I'll assume you're talking about mechanical fits. There are tables of fits in the Machinery's Handbook that delineate what the tolerances should be for various running, locational and interference (force) fits.
But if you are simply designing machines in the real world, you will get laughed at for using some of these tolerances, since many are ridiculously fine (in tenths). The tables are statistical and theoretical, usually without regard for manufacturing methods--that's where you come in. You can refer to these tables as a guidline, but keep in mind who is going to be making the parts and how. You want the machinist to use the easiest and fastest method to get a "good enough" fit for your application. Why lap when you can bore? Why bore when you can ream? Why ream when you can drill or punch? Why mill or grind when you can saw, shear, flame-cut, etc?
Also, remember that there are (or should be) default tolerances in the title block of your drawing that allow you to apply precision based on how many decimal places you use, without a specific callout. Remember also that (unless you are doing an anal-retentive government job) you can often simply tell the machinist what you want on the print, particularly if it's not a super-critical application. So, you can call out a hole diameter and say "press fit dowel" after it, and the machinist should know how to ream it for a good force fit for that sized dowel.
It is often just as important to be sure that the tolerance is wide enough as it is to be sure that it's fine enough. You don't normally, for example, need to dimension a 15-foot-long weldment with three decimal places of accuracy. The machinist will assume that it really does have to be accurate to +/-.005" and waste a lot of time meticulously machining the ends when it isn't necessary. If you're machining a part from a 1.0 x 3.0 bar of steel and you don't need it to be exactly 3.000" wide, then say so, or he'll be fly-cutting the whole thing (or bitching that the material came in at 2.994").
Another mistake that I see young engineers making is putting 1.000 +.005/-.000 on a hole and 1.000 +.000/-.005 on the shaft for a running fit. As long as the machinist stays near the median of these tolerances, the shaft will turn freely, but technically he could make the hole exactly 1.000" and the shaft exactly 1.000" and it would be perfectly within tolerance...yet a clearance of 0.000" won't turn worth a damn. There has to be a minimum clearance even with the *worst* case.
Having said that, to answer your question, most critical things that require tolerances can be found either in the fit tables, estimated through experience, or in the manufacturer's specs for the component parts. The tolerances (and surface finishes) for the housing bores and shafts for ball bearings, for example, can be found in the bearing catalog. The same goes for snap-ring and o-ring grooves, keyseats, etc. Purchased parts like these are already made at the factory within a specific tolerance that mates with those in the catalog.
Hope this helps.
Don
Kansas City
