fixed fastener calculation

[AndrewTT]

Attached is a fixed fastener question from a GD&T textbook. I am interested to see what answers this group can come up with.

---------------------
The part with the clearance holes (part 1) assembles on top of the part with the tapped holes (part 2) and is fastened with cap screws. Allow a tolerance of at least .030 on both the threaded and clearance holes, use zero positional tolerance, and specify projected tolerance zones.
---------------------

fixed fastener formula
H = F + t1 + t2

Givens:
clearance hole LMC
zero positional tolerance for clearance hole (t1)
fastener size (F = 3/8, .375)

Find:
clearance hole MMC (H)
threaded hole positional tolerance (t2)

While there are many possible answers I am interested in using all of the available tolerance (leave no meat on the bone). What is the optimal answer?

 

[pmarc]

There is no single and optimal answer to that question. If I understand the question correctly, each combination of H and t2 given below is ok.

(H) | (t2) |
------------|
.420| .045|
.419| .044|
.418| .043|
.417| .042|
.416| .041|
.415| .040|
.414| .039|
.413| .038|
.412| .037|
.411| .036|
.410| .035|
.409| .034|
.408| .033|
.407| .032|
.406| .031|
.405| .030|
------------|

 

[AndrewTT]

My answer was .420 (H) & .045 (t2), giving as much tolerance to the threaded hole as possible.

I had a few at my work whose answers were not in your table of possible answers. Just wanted to make sure I was doing the calc. correctly before I showed them the correct way to figure it out. Most came up with .405 (H) & .030 (t2). While not incorrect it does give more tolerance to the clearance hole than the threaded hole. I have read books from a few authors who would discourage this practice.

Thank you.

 

[mkcski]

pmarc nailed it (again). And driven by the virtual conditions which are assumed to be equal at MMC size.

Certified Sr. GD&T Professional

 

[3DDave]

Just thinking this through:

The fastener is nominally dia .375 along its entire length.
There is dia .030 projected location tolerance minimum on the threaded hole
(because it makes no sense to be the size tolerance of the threaded hole)
There is dia .030 location tolerance minimum on the clearance hole
(because it's the same interpretation as the threaded hole)

The MMC size of the clearance hole is dia .375 + dia .030 Projected + dia .030 = Minimum (MMC) clearance hole dia .435.
At LMC the clearance hole would be dia .450 and be allowed dia .015 more for a total of dia .045 location tolerance.

There is some conflict with the idea of zero positional tolerance on the threaded hole vs the dia .030 minimum tolerance requirement.

*************************************************************************************

Alternative interpretation (that the .030 minimum tolerance does not apply to both holes):

The fastener is nominally dia .375 along its entire length.
There is dia .030 location tolerance minimum on the threaded hole
(because it makes no sense to be the size tolerance of the threaded hole)
There is dia .000 location tolerance minimum on the clearance hole
(because it's the same interpretation as the threaded hole)

The MMC size of the clearance hole is dia .375 + dia .030 Projected + dia .000 = Minimum (MMC) clearance hole dia .405; similar result that at LMC dia .450 the allowable location tolerance is dia .045.

*************************************************************************************

I keep thinking I'm reading the question wrong, but I don't see where; the requirements look like they conflict.

Normally I look at the typical location tolerance that's been 6-sigma for whatever supplier/process produces the threaded hole, then pick the next larger clearance hole drill size that will accept the fastener plus the threaded hole projected location tolerance. This gives the MMC minimum location tolerance, which might be rounded to zero to build in a cushion when the maker misrepresents what their 6-sigma value really is. Then I look at bearing area and asymmetry limitations to set the maximum size of the clearance hole.

 

[AndrewTT]

3DDave, I double checked that I copied the wording of the problem correctly to my original post. That is how the problem is worded.

