Modal analysis in a liquid tank using ABAQUS

[alishst]

Hello All

I'm relatively new to ABAQUS and I am trying to model a liquid tank using coupled Eulerian-Lagrangian (CEL) technique for seismic analysis. My problem is that I cannot extract the natural frequencies and modes of the liquid-filled tank because abaqus/standard doesn't support Eulerian elements. What should I do? Is there an alternative way I can extract natural frequencies?

 

[FEA way]

Since your analysis is explicit dynamics procedure, you won't need these modes to be used in the subsequent step as it is done in case of analyses using modal superposition technique. Thus you can extract eigenfrequencies in a separate model. Just copy your current model and mesh it with Lagrangian elements. You can even use hybrid elements to account for fluid properties. Another way is to experiment with structural-acoustic model.

 

[alishst]

Thanks for the reply.

I need to provide the first few natural frequencies as a part of a report to compare them with some real-life cases. That's why I wanted to do modal analysis. Do you think purely Lagrangrian elements provide sufficient accuracy for modal analysis?

Also another question, do you know how to apply pressure boundary conditions on the free surface of liquid in case I want to model it using acoustic-structural model? I first started my simulation with acoustic elements but had to switch to CEL because I didn't know how to apply free surface boundary conditions in ABAQUS.

Many thanks

 

[Erik Panos Kostson]

You can often use acoustic elements inside the tank that will account for the water added mass and pressure on the tank vibrations.

You couple them to the structure (normally tie constraint), and then there should be a free surface boundary condition (impedance bc, see the abaqus manual Acoustic and shock loads, that shows how to set that 1/k1=1/rf*g and 1/c1=0) on the top of the liquid (top level).

See this paper for more details on how to model this

https://www.researchgate.net/public...der_Tri-Directional_Components_of_Earthquake.

There are many more out there so just search (could be some in abaqus verification manual).