Hello,
I am working on the Perpendicular Flap problem using OpenFOAM for both the solid and fluid solvers. The setup is represented schematically as shown. An airflow is introduced, and as it passes through the hole over the flap, the flap begins to oscillate. However, as observed in the simulation video, there is noticeable mesh distortion during the motion. Eventually, the simulation encounters a floating point exception error.
What could be the possible cause of this issue?
Thank you.
Hi, can you show the error log? one more, the fluid solver of openfoam used is the compressible or
incompressible?
Best
fluid-openfoam.log (214.8 KB)
Hi
Incompressible fluid flow was used.
I also tried reducing the time step significantly, keeping the Courant number around 0.5. However, problematic deformations in the mesh still occur. While the simulation doesn’t crash, it seems like the same issue might arise if the endTime is extended further.
I also tried refining the mesh resolution of the hole to 10x10, 20x20, and 30x30, but the issue still seems to persist. I’m wondering what might be causing the problem. The setup involves high velocity and a thin plate.
Regards
You can try to check the mesh of fluid and recreate the the to get better quality of mesh, for better Orthogonality and Skewness.
@Claudio
Hi
I saw that you have encountered similar problems in the past.
Hi @Turan,
in the past, I posted something concerning the mesh deformation at the flap tip. Your case is even more challenging, as the orifice is very small at the beginning, but it can become very large when the cantilever bends. I wonder if the mesh deformation algorithm is able to keep the mesh good enough. I am afraid that, at some point, the cells of the orifice become too deformed.
On the other side, it looks like your case crashes well before possible deformation issues. At the orifice, you have a strong pressure gradient. At the beginning of your simulation, the fluid may have trouble to converge. At first, I’d try to run a fluid simulation. If you are able to find a good pressure and velocity field with the rigid beam, I’d use those results to start the FSI simulation.
Hope it helps a bit. Let me know how it goes.
Claudio
Here is the situation: I ran the specified example as a fluid simulation. While I haven’t performed a detailed analysis of its accuracy, the values and the visual output appeared natural and satisfactory. I used the parameters from the paper. My goal is to replicate the experimental conditions from the paper in the simulation. However, when performing the FSI analysis, it seems that the orifice meshes fail to adapt to the deformation.
Turan
I used FEniCS and OpenFOAM for the solid part and OpenFOAM for the fluid part. However, since the issue seems to be on the fluid side, the error doesn’t change. I wonder if I need to adjust the movement of the mesh in that region. But how?
Hi,
some questions:
checkMesh -latestTime on the fluid side?Given the small distance between the faces of the orifice, when the flap moves, the cells of the orifice will eventually become too skewed.
What about applying an overset mesh around the flap? If you have used solids4foam there are examples there.
Claudio
fluid-openfoam.log (683.8 KB)
checkMeshLog.txt (4.1 KB)
Hi
I ran the simulation with an orifice mesh sized 20x20. I shared the checkMesh file for the final time step and the simulation error message with you above. I didn’t fully understand how to apply an overset mesh in this case. What would you recommend?
Turan
fsi9.zip (6.5 MB)
Here is the simulation video. You can see the distortion in the upper regions.
Hello, @Makis
Perhaps you might have an idea as well. Where could the problem be?
Hi,
it looks like there is something wrong in the definition of your boundary conditions. The mesh points of the upper side of the orifice are moving, it should not be, Can you check pointDisplacement there? Or the dynamicMeshDict.
Claudio
You are correct. The point displacement file includes a slip boundary condition. What should I assign to ensure it remains fixed?
It should be the same as other fixed walls…
Something like fixedValue, uniform (0 0 0)
Claudio
Thank you. I figured it out and tried it myself, and it worked. However, at high speeds, the issue still occurs. I believe I need to try reducing the time step and refining the mesh. Do you have any additional suggestions or requests? I will keep you updated on the progress. Thanks again!