Here is the answer that the instructor's materials gives.
----------------------------------------------------------------
total positional/location tolerance = LMC (clearance hole) - F
= .450 -.375
= .075

assign some amount of this tolerance to the threaded hole (each hole must have at least .030 tolerance)
t2 = 60% * .075 = .045

fixed fastener formula
H = F + t1 + t2
H = .375 + .000 + .045
H = .420 (beginning of pmarc's table)
-----------------------------------------------------------------

 

[3DDave]

No wonder the students come up with a variety of answers.

I expect the word that makes the difference is 'allow,' which converts the interpretation into a MIN-MAX problem, which is only satisfied at one edge case instead of being the minimum. It seems especially crafted to be misleading so that the expected outcome is the student just memorizes the process.

It is distressing to see the arbitrary 60% value in the given solution. Had it been an arbitrary 70%, the answer would not meet the requirements. So it's a contrived answer that would fail if the LMC hole was smaller or the percentage was larger.

How about this version of the problem statement:

When the clearance hole is at LMC it should have a 'bonus' tolerance of dia .030 and an initial tolerance of dia .000 at MMC. The threaded hole has a projected tolerance.

What is the MMC diameter of the clearance hole and what tolerance is allowed to the threaded hole?

I will bet many more (maybe all) students will get the answer in the answer key than they did originally.

 

[pmarc]

What is the MMC diameter of the clearance hole and what tolerance is allowed to the threaded hole?

There would still be many answers possible to the underlined part of the question. Any position tolerance value within range <.000; .045> at MMC would work.

The question to this specific problem should rather be:
What is the MMC diameter of the clearance hole and what maximum position tolerance value is allowed to be speficied in the position feature control frame for the threaded hole (of course in order to always assemble both parts)?

 

[AndrewTT]

To be fair to the author there was nothing in the instructor's materials that said that was the only acceptable answer. Also, he actually had an answer of .415 (H) & .040 (t2) but used the format employed in my early post. I should have said "here is the format that the instructor's material gives".

 

[3DDave]

That improves it, but since there is a diagram there is no need to mention the FCF; since the clearance hole is specified mentioning the threaded hole is redundant. Also, there are six parts to assemble.

What is the MMC diameter of the clearance hole and what maximum location tolerance is allowed to the threaded hole?

What about the 60%?

 

[pmarc]

What about the 60%?

Most likely the author of the question liked this number and so it is.
Apparently the instructor prefers 53,(3) over 60.
Diversity is beautiful.

 

[3DDave]

What is 53,(3)?

 

[pmarc]

53.3333333333333.....%

AndrewTT said the instructor's answer for position tolerance for the threaded hole was .040.
(.040/.075)*100% = 53.3333333333....%

 

[3DDave]

I didn't see it originally because it was 4 seconds before my post and would have been edited at the same time as mine.

Still, without justification, it's garbage answer.

In accounting (3) is a negative value and a percent would still have a percent sign and comma separation for decimals is a decidedly European convention.

 

[JNieman]

I have never seen someone so sensitive to parenthesis.

I appreciate this thread. It was good following along and validating my understanding of the FFF.

 

[mkcski]

JNieman:
What does FFF translate to?

Certified Sr. GD&T Professional

 

[Belanger]

fixed fastener formula ?

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[pmarc]

JNieman,
How dared you use such devilish acronym!?

(Hopefully, this time the irony is evident).

 

[mkcski]

Did I miss a joke of some sort? Maybe Form Fit Function ???

Certified Sr. GD&T Professional

 

[AndrewTT]

I guess the real reason for my original post was trying to confirm how to calculate the total tolerance that could be divided between the two holes (clearance and tapped). The textbook I refer to says that it is equal to the LMC of the clearance hole - F. I could not find this same definition in appendix B (B.4) of Y15.4-2009. From what I read in B.4, in the example given T = (6.44-6)/2, the 6.44 = H, the 6 = F, so they are dividing up .044 tolerance between the two holes (either equally or unequally as the designer sees fit: 2T or t1 + t2). B.4 makes no reference to the LMC of the clearance hole.

So in summary:
textbook says TOTAL LOCATION TOLERANCE = LMC - F

ASME Y14.5 - 2009 says TOTAL LOCATION TOLERANCE = H - F

These are not the same, right?