but you may be able to use API ...
you're doing the same connectivity each time ... create new independent node, dependent nodes on one or two curves (that create the hole), or surfaces (that create the bore).
another day in paradise, or is paradise one day closer ?
I thought you could do something in API to increment selections (so long as things obey convenient rules).
It sounds like you're using spiders for rivets. I personally don't like this, and would rather model the rivets as welded nodes (ie rigid fastener) or with a CBUSH (if you think fastener stiffness is critical).
But then maybe you're doing what you're told ?
another day in paradise, or is paradise one day closer ?
yeah, I get what you're doing. My question is why make your FEM so complicated by modelling the holes ? Mesh the surfaces with the bolt center embedded, maybe refine mesh around these points, have co-incident nodes for the bolt, merge these two nodes. You'll get the load transferred via GPFB. [1] This models the fasteners as rigid ... if one fastener is seeing an unrealistic amount of load, replace with a flexible CBUSH.
There's a way to do what you want ... you just don't want to get the carpal tunnel (and the mind-numbing boredom) that'll result !
[1] Personally, I think this is overkill unless it's a very sensitive joint, and that it's usually enough to mesh the two parts and to obtain the load sheared from one to the other over some length (rib/frame pitch) and say fastener load = P/n = P/(L/p) and maybe add some load peaking (peak is 1.5 (2?)* average).
another day in paradise, or is paradise one day closer ?
I reckon you can either
1) mesh the model as you feel needs it (without meshing fastener locations), have common mesh on both parts (effectively welding the parts together). You're working with 1000s of fasteners, "surely" its reasonable to assume some load distribution between fasteners, and so base calcs on the average load (so much load is sheared over so many fasteners). or
2) mesh the two parts as you see fit, and join the meshes at a select number of locations representing the fasteners (so you're stitching the two parts together). Clearly a ton of work. You can embed locations into the mesh (ie place nodes where your fasteners are), still a ton of work, particularly in cleaning the mesh distortions around these points. Then you'll have specific fasteners modelled … merging the nodes means a rigid connection, coincident nodes joined by CBUSH means a finite stiffness connection.
another day in paradise, or is paradise one day closer ?
solution 1 is quite an assumption, as it does not work for a complex or non-symmetrical geometry
solution 2, as you say is a ton of work. besides I don't recommend it to anyone merging nodes to represent a fastener; as this way you cannot dimension any bolt size since you don't get the forces at the fasteners.
all and all, the answers are moving appart from my initial question
with solution 2 you get fastener forces, and you hand calc bending if you thin it's an issue.
solution 1 has worked for decades (before we had computing capability to model 1000s of fasteners). It reflects the real world, where fasteners yield and redistribute load. As for complex geometry … pick the areas you're averaging over carefully.
another day in paradise, or is paradise one day closer ?
In Femap Custom Tools/Meshing/Hole to Hole fastener there is an API that allows you to select the top hole and bottom hole, then auto creates the spiders and the beam and property for the fastener. It might be a good start in automating your task, the source code is in the API directory for you to modify.
Also, there are some very talented API programmers over on the Femap forum on the Siemens website, you would likely get some advice and help in automating your task there. There is a link to the Femap forum under Femap/Help/User Community.
