Chamfer call out on a threaded hole, where is it measured from?

[jdg1111]

Is the chamfer call out .015 x 45 (degree symbol)on an internal threaded hole measured from the diameter of the cylindrical hole feature or the major diameter of the thread?

Example: I have a 3/8-24 UNF-2B threaded hole and I want a .015+/-.005 chamfer on the edges of the letter Q (.332) hole. Please note that I am aware that the .357-.372 diameter chamfer is not an appropriate lead in for the tap but is required for other reasons.

 

[powerhound]

Can you call out the diameter of the chamfer?

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[jdg1111]

Of course and that would be a better way to clarify the design intent, however the question of where the original (.015 x 45 deg) measurment starts from remains.

 

[ctopher]

Cross section of thd hole. Measure diameter, angle, and start of angle. I would not measure from any part of thd, very difficult to inspect.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[MikeHalloran]

Because the thread is often cut after the chamfer, the tapping operation will generally destroy one of the circular edges that are assumed to exist when you specify a chamfer by a linear dimension and an angle.
So, there's nothing to measure.
So, linear dimension and angle is just a silly way to specify the chamfer on a threaded hole.
You could specify the chamfer that way, to be measured when it still exists, after chamfering but before tapping. ... but you can't know after tapping what that dimension was before tapping.
So, it makes much more sense to specify by angle and diameter of the intersection of the chamfer with the normal surface.




Mike Halloran
Pembroke Pines, FL, USA

 

[jdg1111]

Thank you Mike and PowerHound. I completely agree with your suggestions but to the root question, do you agree that the origianl call out starts from the cross section of the hole?

 

[MikeHalloran]

As for the original question, the design intent can only refer to the surface of the drilled hole that becomes the minor diameter of the internal thread. ... but the dimension would be to the intersection of the cylindrical surface and the conical chamfer. ... and production of the thread removes that material.

So the dimension is to a 'theoretical sharp corner' in circular form.
Since it's all but impossible to measure, the requirement is stupid.




Mike Halloran
Pembroke Pines, FL, USA

 

[ewh]

Bottom line, it is a vague callout. You could inspect it by measuring the diameter and angle of the countersink (chamfer) and trigging it back to the minor diameter, but this is assuming that the chamfer was supposed to be applied to the minor diameter. As pointed out, part of the chamfer has been removed when the hole is tapped. For this reason, it is better to call it out as a countersink, which can be measured after machining the threaded hole. I realize that this does not help with your situation, but perhaps it will help further your understanding.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[jdg1111]

ewh,

I agree and apologize to you and Mike. Effectively the part is blanked on a lathe and the edge that gets this chamfer is there only to remove the burr left from the cutoff process. It is not intended to provide your typical thread lead in as the design intent is to have no chamfer after threading at all. Having the chamfer call out on the drawing is intended only to prompt the machinist to include this step in his/her programming steps. I could have placed a note to "break edge MAX .372 dia) but there simply wasn't enough room on the drawing to fit that. The machinist interpreted it as starting from the major diameter of the thread and face and bet me a pizza that they were right. Not wanting to pass up on a free meal I was hoping to get a consensus from others as to the definition of the start point (cross section of the hole to the face), not when to measure it, or if the design intent is "silly" or "stupid" as Mike put it.

 

[powerhound]

In general, I think the machinist's interpretation was wrong BUT he may have made that conclusion because he knew the chamfer would be removed in the threading process and assumed that you actually wanted one there. If this was the case then a note or diameter may have been a better option. When specifying threaded holes, using an angle and diameter tends to be more clear since it removes the question of where to begin measuring the angle.



John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[jdg1111]

Thank you Powerhound. I will send you a slice of the winnings.

 

[MikeHalloran]

I'd have to say the machinist was "not wrong", given the ambiguity in the drawing supplied him/her. You should buy the pizza anyway; the ROI will come later.

Least awful way to specify, I think, is "CSK 90deg to .372in max dia" or similar, but it should be on the process sheet if there is one, or on a raw/intermediate "make from this" drawing, since the feature doesn't appear on the finished part in an inspectable form.



Mike Halloran
Pembroke Pines, FL, USA

 

[jdg1111]

I think your right in that the best place to have it would have been on the process/"make from this" drawing as you have it called out. With the "make from this" drawing in process and the finished drawing clarified I think the machinists and I will split the pizza and each send you a slice.

 

[KENAT]

If you're drawing to ASME then it's debatable if a feature that will subsequently machined off should even be on the drawing, almost certainly contravenes 1.4(e) of ASME Y14.5M-1994. So like Mike says probably best as information on the traveler or 'make from' drawing etc.

This being the case I'd buy the machinist the pizza just to buy the good will;-).

Posting guidelines faq731-376

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

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