

I want to minimize fatigue failure by having the thread taper off at the point where the thread terminates on the interior portion of the shaft, versus having the single point cut a full rotation at the end of the thread.

Is there a standard callout for this operation?

 

[CMfgE1]

I have not come across such a callout. Maybe somebody should develop a good standard to follow. I would think that if you specified the start point of the taper and the end diameter (in this case the minor diameter of the thread)
that should be sufficient. You would have to be specific so as not to confuse the machinist into thinking it was some sort of tapered thread. I would highlight the detail on a drawing and use notes on the side to explain. Or a cross section with dimensional callouts would work to.


Maybe you just started something new!

Good Luck

Quote: "Its not what you know, its who you know" - anybody trying to find a decent job

 

[pennpoint]

dizork
If you are using a thread cutting die you should not have a circumferential cut at the end. The die starts as a taper and will end as a taper. Look at any pipe or screw tread.
BTW, having a circumferential groove at the end of the thread can profide some stress relief if a small radius is allowed in the bottom corners.
If you are machining threads on a lathe you should have a bit of run out to exicute the thread ending. Run out is a small gap where the thread ends to where the maiting component seats. Again provide ample radius there at the bottom of the runout groove and you should be fine.

If I have miss interpreted your meaning forgive me.

Best Regards

pennpoint

 

[dizork]

Thanks for the replies and good suggestions. For clarification, this part is being cut on a lathe with a radius point UNJ insert. This type of insert if allowed to cut a revolution without feed should leave a circumferential groove with a radius bottom (current parts). Unless I find some type of standard, I will have to make something up and try to detail it as best I can.

On a side note.
These are wheelchair axles. Our marketing guy is a wheelchair user and of course managed to break one. Here is the funny part. A local University’s test lab built a fatigue test fixture which failed before the axle. Maybe I will have marketing do all the testing from now on....NOT!

 

[Cockroach]

Dizork, sounds like you are clipping the box threads, I'm not sure for your original post. It sounds like it.

In the oilfield, the typical convention is to call out a quick start, which is simply grinding or cutting the minor to major diameter for about 1/8 rotation on the box. In this regard, there is no standard but a practice developed out of design concerns.

I'm not overly surprised with the lab results. Your marketing guy could of had a faulty shaft, perhaps a minor crack at the root of the thread, material issue, perhaps the shaft was somehow overloaded, etc. If you statistically monitor the population of failure and their mode, you would probably find the shaft to be of acceptable design given the loading.

Good luck with it.

Kenneth J Hueston, PEng
Principal
Sturni-Hueston Engineering Inc
Edmonton, Alberta Canada

 

[Screwman]

I would specify that the thread be rolled, nut cut. Right away, by doing that you will greatly increase the fatigue life, regardless of what you put on a callout for the thread runout. Thread rolling is a great way to improve fatigue properties and in most cases you will be able to set up a rolling attachment right on the lathe.
If that is not an option, I would specify that the thread root must runout over a length of not less than three thread pitches.

 

[rorschach]

I agree that your best bet woulkd to put a groove with a large radius at the bottom at the end of the thread for the tool to run out into. Thread rolling is also an excellent idea. Another idea maybe to approach this from a materials point of view. Perhaps 17-4PH H900, or quenched and tempered tool steel (maybe D2 or O1?)

 

[jrgreen]

Dizork,

What model wheelchair were you talking about in your side note?

 

[BillPSU]

If you are making the thread in-house on a CNC machine the programmer can add the tapered lead out to the threading tool to the CNC program. Trying to call out such a thing on a print will be fairly difficult and how it would be measured on the part I haven't a clue.

I'm not sure any of the CAM systems can automaticly generate the proper CNC codes to do it. This will probably have to be manually programmed and not with a canned cycle thread process but with individual threading passes.

Over the years I have cut face thread/groove and removed the first thread on an OD threaded part with a grooving tool used in a threading cycle with a threading cycle to withdraw the grooving tool from the part.

 

[unclesyd]

Guess what I found in my father's books, one dated 1922 the other dated 1931 concerning threads on shafts.

The callout is "Threads Full to Taper" both books show exactly that in a pullout with the arrow pointing to the position where the taper is to start.

Doing some checking I found the same notation in a reference to creep and fatigue testing coupons from US Steel Research labs.

 

[BillPSU]

unclesyd

Does it give an angle or the rate of pullout(in/ft)?

 

[unclesyd]

I don't see any notation for the amount of taper called out on the threads. Just looking at the drawing from US Steel it would correspond to the following.

Just talked to an old machinist and he stated he usually used 1/4"/ft based on the diameter of the part being threaded. He also stated this was not always possible and the norm was to taper out in 1 1/2 to 2 revolutions of the part being threaded if possible.

None of my books have good indexes so I’ll keep looking. I will try to get some information from some people who do single point threading for living.