[Elvis_M]

Hello everyone,
I use adjointOptimisationFoam to shape-optimize a geometry consisting of several cubes. The solver was slightly modified, the apparent porosity in the Navier-Stokes equation was removed. Compiling works and simulating other geometries also worked.

My problem is that the adjoint system of equations does not converge and always diverges after a few 1000 iterations (due to large continuity error). The primal system converges.

I have attached pictures of the primal and adjoint residuals.

I tried the following:
- Refine mesh
- Vary relaxation factors
- Increase cylinder diameter

I will also try do increase the cylinder length before and after the geometry.
Do you have any ideas what else I can try?

This is my fvSolution:

solvers
{
    "(p|pa)"
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.001;  // was 0.01	
        smoother        GaussSeidel;
    }

    "(U|Ua)"
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-08;
        relTol          0.01; // was 0.1
    }
}

SIMPLE
{
    nCorrectors 3;
	nNonOrthogonalCorrectors 0;
	momentumPredictor   yes;
}

relaxationFactors
{
    fields
    {
        p               0.1; // was 0.3
		pa              0.1; // was 0.2
        alpha           0.1; // was 0.1
    }
    equations
    {
        U                          0.1; // was 0.7
		Ua                         0.1; // was 0.3
    }
}

Thanks in advance,
Elvis

[AndreP]

If you're still struggling with this, from personal experience I noticed that divergency is quite sensitive to the fvSchemes.

Have a look at your gradSchemes and divSchemes, for me it helped going to upwind instead of linearUpwind (2nd order). Indeed accuracy is sacrificed, but it's a good first step to realize where is the problem.

Otherwise, a good tip to see where the problem is coming from, is to stop the solver when the simulation is on the early stages of divergency (have a look at the log file, and make the simulation stop a few iterations after initial stages of divergency), then use Paraview or other post process to plot velocity/pressure or adjoint fields so you can see where the problem is starting, this might give you some hints what's causing the divergency (whether it's meshing, boundary conditions, etc etc etc)

[Elvis_M]

Thank you for your reply! I tried adjusting fvschemes but that didn't solve the problem. But after increasing the cylinder length and width the simulation finally converged.