Modeling fasteners with CBUSH or CFAST

[flambter]

Hi,

I am modeling a simple two plates (offseted so no coincident nodes) with Nastran/Patran, attached with two rows of two fasteners with applied load axially in order to mainly transfer shear load (by default some tension since the plates are offseted.)

Theory and hand calculation shows that the load share between the two rows should be about 52.1% and 47.9% of total shear load. I peformed one model using cbush with hand calculated tension and shear stiffness. The cbush connect the two plates on a single node. I did another model using Nastran CFAST connectors, still using the same hand calculated stiffness.

REsults:

CBUSH: 55.5% and 44.4% (Close enough)
CFAST: 65.5% and 34.5%

THis seems like a huge difference, especially since MSC pushes to use the CFAST. Ok, there is no hot spots because the CFAST redistribute the load on multiple elements, but the load in the fasteners seems very off.

Any of you have any idea why or any thoughts on CFAST to model fasteners?

Also, when using CBUSH with only tension and shear stiffness for two offseted plates, then a freebody diagram of the cbush shows that it is not in equilibirum (moment created by the shear load and the offset of the plates). The same thing actually happens for CFAST. Is this normal? should those elements be considered as a "real" element and not just a mathematical function to transfer load? Should rotational stiffness be added just for the sake of equilibrium of the fastener? If this is done, tension values in the fasteners changes a lot (50%) while shear values do not change.

Any thoughts?

Thanks.

 

[JeffPW]

In my experience of modelling joints, a simplified one-dimensional model is used to obtain the shear load in each fastener and the bypass load in each plate. The shear loads can then be compared with the joint allowables for static strength.

Jeff W

http://www.p-over-a.co.uk

 

[ESPcomposites]

Do you have a picture of the model?

You "may" have hit the nail on the head? If the CFAST (as I remember from a MSC pitch) prevents it from "hot spotting", it is also affecting the local stiffness in the area around it by doing so. In that case, it will become mesh size dependent. I mentioned this to the presenter and I did not get a good answer, but rather you need to have "judgement" as to the mesh size. I can understand what this means, but some may not.

If you use a CBUSH (or spring), you can also calibrate out the "hot spot". This is done by creating a model with just a single fastener representation, with a like mesh density as used in the actual model. Calculate the anticipated deflection from theory (sum of AE/L and spring k) and compare to the FEM. Then adjust the spring k to obtain what you should get from theory. This is done in practice sometimes. Generally it is not that sensitive though.

With the calibrated spring stiffness, rerun the model and it should match very well, even though there is a "hot spot". You are not using the FEM for anything more than a loads (i.e. bearing and/or bypass) I presume. So while it doesn't look "pretty", it simply works.

Just as in a recent discussion, I might use the CBUSH or even a spring element. The reason is that it works every time (especially for the spring which you can't mess up), even if it is clunky. I know many modern FEM users and MSC will say that is archaic, but I like simple and proven over what you seem to be experiencing. You will need to get familiar with the pitfalls of the element, do some more test cases, etc. before you can gain confidence with it. Of course, it does have some nice advantages once you get to that point and if you are using it regularly enough to remember proper usage.

And just because MSC is pushing the element, does not mean it is immediately adopted. For the major aircraft programs I have worked, it was not being used. At least in the sections I am familiar with.

Brian

http://www.espcomposites.com