Acoustic-structural analysis on ABAQUS- Coupling error.

[S1mul4t0r101]

Hello Everyone.
I am new to ABAQUS. I have some previous experience in Ansys Structural FEA. I am trying to perform acoustic-structural analysis to find sound proapgation in air. I looked it up in the manual and followed the instructions but the results with the TIE constraints were not what I was hoping for. Many of the elements don't get contrained to each other and the analysis runs without coupling the acoustic and structural media. I am using a spherical air medium as the acoustic medium and a semi-spherical hollow steel object of 1cm thickness as the solid medium. I have tried using the same mesh parameters on both the media but they still are not coupled. I am running a modal analysis and steady state dynamic (Modal) on the system and the values I receive are probably for individual interactions of the media. I want to find the POR in the air medium due to a force acting on the solid medium.
Please suggest a solution to this problem so the the two media can be coupled together. I am using the air medium as the master and the solid surface as the slave.
I have attached the mesh models of the media here.

 

[FEA way]

Try increasing tolerance and enabling adjustment for tie constraint.

 

[S1mul4t0r101]

@FEAway, I have tried increasing the tolerance and the adjustments are enabled but still the same.

 

[FEA way]

The STRAINFREE output variable, together with internally generated node sets (WarnNodeMissMainIntersect and WarnNodeAdjust) can help you identify problematic regions and apply proper changes. Also, keep in mind that the mesh sizes (and thus also main/secondary surface assignments) have to be selected based on wave speeds in such analyses.

 

[S1mul4t0r101]

I changed the mesh size according to the wavelength and these are the errors I get.

 

[FEA way]

What about the main/secondary surface assignment ? Did you try inverting it ? The rule is that the secondary surface should belong to the part with a more refined mesh. As a last resort, you could use ASI (acoustic-structural interface) elements but it's generally not recommended and it should be possible to make tie constraint work for such simple geometry.

 

[S1mul4t0r101]

I have used same msh size for both the solid and fluid domain. I use the fluid domain as master since it is larger and I read somewhere that if we are solving for POR then the fluid should be master.

 

[FEA way]

Try meshing those parts in such a way that there's a significant difference in mesh densities, with a larger density on a part with a lower wave speed. Assign a secondary surface to it.

 

[S1mul4t0r101]

So, should i use surface to surface or surface to node region constraints?

 

[FEA way]

The default surface-to-surface formulation should work. But instead of relying on the tolerance criterion, you could try specifying the secondary nodes directly (with the TIED NSET parameter).

 

[S1mul4t0r101]

If i select surface of the air domain does it take the outer surface or the surfaces of the nodes? If it does how will it couple with the surface of the solid domain since the solid is within the air?

 

[FEA way]

Can you share the file or at least a screenshot showing the cross-section of both parts assembled together, rendered with different colors (Color Code --> Part instances) ? There should be a cavity for the solid body in the fluid domain.

 

[S1mul4t0r101]

Ohh. I have been trying to couple a solid air domain to the solid domain. I didn't make a cavity for the solid. Where is the color code option?

 

[FEA way]

It can be found on the top toolbar - it's a drop-down list next to the color palette icon. There you can select the criterion for coloring.