Countrsink lead-in for internal threads--is there a std?

[wgchere]

I'm looking for a standard or information regarding the countersink on an internal thread.

I have an engineer who insists on specifying a countersink on all internal threads. I have contended that it is standard machine shop practice to put a 90° csk as a lead-in (he always specifies 120°) a little larger than the major dia.

"Prove it!" he said.

I thought I had seen it in Machinery's Handbook, but I couldn't find it, and a search of several hours and many keywords turned up nothing--except this site, which I had never heard of before.

Anyone have any info/ideas?

Thanks,
WGC here.

 

[diamondjim]

I know that the 120 degrees is typical
for drilling for heli-coil inserts, but
our shop normally chamfers 90 as you
suggest for standard internal threads.
I have not seen a standard for countersinking
tapped holes for threads but have read
that the c'sink diameter should be greater
than the major diameter of the thread.
Will look forward to other opinions.

 

[MikeHalloran]

Old timers will normally csk a thread, if they are making a part for their own use. But when making parts for someone else, any shop that has ever worked in a highly regulated industry, or is subject to inspection, will make parts _exactly_ like the print. You can't rely on 'standard machine shop practice'; there is no such thing. You can have any csk you want, but you have to specify it on the print.

That said, I think the 120 deg csk used to be customary, but CNC shops have adopted the practice of using the same 90 deg cutter for spot drilling, countersinking and chamfering, to save tool change time. That's the 'new' custom.



Mike Halloran
Pembroke Pines, FL, USA

 

[ewh]

I have always used a 90 degree c'sink on threaded holes as good practice, but I know of no standard (other than a company standard) that requires this.

 

[BillPSU]

I use a 1" x 90 degree spotdrill and generate the chamfer using it. This gives better hole location and the chamfer all at the same time. I've never used a 120 degree as a drill will again hit on the point and wander and I have never seen a 120 degree anything as a standard tool.

 

[CorBlimeyLimey]

http://www.jjjtrain.com/vms/cutting_tools_csinkborespot.html#2

Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[alexit]

If you layout the thread in CAD or on paper (if your good) you will see that a standard 60° profile thread (UNC, UNF, METRIC, etc.) will have a much cleaner entry/exit with a 120° chamfer than a 90° one. (The 90° has a longer interaction leaving a greater lenght of material to become a burr.)

Your Engineer is right, buy him a coffee then tell him to get back to work.

 

[tbuelna]

The purpose of c'sinking an internal thread is to prevent a raised "burr" at the imperfect lead thread. A burr will prevent the mating part from sitting flat on the surface with the threaded hole.

 

[diamondjim]

It also helps to get the bolt started
or aligned.

 

[JDana]

In electronics assembly it also prevents the raised burr from breaking loose and shorting something out.

 

[CoryPad]

While burr prevention is an important reason to chamfer holes, the major reason to do it is to provide clearance for the bolt underhead fillet.

Regards,

Cory

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[diamondjim]

Cory,
Isn't the chamfered washer supposed to take care of
the bolt fillet radius problem?

 

[Screwman]

Cory is right on clearance holes. It is not standard practice to use use a chamfered washer except in aircraft.

On tapped holes the issue is that without a chamfered hole there is a possibility of a burr that will extend above the bearing surface. When the mating part is placed on this it can be forced down, effectively 'closing' the thread and creating an increased potential for cross threading.

I have not seen any standard practice to chamfering tapped holes and I looked for it just like you have. IMHO the best way to do it (unless there is a definite reason to specify a specific configuration for perfomance resons) is to simply indicate "chamfer all tapped holes" and leave it open for the vendor to make them the easiest and lowest cost way he can.
We have not found a significant difference between 90 and 120 degree holes for cross threading and we have tested for just that condition. The experimental noise was much greater than the impact of the chamfer angle.

 

[codeeng]

For screws and bolts this practice is called pointing and most standards specify this as being optional by manufacturer. Since there is no standard for tapped holes you'll not see this specified anywhere. My experience is that if its not on the drawing it generally doesn't get done. Your engineer has a valid comment.

 

[wgchere]

Thanks to all. It looks like we ought to have another boilerplate note something like:

ALL TAPPED HOLES SHALL HAVE A CHAMFER OF DIMENSION MAJOR DIA+.010/+.020 X 90°-120°.

(And I was so sure I was right... darn! I probably ought to hire him back...)

 

[diamondjim]

If you are calling out a chamfer,
shouldn't it be 45 to 60 degrees.

 

[wgchere]

Does this sound better?

ALL TAPPED HOLES SHALL HAVE A 90°-120° CSK WITH A DIAMETER EQUAL TO THE MAJOR DIA +.010/+.020.

 

[diamondjim]

Yes that is better.
Sorry to be picky.

 

[wgchere]

No problem. I figure nearly all the people logged onto this forum are picky by nature or we wouldn't be searching Websites for answers—we would just do what seems expedient appears to work. I imagine most of us are also pretty opinionated!

 

[METALART]

There is a chart, have one and use it. It is a machine shop practice to chamfer all holes, break all edges, no burrs. 120° is hard to control, gets big in a hurry.