The thing you are asking for (a simple comparison to see if the interference volume is within 2 cosmetic threads) seems so obvious to us who use the software all the time, but PTC PMs that spec the software don't use it, they dabble only, so they don't think about the implications. That means we have to find these convoluted workarounds. Well, here's one for you.
Most of the time I just coast through the interference checks and ignore the fasteners. However, if I know I'll be doing a lot of checking, and a lot of fasteners, I'll use these relations. Works well for cuts that pose as holes (just modify the diameter), but if you use the "HOLE" features, then you'll need to add a cut to consume the inside area where the threads are. Drive the diameter with a relation.
In the PART - create these relations. I paste this whole thing with a long list of common bolt sizes I use. (Sometimes I'll delete the ones I know are not applicable in this part.) Yes, it creates a lot of extra parameters, which is part of why it's convoluted. Oh well. Save the relations, then open it up again and delete the first one, Holethreads=1. That assigns it within the model, but removes it from the relations so it can be assigned at the assembly level. It will give an error if you past in the relations without that one the first time. (I know, it's just a backward way of establishing a parameter.)
In the ASSEMBLY - create these relations. The :X number is the part assignment so it carries the requirement for threads or for clearance (line to line) to the parts.
In the Assembly you can change the one parameter - either in the relations like here (or in parameters or program) - then regenerate. For Hole features where you add a cut to consume the thread area, when you regenerate with "material size for threads" you will get this error on regen. Just ignore it.
If you do interference checks a lot, then it's worth the effort, IMHO. Anyway, it's a workaround.
It's a hassle, but it's not that bad if you save all the relations in a text file so you can just cut and paste then change the dim params to make it work. Especially with a lot of patterned holes, it saves verification time. Also, if you have a lot of fasteners in large assemblies where zooming in and out for verification is a hassle for interference checks.
I'm not aware of anything out of the box like in other CAD packages - see Solidworks, for example. Note how some thought was put into the competing solution - and a M10x1.5 coarse bolt that was mated to a M10x1.25 fine threaded hole is flagged in their process.
I suppose if you use PTC software and the intelligent fastener extension (IFX), then the issue is somewhat solved by the automated process of creating the clearance / tapped holes to match the fastener, but that still does not solve the issue of not detecting fastener heads interfering with the structure...
So my conclusion: you are forced to come up with some hacky work-arounds. For example, maintain a custom library of fasteners that have a "no interference" variant in which the cosmetic thread region is removed from the solid and then do a swap-out using interchange assemblies.
Maybe it was already obvious, but I just thought of it: you can "solidify" the cosmetic thread surface and remove that volume from the solid:
I suppose another thing to consider is whether you need to worry about the fastener parts at all?
I.e., "prepare" for the interference check by turning your parts with internal holes into the "no-interference" versions where their cosmetic thread volumes are removed...
Anyway, good luck! and do let us know how you solved the issue.
