Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations waross on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Acoustic-structural analysis on ABAQUS- Coupling error.

Status
Not open for further replies.
S1mul4t0r101

S1mul4t0r101

Student
Mar 7, 2023
17
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.
Screenshot_2023-03-07_132313_i4iafd.png
Screenshot_2023-03-07_132156_c77ewd.png
 
Replies continue below

Recommended for you

Sort by date Sort by votes
Try increasing tolerance and enabling adjustment for tie constraint.
 
Upvote 0 Downvote
@FEAway, I have tried increasing the tolerance and the adjustments are enabled but still the same.
 
Upvote 0 Downvote
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.
 
Upvote 0 Downvote
I changed the mesh size according to the wavelength and these are the errors I get.
Screenshot_2023-03-08_140719_g6v12p.png
 
Upvote 0 Downvote
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.
 
Upvote 0 Downvote
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.
 
Upvote 0 Downvote
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.
 
Upvote 0 Downvote
So, should i use surface to surface or surface to node region constraints?
 
Upvote 0 Downvote
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).
 
Upvote 0 Downvote
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?
Screenshot_2023-03-09_155950_khlhvt.png
 
Upvote 0 Downvote
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.
 
Upvote 0 Downvote
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?
 
Upvote 0 Downvote
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.
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

S
Abaqus Element set Not defined error
Replies
1
Views
2K
FEA way
FEA way
Abedalhameed A Habashneh
  • Locked
  • Question
Abaqus Girder Analysis
Replies
2
Views
128
Abedalhameed A Habashneh
Abedalhameed A Habashneh
otaviobarodrigues
  • Locked
  • Question
Buckling analysis in ABAQUS
Replies
0
Views
141
otaviobarodrigues
otaviobarodrigues
Ajay Meena
  • Locked
  • Question
SMATsoTsoToscaOpt error in abaqus
Replies
0
Views
91
Ajay Meena
Ajay Meena
PSRani
  • Locked
  • Question
Dynamic explicit, ABAQUS Keyword error
Replies
6
Views
222
FEA way
FEA way

Part and Inventory Search

Sponsor

Back
Top Bottom