Abaqus: Acoustic-Structural Interface Boundary Condition 1

[Wayneeeee]

Hi All,

I am new to Abaqus and have been trying to use it to generate an ultrasonic testing water-immersion model. From what I've read, I need to apply a tie constraint between the water-metal interface which will automatically define the required boundary conditions at the interface. Theoretically speaking, the boundary condition at the interface should be non-penetrative and free to slip. However, I can't seem to find any documentation on what the boundary conditions at the interface actually are. Does anyone have any insights on that?

Thank you.

 

[FEA way]

Abaqus uses special acoustic-structural interface (ASI) elements to couple acoustic mesh and structural mesh. They can be defined in two ways. Either created explicitly (create a skin and then use Create section --> Other --> Acoustic interface) or generated automatically from tie constraint, like you say. The second approach is recommended. It is generally advised to select material with lower wave speed as slave surface in tie definition.

 

[Wayneeeee]

Hi there,

Thank you for your prompt response! I found some more information regarding the interaction at the boundary but I am still trying to understand it (

https://classes.engineering.wustl.e.../stm/default.htm?startat=ch05s02ath139.html).

I have some follow up questions regarding what you've said - is there a particular reason why lower wave speed media is advised to be used as the slave surface? So if I were to set up the model as you have recommended - tie constraints, slower media as slave surface, can I assume that at the water-metal interface, the normal stresses and velocities will be continuous (non-penetrant condition) while parallel velocities are not constrained (slip condition)? Thanks!

 

[FEA way]

The reason to select material with lower wave speed as slave surface is related to general rule known from regular structural simulations - slave surface should be the one with finer mesh. And since material with lower wave speed needs to have finer mesh, it usually serves as slave in tie interaction. However if you need detailed solution in the vicinity of the interface then refine both sides equally, according to requirements of lower wave speed material.

In Abaqus acoustic medium is defined in such way that fluid is assumed to be inviscid. Thus normal coupling and slip condition are exist in the model, as you said. To simulate viscous fluid with no-slip condition you would have to use FSI instead.

 

[Wayneeeee]

I see, okay. Thank you for the clarification!