geometric tolerance value

[4Ed]

Hi,

When starting a new part that will have a pattern of holes and where no tolerances are established yet on both the part with holes and the mating part. How do determine the geometric tolerance value at max material condition on the part with the holes? What are the questions you have to start with? And again how do you determine the limits on the hole that has no conventional tolerance yet except in the sheet metal title block, so to establish the geometric tolerance value? The only given is on the mating part the holes are for a standoff, so it's size is nominal but it's location tolerance isn't established yet either.
Not a student this has always bother me on new parts, do you go with the sheet metal tolerance in our title block .xx = +/-.03 and .xxx = +/- .010?

thanks...

 

[CheckerHater]

If your parts are sheet metal connected by rivets or bolts with nuts, start with “floating fastener formula”:

[smallest hole dia] = [largest bolt dia] + [positional tolerance]

Or

[positional tolerance] = [smallest hole dia ]- [largest bolt dia]

So, your bolt is standard, say ¼, so it’s .250 or less,
You pick 9/32 hole; your punch is .281, title block tolerance +/-0.010, smallest hole .271
[positional tolerance]=.271-.250=.021
Your positional tolerance is POS DIA.021(M)

But because you have a formula, you can have infinite number of different solutions.
You can play with numbers according to your functional and/or manufacturing requirements.

Also, to give your shop the most freedom, you may add your size tolerance and positional tolerance together and specify hole DIA .281+/-.031, position POS DIA.000(M).
This way, the larger the hole is, the larger positional tolerance becomes. So DIA .312 hole can have actual positional error of DIA.031

 

[KENAT]

Start with what your functional requirements are, however if alignment of 2 parts to each other is critical then using the fasteners to do it may not be the best approach.

Like Checker Hater says to actually calculate the values use the formulas (ASME Y14.5-1994 has them in appendix B FYI).

Then make sure they mesh with likely manufacturing tolerances/process capability.

Good point on the 0 position too CH - some shops may not understand this well but if they don't understand that then they don't really understand non zero MMC anyway.

Posting guidelines faq731-376

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

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

 

[4Ed]

Thanks for clearing that up. Although, they entered my mind in my old job all the time it also was presented to me at a job interview where the interviewer gave me a +/-.13 tolerance and wanted the positional tolerance value. I asked what it was mated to in order to use either fixed or floating formula. Anyway, he shown me the Pythagorean theorem switch to the square root of .26sq'd + .26sq'd = .1352 = DIA 0.37 positional tolerance. Although, I loved how easy it was, and I think only can work with bilateral tolerance, I can't stop thinking about the mating part and how you can assign a positional tolerance to something without knowing how it fits together?

 

[KENAT]

So the interviewer wanted the literal translation of a +- dimension to a positional diameter, in itself fair enough.

However, to actually properly assign the tolerance values you do need to consider what CH put (and what it seems like you were already thinking).

Posting guidelines faq731-376

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

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

 

[4Ed]

Honestly, at the time I drew a blank. I study WOW tolerance approach but not positional tolerance and couldn't answer the question at my interview. At my old job most parts were similar to older parts and to be completely honest we hardly ever used GDT for sheet metal only for machined parts.