Bar vibration in cross-flow

[Aurélien J]

Hello,

I am currently studying the flow-induced vibrations of hydro power plant trashracks. One part of that study is a numerical investigation, modelling the problem in 2D. I already got some results for the flow pattern around a trashrack bar, using Code_Saturne at a Reynolds number of about 5000 with the turbulence model "Rij-EBRSM". This is how the vorticity looks like :

Now I would like to let the bar move, using the ALE module. This way I would access the frequency of vibration for a given mass and stiffness. I could thus determine e. g. the added mass.
I have gotten acquainted with the ALE module via this example and could make it work. However in the case of the trashrack bar profile, the computation stops after about 80 time steps :

Abort due to the detection of a negative control volume.

I assume their must be some problem with the deformation of my mesh, but I couldn't find which cell gets broken, so I haven't fixed the problem yet. I have tried to abide by the best practices for mesh generation, i. e. having rectangles in the mesh, but this proved to make the meshing process (using Salome) quite tedious.

Would you advise, in that case, that I preferably use a mesh with triangles? I guess it would make the task of refining the mesh close to the wall easier.
I have attached an archive with the xml file and the listing; the mesh file (44MB) can be found here (time-limited link). In that case I have let the mesh viscosity distribution uniform with value 1. I have also tried defining mathematically the shape of the bar and setting the mesh viscosity to 1e10 inside the bar, following the example of Alexandre Douce ("flow around a cylinder"), but in the end I got the same error in the solver. I point out that I expect very low vibration amplitudes (of order 1e-3*bar thickness) since the structure is very stiff, so the mesh is not supposed to move a lot.

I am aware that this might be more a problem of preprocessing than a problem of Code_Saturne, but I would be pleased to get advice about it if you have some.

Regards

[Yvan Fournier]

Hello,

Switching to tetrahedra will not help, and probably degrade your results quality (assuming an equivalent number of cells).

As ALE deforms the mesh, some cells may become inverted, and that seems to be the case here.

The usual solutions to this are to reduce your time step and/or increase "mesh viscosity" (the latter so that deformations are spread over a wider number of cells, so as to avoid having large deformations only on cells near the boundary).

The more refined the mesh near the wall, the smaller the deformation required to "invert" a cell, so using a slightly coarser mesh may help (I do not believe ALE is often used in conjunction with low-Reynolds models, requiring a refined mesh at the boundary, so its robustness in these cases may not be very well tested).

As you seem to have run tests with mesh viscosity, if this is not enough, maybe using a smaller time step may help.

Regards,

Yvan

[Aurélien J]

OK, I will try this, thanks a lot.

[Aurélien J]

Your answer helped me because it encouraged me to do a trouble-shooting process with my simulation, having in mind some parameters which could cause my simulations to break.

It seems actually that it had nothing to do with the mesh viscosity. The problem was most probably the precision. Indeed, the simulation I carry out has small dimensions. I am interested in vibration amplitudes of about 1e-5. Yet the parameter "relative precision for implicit coupling with internal structures" in the GUI ("implicitation_precision" in the xml file) was set to 1e-5 too. It made the mass-spring system to diverge, which in turn made the mesh to evolve very fast and then to collapse at some points.