[itsthekv]

Hi Everyone,

I am doing a coupled 3D multi-physics FSI simulation using preCICE with SU2 as the fluid solver. I had previously run and got converged results in both steady and unsteady simulations (without mesh deformation) for the same test case, even for multiple levels of mesh. However, when there is mesh deformation, the solution is diverging for most settings. The issue seems to be with the following step:

Non-linear iter.: 1/1. Linear iter.: 3000. Min. volume: 1.50654e-13. Error: 0.149249.

The error value keeps increasing from time-step to time-step, and once it becomes of the order of, say, 10^3, the CFD solution diverges. At this point, I must admit that I do not fully understand what this "error" means.

The config options I am using, after a lot of trial and error, are appended below:

DEFORM_LINEAR_SOLVER= FGMRES
DEFORM_LINEAR_SOLVER_PREC= LU_SGS
DEFORM_LINEAR_ITER= 3000
DEFORM_NONLINEAR_ITER= 1
DEFORM_CONSOLE_OUTPUT= YES
DEFORM_TOL_FACTOR = 0.000001
DEFORM_STIFFNESS_TYPE= INVERSE_VOLUME

If I change preconditioner to ILU or JACOBI, it doesnt run at all. If I increase the tolerance, it diverges faster.

Can someone please ---
1. Tell me what is the "error" for mesh deformations?
2. What can be a better config options than what I am using, for stability as well as reasonable speed?
3. How does the tolerance factor, non-linear and linear iteration limits work towards performing the deformation?

Thanks a lot

[pcg]

Hi Vishnu,
The ILU should be your best bet regarding preconditioner, for linear solver FGMRES is fine unless you start needing many iterations in which case I would try CONJUGATE_GRADIENT to avoid a lot of memory being allocated.
I have often found that DEFORM_STIFFNESS_TYPE= WALL_DISTANCE gives better quality, especially if you have refined wake regions.
Currently (v6+) a solid elasticity analogy is used to deform the mesh. The Poisson ratio for this deformation can be manipulated to make the problem a bit easier, set DEFORM_COEFF to a small value (e.g. 0.2) or to something very large (e.g. 1E8) to reduce locking, the default is 1E6.
I recently fixed a bug in the mesh deformation affecting triangular prism cells, if you have this kind of cells close to the moving walls you may want to give the current develop version a try (git checkout develop and re-compile) (be aware there are ongoing issues with the multigrid and parallel execution on that branch).
If none of this helps please create an issue (https://github.com/su2code/SU2/issues) with instructions and required files to replicate the exact problem.
Regards,
Pedro

[itsthekv]

Hi Pedro,

Thanks for your suggestions...
I am using v6.0.0, but cannot upgrade due to compatibility issues with the other codes I am using for coupling. Also, bugs in parallel computations will be a no-go for me, since I am running on a cluster.

My mesh presently has 30 layers of triangular prisms next to the wall. Should I remove the prisms and make an all-tetra mesh? Or is there any other workaround for the bug you mentioned?

Thanks and Regards,
Vishnu

[pcg]

The bug was making that type of cells too flexible during deformation, so if that area of the mesh is the one being distorted I would say replace by hexes (an all tetra mesh is not going to be very good for RANS).