CFD Online Discussion Forums - About adjointShapeOptimizationFoam

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - About adjointShapeOptimizationFoam (https://www.cfd-online.com/Forums/openfoam/110118-about-adjointshapeoptimizationfoam.html)

About adjointShapeOptimizationFoam

Dear Foamers,

I am trying to figure out how adjointShapeOptimizationFoam works. The first attempt I did was to run the tutorial. Everything goes well - tough I don't completely und the results - except for a detail: if I change the inlet name (e.g. from inlet to inlet1) I get this error:

Code:

phd@lab-laptop:~/Scrivania/pitzDaily$ blockMesh 

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.1.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : 2.1.0-0bc225064152

Exec   : blockMesh

Date   : Dec 04 2012

Time   : 10:58:58

Host   : "lab-laptop"

PID    : 3302

Case   : /home/phd/Scrivania/pitzDaily

nProcs : 1

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Disallowing user-supplied system call operations



// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Creating block mesh from

    "/home/phd/Scrivania/pitzDaily/constant/polyMesh/blockMeshDict"

Creating curved edges

Creating topology blocks

Creating topology patches



Creating block mesh topology



Check topology



        Basic statistics

                Number of internal faces : 18

                Number of boundary faces : 42

                Number of defined boundary faces : 42

                Number of undefined boundary faces : 0

        Checking patch -> block consistency



Creating block offsets

Creating merge list .



Creating polyMesh from blockMesh

Creating patches

Creating cells

Creating points with scale 0.001



Writing polyMesh

----------------

Mesh Information

----------------

  boundingBox: (-0.0206 -0.0254 -0.0005) (0.29 0.0254 0.0005)

  nPoints: 25012

  nCells: 12225

  nFaces: 49180

  nInternalFaces: 24170

----------------

Patches

----------------

  patch 0 (start: 24170 size: 30) name: inlet1

  patch 1 (start: 24200 size: 57) name: outlet

  patch 2 (start: 24257 size: 223) name: upperWall

  patch 3 (start: 24480 size: 250) name: lowerWall

  patch 4 (start: 24730 size: 24450) name: frontAndBack



End



[2]+  Done                    gedit constant/polyMesh/blockMeshDict

phd@lab-laptop:~/Scrivania/pitzDaily$ adjointShapeOptimizationFoam 

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.1.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : 2.1.0-0bc225064152

Exec   : adjointShapeOptimizationFoam

Date   : Dec 04 2012

Time   : 10:59:01

Host   : "lab-laptop"

PID    : 3303

Case   : /home/phd/Scrivania/pitzDaily

nProcs : 1

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Disallowing user-supplied system call operations



// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Create mesh for time = 0



Reading field p



Reading field U



Reading/calculating face flux field phi



Reading field pa



Reading field Ua



Reading/calculating face flux field phia



Selecting incompressible transport model Newtonian

Selecting RAS turbulence model kEpsilon

kEpsilonCoeffs

{

    Cmu             0.09;

    C1              1.44;

    C2              1.92;

    sigmaEps        1.3;

}







--> FOAM FATAL ERROR: 

Patch named inlet not found.





    From function fvBoundaryMesh::operator[](const word&) const

    in file fvMesh/fvBoundaryMesh/fvBoundaryMesh.C at line 145.



FOAM aborting



#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#1  Foam::error::abort() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"

#2  Foam::fvBoundaryMesh::operator[](Foam::word const&) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"

#3  

 in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/adjointShapeOptimizationFoam"

#4  __libc_start_main in "/lib/libc.so.6"

#5  

 in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/adjointShapeOptimizationFoam"

Aborted

What does this mean?

Thanks for help.

Samuele

Hi Samuele,

In createFields.H of this solver, there is a line

const labelList& inletCells = mesh.boundary()["inlet"].faceCells();

so you got the error message.

Hope that helps,
Fumiya

So,

isn't it possible to have more than one inlet?

If so, what should I do? Should I edit the solver?

Also, always about that solver, could it solve 3D flows?

Thanks a lot,

Samuele

Hi,

I think you have to edit the solver to use with the geometry that has
the multiple inlets. In the original solver, the inletCells defined in the
code is used to keep alpha=0 at cells adjacent to the "inlet". If you
have another inlet, I think you need to the same for it.

This solver can solve both 2d and 3d flows.

Hope that helps,
fumiya

Thanks again. So, it seems feasible and pretty easy. Let's see. If I have problems, I'll post them here.

Also, just one more question: I don't want to modify alpha, but I'd rather change mass flow or something like that to optimize my flow (in a fixed geometry). Do you think it is possible?

Thanks a lot,

Samuele

Hi Samuele,
adjointShapeOptimizationFoam performs a "topological" optimization of the flow, i.e. it modifies the porosity of each cell; so at the end of the cycle you will know where you have to modify the geometry wrt the distribution of alpha.

What you ask to perform ( change mass flow for example) I think it's not feasible with this kind of optimization and, by the way, with a fixed geometry.

Hope this help
Simone

I am gonna try to edit the source. In this case I should be able to he the optimization I like best. Right?

That's for sure the best solution! :)

Something wrong in my case (see attached pictures).

Maybe it's wrong BC in U, Ua?

Places, where I'm not sure:

in 0/U

Code:

    inlet

    {

        type            surfaceNormalFixedValue;

        refValue           uniform -26;

    }

in 0/Ua

Code:

    inlet

    {

        type                surfaceNormalFixedValue;

        refValue                uniform -1;

//        type            fixedValue;

//        value           uniform (-1 -1 -1);

    }

Can this situation be the after-effect of wrong alpha range? Here alphaMax = 200.0.

Hi Avdeev,

The adjoint velocity direction is opposite to the primal. See the tutorial files.

I hope this helps.

Best regards,
Sylvester

Thanks, Sylvester.
0/U was ok.
Problem was in Ua - now it's work fine:

Code:

    inlet

    {

        type            fixedValue;

        value           uniform (-1 0 0);

    }

adjointShapeOptimizationFoam/pitzDaily tutorial

Hi,

Judging from the direction of the adjoint velocity on the inlet of the pitzDaily tutorial,
I think it converts a minimization problem of total pressure loss(=I) to the maximization problem of -I.
If this is the case, the adjoint boundary conditions on the outlet boundary do not correctly correspond to the reference.

I think lambda should be set to an negative value in constant/transportProperties file when solving minimization problems.
In this case, you have to change the boundary condition of the adjoint velocity Ua:

Code:

    // For pitzDaily tutorial

    inlet

    {

        type            fixedValue;

        value           uniform (1 0 0);

    }

Best regards,
Fumiya