divergence error with structured mesh+dynamic mesh
 

Hi all !

I am simulating a cylinder vibrating due to a constant inlet flow. I have two meshes. The quad mesh and triangular mesh. Both meshes are composed of three regions, an O-ring zone near the cylinder that preserve the boundary layer and satisfy SST k-omega y+<1 condition, a deform zone and a stationary outer zone of quadrilateral elements. The main difference between both meshes is the deforming region, one has triangular and the other has quad elements.

The quad mesh shows a divergence in the lift/drag forces that lead to excessive mesh deformation and produce negative cell volumes after a few iterations. The mesh with triangular elements doesn't have this issue and the cylinder reacts normally. Weirdly enough, there are some papers that use a similar quad mesh without problem. I attached an image of the mesh of the paper and my meshes.

Attachment 75169

Since the paper was able to do it using a quad mesh, I am quite clueless as to why my mesh diverges. Anyone can give me some feedback on this? Thanks !

Regards

Quad vs Tri
 

Mesh deformation can be simulated with both quad and tri, however, remeshing is allowed only for tri. Quads can be remshed only via layering, not in arbitrary motion. So, if quad is to be used, deformation has to be kept within certain limits so that deformation can be handled just by compression and expansion of the cells, called smoothing.

Thank you vinerm. That's what i was thinking. I simplified the issue by doing the following:

1.- I did the mesh again using the inbuilt program of fluent. The mesh is not as uniform as the one from ICEM but its pretty close.
2.- I imposed a constant velocity motion on the cylinder in the vertical direction.
3.- I used smoothing only with a diffusion parameter between 1 and 1.5.

I noticed that there is a very small difference in the displacement of the cylinder compared to the Oring. Here I put the first few values.

time : Y_cylinder - Y_oring
0 : 0 - 0
0.001 : 0.0005 - 0.0004979
0.002 : 0.001 - 0.0009957
0.003 : 0.0015 - 0.0014936
0.004 : 0.002 - 0.0019915
0.005 : 0.0025 - 0.0024893

The difference increases linearly as the simulation continues. If the velocity imposed is constant both interfaces should have the same displacement right? I have no idea how this error is introduced.

Diffusion Smoothing
 

Since you are using translational motion, it would be better to keep a value of 0 for the parameter. The numbers you see are averaged values over the nodes of the zone. With a value higher than 0, the diffusion is non-uniform, hence, the numbers can be slightly off due to non-uniform compression and expansion of cells. Since, finally you want an SHM, as far as I remember, if these numbers remain bounded, it would not be a problem.

There are a few settings, such as, increasing the max number of iterations for Laplace equation that might help in improving the accuracy to some extent.