Bolt Group Analysis with FE

[stresscalcs]

I am currently looking a a problem of trying to establish the difference of attachment loads in a attachment group in the three situations of

1) Attachment loading if only the attachment strengths are considered (strengths are either shear or bearing).
This is the standard hand method we are all using without any reference to the stiffness of the surrounding structure.

2) Attachment loading if the surrounding structure materials, local thicknesses and component form are considered but friction ignored.

3) Attachment loading if the surrounding structure materials, local thicknesses and component form are considered but friction ignored and with the attachments (say 6.3mm/0.25in dia) passing through holes which are slightly oversize (say 0.1mm/0.040in).

The results are very different for 1) and 2), I am sure.

Has anybody considered such a problem as 3)?
I am sure everybody is thinking FE analysis. I can think of no other way.

Does anybody perhaps have any suggestions for a not too complex FE which would indicate the differences of the 2) and 3) situations?
A full blown major FE model using thousands of solid elements that takes an age to get up and running is not what is wished for here.

Any helpful thoughts would be appreciated.

 

[RPstress]

As you say, the traditional bolt group methods are approximations which can be bettered using more representative stiffnesses.

I have modelled several joints with shell elements and spring elements for the fasteners. This is usually adequate. Finding the stiffness to put in for the springs is a bit tricky, but you can usually find an acceptable number. In a pinch you can do separate anlyses with extreme values.

For flat joints you can model the different layers separated from each other in (say) Z, with the springs making connections only in X and Y. This will give you out of balance moment reports, but will produce identical forces and deflections to modelling everything in the same plane with all the inconvenience of coincident nodes.

It's rarely necessary to go the whole hog and model the thicknesses explicitly. Also it's never really necessary to model hole clearance explicitly. Generally at ultimate everything's bedded in nicely. (It may be a different matter for fatigue, but the largest fatigue loads are usually about a limit load.) It's just possible that with composite substrates some people are worried about things like uneven load distribution which may persist if the bolts don't yield before substate failure, but I personally have never worked on a job where this was so.

 

[stresscalcs]

Thank you for your comments, RPStress.

I have in the past used springs and geometrical positions in 3D situations where nobody has complained about being the results being unrealistic, because most people are not wanting to acknowledge the limitations of the classic "hand calcs" method which may be found in almost all books on structures. For this method (2D or 3D), the question is always "What is the effective spring stiffness?" The results of using stiffnesses relating to shear strength, bearing strength or structures handbook failure loads clearly show different results.
I have never been convinced that an additional safety factor of 1,15 covers much of the lack of reality of the hand calc.

The most fortunate part of the situation is for ultimate loads the joint knows how to share out the load much better than we do and experience has shown the hand calc method is unlikely to predict a failure higher than a test result, if the joint has no obvious "weak spots". Interestingly, yield load distributions are hardly ever looked at.

Though you say (and quite rightly) the oversize holes are covered by the bedding in process for an ultimate static load, the customer sees the situation as a possible fatigue problem due to an unclear load distribution at the attachments.
Consequently, the problem.

Just a further note here. We have a 3D FE model made up of shell elements representing a beam to bulkhead joint, with representative thicknesses and a small number of CBars to represent the attachments. Element stiffness is controlled simply (crudely) by the material E values, so far.
From the results we have seen, the FE analysis shows up to about 70% higher loads than the initial hand calc on some attachments and of course reduced loading on others. Comparing the two load distributions as a whole, they are so different that it seems that they come from different "planets".

Something to think about perhaps?