Different ways of modeling fasteners 1

[admiral007]

Hello all,

I am currently reviewing a FEM. There is a critical section of this model in which two large bays are fastened together using about 20 "large" bolts. I'm examining this area because I am expecting high stresses and shear forces around the bolted connections.

If I were making this model, I would have connected the bolts (using RBE2 elements) to existing nodes of the adjacent ribs (plate elements).

In this model, the bolts are modeled as bar elements. The ends of the bar elements do not connect to any of the plate elements above or below it - the ends of the bar elements are connected to the closest plate elements via RBE3 elements. Initially, it seemed to be to be a viable way to model the fasteners (although I've never seen it done like this before). After loading results into the model and looking at the stresses and shears as the model deforms, I cannot see any stress buildup around any of the bolts.

My question is if it is common practice to model a bolt as a bar with RBE3s at its ends?

Looking at it again, this method doesn't seem like a very good idea because the load transmitted through the RBE3 is being distributed over a much wider area than the bolt shank area in real life.

Any thoughts or comments would be appreciated. Thanks!

--Erik

 

[SWComposites]

"I would have connected the bolts (using RBE2 elements)" > this approach will give very high, unrealistic stresses in the area of the connections.

"is common practice to model a bolt as a bar with RBE3s at its ends?" > this approach has been used, and has the advantage of not being as grossly overly stiff as when using RBE2s. It will give a better fastener load distribution result.

If all you want from the model is fastener load distributions or overall model stiffness, then using bar or spring elements to represent the fastener flexibility and RBE2 or RBE3 connections between the bars/springs and plate is the usual approach that can give reasonable results when done properly. All fastener flexibility modelling approaches should be validated using simple 1 or 2 fastener axially loaded test FEMs.

If you want the stress field in the vicinity of the fastener holes, then you have a much bigger problem, which will require a much more detailed model. The general rule is that the stresses in any elements connected to rigid elements are not correct. Again, a simple test model to validate the modelling approach should be run and understood first.

SW

 

[rb1957]

RBEs are rigid which exaggerates the load transfer

beam elements (or zero length DOF springs) are elastic ... the deflections of the beam due to shear load should match some fastener flexibility stiffness (huth, etc).

personally i'd've embedded a matching node in the second plate (rather than RBEing this point to the existing mesh).

I'd also ignore the stresses in the plates local to the fasteners, unless there's a ridiculous amount of mesh refinement at these points (and maybe not even then !?). i'd use a hand calc, using the shear load on the fastener.

 

[admiral007]

SWComposites - thank you for the reply.

My concern is that the creators of this model were being too conservative when they placed these fasteners. I do want to see the stress field in the vicinity of these fasteners, and I don't think that has been accurately captured in this model.

I'm concerned that their design of this part is not ideal, and I'm trying to prove that via structural analysis. Since this is a more general topic than FEA, I've made another post here:

http://www.eng-tips.com/viewthread.cfm?qid=295116&page=1