Hey Ben,
the adjoint solver is not written into OpenFOAM®. I got a piece of code which was written for OpenFOAM® and could integrate it into my version.
I do not know if it is planned to integrate an adjoint solver into the standard version of OpenFOAM®....

@ Ben: The adjoint solver is not part of the standard OpenFOAM® version. I got a piece of code written for OpenFOAm and integrated it into my version. It is a SIMPLE solver which solves for the primary Navier Stokes equations and foe the adjoint equations.

@ Guido: I know this paper. What is described in the paper is quite similar to what we are doing. Do you also want to solve adjoint equations with OpenFOAM®? It is also important to implement new boundary conditions for the adjoint variables which depend on the objective function. This might also be the problem in the thread www.cfd-online.com/Forums/openfoam-solvi...r-flow-problems.html

which you were mentioning....

Has anybody used the DAKOTA Project for optimization at all (dakota.sandia.gov/)? I see that Engys is involved with it and I've seen it mentioned a couple of times before when it comes to optimizing CFD based models.

Hi,
I have been using DAKOTA coupled with OpenFOAM® quite extensively for both CAD-driven and surface morphing shape optimisation. DAKOTA is quite robust and efficient and we use it on a daily basis as standard optimisation tool.
Paolo

Hi Paolo,
Can you explain how to couple the DAKOTA and OpenFOAM®??? I have been successful in installing DAKOTA ver 5.0 and openFOAM-1.7.x.Also, can you share a case as tutorial !!

Thanks

Arvind

Hi Arvind,

Here is a typical sequence of steps required to couple DAKOTA with OpenFOAM®:

1. Create the DAKOTA input deck file including the variables, objectives, etc.

2. Create a parametric OpenFOAM® model where each variable is marked with curly brackets, like in the following:
inlet
{
type fixedValue;
value uniform ( {Uin} 0 0 );
}
where Unin defines a parametric inlet velocity in this case.

3. Create a shell script which performs the following tasks:
- pre-processing tasks (e.g. copy the OpenFOAM® template case working directory)
- update the OpenFOAM® parametric input file(s) by using Dprepro utility provided by DAKOTA
- create the mesh
- run OpenFOAM®
- read the results

Here is a sample script to run OpenFOAM® from within DAKOTA (i.e. "run_openfoam.sh"):

# $1 is params.in FROM Dakota
# $2 is results.out returned to Dakota

# Add pre-processing commands here

# Update OpenFOAM® parametric file (i.e. "U") by reading from template (i.e. ("U.template") using Dprepro utility
dprepro $1 U.template U

# Run snappyHexMesh or other to create mesh
snappyHexMesh

# Run OpenFOAM®
simpleFoam

# Copy the OpenFOAM® results back to DAKOTA
mv openfoam_results.dat $2


Remarks: make sure the relevant output response(s) (e.g. pressure drop) are written to a proper text file (e.g. "openfoam_results.dat") for later reuse in DAKOTA.

4. In the DAKOTA input deck file, use the following specifications for the interface section:

interface,
system
analysis_driver = './run_openfoam.sh'
parameters_file = 'params.in'
results_file = 'results.out'

Paolo