implied specification

[Tmoose]

In the past we have specified a thread on a shaft for a bearing nut without specifying a relief where the thread runs into the bearing seat diameter. We have a note that all fillets to be 1/8 inch radius unless otherwise specified. The nut manufacturers generally spec an undercut with a max diameter a little smaller than the thread minor diameter, but no minimum diameter or radius in the undercut corners.

We got a shaft recently with an undercut whose depth matched the keyway for the bearing lockwasher ( 0.125/0.130 inch), significantly deeper than the minor thread diameter depth ( ~0.035 inch ). This is a product made since the 50s, maybe longer.

I know generally the rule is, and should be, make the part to meet the drawing. The shaft design guidelines etc are for the designer or engineer, not the machine shop.

But, are there some underlying implied tolerances for this kind of thing?

thanks,

Dan T

 

[flash3780]

You cannot cut threads without leaving some room for incomplete threads or including a thread relief. It sounds like your drawing is missing a thread relief (incomplete threads might booger up your nut).

The shop would have had to make an assumption about what is going on between the threaded surface and bearing seat diameter. From the sound of it, the deeper undercut that you're seeing is an extrapolation of the assumption of a thread relief to include your minimum radius.

You may want to define the thread relief on your drawing, so that you don't run into the same problem again.

 

[drawoh]

...

But, are there some underlying implied tolerances for this kind of thing?

Not to my knowledge. I must admit that I show undercuts to be an extension of the thread's minor diameter, without dimensions.

If your undercut is structurally critical, you should draw it out and apply dimensions and tolerances.

JHG

 

[desertfox]

Hi T.moose

I found this information on the screw thread undercuts:-

http://www.pmpa.org/technology/design/threadrelief.htm

Also in the uk BS1936 Part 2 1991 gives controling dimensions for thread undercuts.

Any chance you can post a picture like the one you posted in the "Broken Shaft Thread" I assume its related.
On the assumption it is that failure is a rapid shear failure and probably not a fatigue failure, that said I would like to see a pic of that shaft at 90 degrees to the one you posted.

Regards

desertfox

 

[KENAT]

The thing is, something like BS1936 is only relevant if you call it up on the drawing as I recall. If the drawing doesn't somehow reference a standard like this then there may not any explicit requirement.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[desertfox]

hi KENAT

Thats true, but when a tapped hole or external thread is called up, I have often seem just "M6 tapped hole" no tol and from that you would normally get a course pitch and probably 6H tol which are only implied.

desertfox

 

[flash3780]

...when a tapped hole or external thread is called up, I have often seen just "M6 tapped hole" no tol and from that you would normally get a course pitch and probably 6H tol which are only implied...

There are a lot of incomplete drawings in the world, but I think that a proper external metric thread call-out will include all of the details of the thread (i.e. lead-in chamfer, relief geometry, tolerance class, M or MJ, diameter, and thread pitch). It may be "understood" that if you call out a M6-1, you're referring ASME B1.13M, but perhaps not.

Many things like this are often defined in general specifications that companies assemble, but if you're not referencing such a specification, I think you should probably be explicit. If you leave any definition off of the drawing, the manufacturer can make the geometry however they'd like to - or not at all. As Kenat mentioned, if you wish to invoke a particular standard it may be best to do so explicitly.

 

[KENAT]

desertfox, to ISO standards if you just say "M6" you get the standard course pitch and you may even get a default tolerance class, I can't remember. So as long as relevant ISO standards are somehow specified on the drawing you're safe, even if they aren't explicitly referenced in most of the world they will be inferred.

To ASME standards you have to spec the pitch. We've had phone calls from machine shops in US wanting to know the pitch when the drawing didn't spec it.

The ASME thread specs, at least B1.1, actually say you should reference them on the drawing, but I suspect we've all seen a lot of drawings that don't and generally lead to acceptable parts. Thing is, if they make non acceptable parts, they may have an out and you have to buy them because you didn't explicitly spec what you wanted.

As I recall BS1936 wasn't a spec that got generally invoked without explicitly calling it up. That's the point I was trying to make.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[desertfox]

Hi Kenat

Yes I don't disagree with you, BS1936 crtainly wasn't heavily used as I remember on drawings either.

desertfox

 

[Tmoose]

Hi Mr Fox,

Thanks for the reference. Our parts group had sent me a link to that same PMPA reference within minutes of your post!

http://www.pmpa.org/technology/design/threadrelief.htm

I had to read it several times to be sure, but I think the wording that the relief should be "minimum .015" less than the minor diameter of thread" focuses on providing machining clearance, not maximum shaft shaft strength, similar to the nut manufacturers' tech info.
Dan T

 

[desertfox]

Hi T.moose

I Have had a quick look in BS1936 undercuts for external threads the tolerance on the undercut dia is h13.
To be more specific it depends on the diameter and pitch of thread.
So say an M10*1 thread the dimensions given for a undercut are:-

d-g= u/cut dia so 10-2.3 = 7.7mm diameter

the 7.7mm diameter would be subject to a h13 tolerance.

regards

desertfox

 

[mfgenggear]

It is better if the the thread data is explicit on the engeening drawing.

the relief must be specified to insure structual integrity.

many drawings I have reviewed and it is left up to the manufacturer to decipher, which can cause mistakes.

which is the mfg's problem but will delay your parts.
or is it?

my 2 cents
hth

 

[tbuelna]

tmoose,

Most bearing locknuts are 16 or 18 pitch threads. If your drawing has a general requirement for 1/8" fillets, by definition that would imply at least a 1/8" thread runout, which is 2P for a 16 pitch thread.

Shaft threads and keyways for standard bearing locknuts are covered by ANSI Std 8.2-1978.