Jlang, welcome to my world.
I (and my contract colleagues) frequently get asked to check drawings that have already had components made from them which 'worked' but a quick tolerance analysis of will reveal potentially large interferences. Sometimes it's prototype batches but sometimes its items that have been in production for some time.
Philosophy here seems to be, if you can build one prototype and it fits together then you're good to go no need to bother about tolerances before or after. This bites us in the a$$ every now and then. It's especially bad if we change machine shops or maybe split mating parts originally made at one shop across several, or sometimes if we have changes in our own assembly staff etc.
You haven't mentioned what the tolerance on the hole size is, you only explicitly talk about position. Typical drill tolerances tend to be -.001 +.004 (or more on the + as the drill size increases)
So, unless you specify tighter on your prints your .114 will likely be drilled by a 2.9mm drill (.1142) with tolerance of -.001 +.004. This means that it's likely that most of your clearance holes are oversized. This in turn buys you something on location - even if the old prints didn't explicitly mention MMC a larger hole at least accommodates more movement of the threaded hole.
Second, the thread value you give of .112 is a max, so in practice will usually be smaller than that, which again will help with fit.
So, even without exceeding the (assumed) stated tolerance you at least statistically have a better chance of fit.
Then as others hint at, you have the person putting it together. Even if they aren’t deliberately filing, reaming or otherwise enlarging the clearance holes, they may do so by forcing the screws in ‘chewing’ out the side of the hole, especially if the part with the clearance hole is thin and/or of softer material than the screws.
.0005 position on a non threaded hole is achievable, may not be cheap, but we have parts with that kind of tolerance, and tight hole size tolerance. However, these are mostly on precision pin location holes etc not for matching threaded holes. 0 position is legitimate if you invoke MMC.
On threaded holes I would not expect .0005 to be realistically achievable for reasonable cost. I have experienced colleagues who refuse to put less than .005 position for threaded holes and prefer at least .010.
I had some parts similar to yours where I had to make an updated threaded hole pattern (#4 I think) work with existing clearance holes. Based on the calculations I needed 0, or maybe slight negative (which is impossible) position on the threaded holes. I spoke to the machine shop, and bear in mind this was a precision part used on microscopes so the shop is used to tight tolerances, and the tightest they’d commit to was .003 positional on the threaded holes.
So in this case I was not able to guarantee fit at worst case, but did my best to minimize the chances of interference and relied on the factors above to ensure fit most of the time.
Simplistically conventional hole pattern calculations (as in ASME Y14.5M –1994 appendix B) assume worst case, in practice worst case is rarely achieved with actual parts so the parts go together much of the time. The problem of course occurs when they don’t.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:
