Determining Acceptable True Position for the FCF

[BodyBagger]

I understand how to calculate the true position given the actual x/y dims and then to say if the part is acceptable or not based on the TP allowance. What I am trying to understand how does the designer determine the amount of acceptable TP for a situation? I guess what I am looking for is the process a designer should follow to determine the acceptable TP for the FCF. Feel free to use the following example if it helps to explain.

Print Drilled Hole Size = Ø0.781 ±.010
Bolt = 3/4"-10 x 3.25 (passes thru the plate into threaded hole)
Plate thickness = 2.5"

I hope I did not over-complicate the question...
Thanks much for any assistance.
BB

 

[pmarc]

BodyBagger,

It looks like you should use fixed fastener formulas for positional tolerancing. If you have access to Y14.5 standard (1994 or 2009 editions), please take a look at nonmandatory appendix B. B4 and B5 are the formulas you are looking for.

 

[BodyBagger]

I will reference the sections you mention in the 1994 which I have now, and have just ordered the 2009 for good measure.

Thanks for your input.
BB

 

[KENAT]

Look at appendix B in ASME Y14.5M-1994 or equivalent.

It varies for floating (nut & bolt) or fixed (threaded hole pattern in part & screws) situations.

thread1103-221602 4 Sep 08 3:26 even has some worked examples.

Simplistically, you calculate the clearance. For a fixed fastener this has to be split between the 2 parts. For a floating fastener both parts get this value.

E.G.

#4 (.112) screws floating in .140 minimum dia hole:

.140-.112 = .028 'clearance'. Now you could divide this equally as .014 dia pos on both. Or, you could take into account that threaded holes are 'harder' to make and don't benefit much from MMC (arguably in some gageing situations), while the clearance hole is easy to make and benefits from MMC. In this case you might assign more to the threaded hole, perhaps .016 with .012 to the clearance or similar.

#4 (.112) screws floating in .140 minimum dia hole:

.140-.112 = .028 'clearance'. The holes in both parts are assigned .028 dia true pos tolerance.

The above is a short explanation of how to Analise it.

To design it really well you need to know standard tool sizes, not just drills but also ideally Counterbore tools if applicable (there are tables in machineries - just be aware that the sizes for small fasteners in 'close clearance' almost require match drilling). Also some appreciation of the process capability for making the holes and probably some other stuff that doesn't pop into my head right now, such as maybe inspection.

There are usefull tips too like, don't try and use threaded holes for position alignment or parts. Also there are tricks for handling countersunk fixed fastener situations which I've posted before but would probably confuse you right now.

Important thing is that while function is the primary driver, don't' forget manufacturing and inspection.

(I've rushed this a little, so sorry for any errors.)

Posting guidelines faq731-376

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

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

 

[BodyBagger]

Is the tolerance for the hardware ever taken into account? For example, the 3/4 hex bolt has a MAX body diameter of 0.768 according to Mach Handbook.

Thanks again,
BB

 

[BodyBagger]

Sorry, I spoke too soon. I see in the Appendix "b" the formula included the hardware MAX diameter.

Thanks

 

[KENAT]

Which handily, for fully threaded fasteners, is the same as the nominal size.

Posting guidelines faq731-376

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

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

 

[KENAT]

Well, if you take MMC into account, then with that +-.010 on the hole diameter I think it's workable, since a hole that size will typically be somewhere around +.010-
.001 if you believe in the old standard drill tolerances.

Apply around .014 to the threaded hole, I don't like to go less without talking to the shop, and you're left with .007 for the clearance holes + all that MMC allowance.

Now, that is a fairly thick plate so you almost certainly want to spec a projected tolerance equal to the plate thickness on the threaded holes. This effectively tightens the tolerance on your threaded holes, so you may want to go a little higher than .014.

I suggest you start looking at your (shops) process capability and adjusting accordingly.

Where did you get the hole tolerance from? Is the hole size set or could you adjust it if need be? If your shank 'MAX' .768" is correct, then you may need to increase your hole a bit or your tolerances may get tight.

Posting guidelines faq731-376

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

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