CFD Online Discussion Forums

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

- OpenFOAM Verification & Validation (https://www.cfd-online.com/Forums/openfoam-verification-validation/)

- - wss validation (https://www.cfd-online.com/Forums/openfoam-verification-validation/133613-wss-validation.html)

hi
I am trying to find wall shear stress contours in a 3d pipe with openfoam .simulation information are
laminar,unsteady,newtonian fluid.I am using icofoam solver .
openfoam Y velocity quantities are almost the same as the right answers but wall shear stress quantities are completely wrong in the other word the right answers are given from 0.4 to 7 but mine are between [1.61669e-06,1.61669e-05]
I used these codes please help me to find the solution.
in 0 file ,wallShearStress folder

Code:

dimensions      [0 2 -2 0 0 0 0];



internalField   uniform (0 0 0);



boundaryField

{

    body

    {

        type            calculated;

        value           uniform (0 0 0);

    }

    inlet

    {

        type            calculated;

        value           uniform (0 0 0);

    }

    outlet

    {

        type            calculated;

        value           uniform (0 0 0);

    }

}

in constant folder,RASProperties

Code:

RASModel        laminar;



turbulence      on;



printCoeffs     on;

in turbulenceProperties in constant folder

Code:

simulationType RASModel;

Ali,

CFD can be tricky for even seemingly trivial tasks. There are numerous settings and requirements that influence the answer since, after all you are modeling a real system with discretized equations and discrete time and space. With that said:

Your mesh could be too coarse, skewed, or just poor quality (use checkMesh to see)
You could have chosen an improper divergence, Laplacian, and/or gradient scheme.
your time steps could be too big (is it scaled to the CFL condition outlined in the users guide?)
you may have entered the wrong viscosity in constant/transportProperties
etc.

There are many possibilities for "why", but without more information this is as good as I can get. Have a look at

http://www.cfd-online.com/Forums/ope...-get-help.html

and people always love pictures. Good Luck!

thanks for your attention
I have attached the mesh . About transport properties I should mention that I put nu quantity equal to result of nu = mu/rho.This is checkMesh result:

Code:

Create polyMesh for time = 0



Time = 0



Mesh stats

    points:           302592

    faces:            885385

    internal faces:   864251

    cells:            291606

    faces per cell:   6

    boundary patches: 3

    point zones:      0

    face zones:       0

    cell zones:       0



Overall number of cells of each type:

    hexahedra:     291606

    prisms:        0

    wedges:        0

    pyramids:      0

    tet wedges:    0

    tetrahedra:    0

    polyhedra:     0



Checking topology...

    Boundary definition OK.

    Cell to face addressing OK.

    Point usage OK.

    Upper triangular ordering OK.

    Face vertices OK.

    Number of regions: 1 (OK).



Checking patch topology for multiply connected surfaces...

    Patch               Faces    Points   Surface topology                  

    body                19650    19700    ok (non-closed singly connected)  

    inlet               742      768      ok (non-closed singly connected)  

    outlet              742      768      ok (non-closed singly connected)  



Checking geometry...

    Overall domain bounding box (-14.2294 0 -15.1572) (12.9588 47.2016 2.2)

    Mesh (non-empty, non-wedge) directions (1 1 1)

    Mesh (non-empty) directions (1 1 1)

    Boundary openness (-3.50243e-16 -1.50181e-16 -6.31521e-18) OK.

    Max cell openness = 3.22113e-16 OK.

    Max aspect ratio = 9.66007 OK.

    Minimum face area = 0.000865714. Maximum face area = 0.0893054.  Face area magnitudes OK.

    Min volume = 0.000258464. Max volume = 0.0187293.  Total volume = 1091.82.  Cell volumes OK.

    Mesh non-orthogonality Max: 24.5048 average: 5.06496

    Non-orthogonality check OK.

    Face pyramids OK.

    Max skewness = 0.361871 OK.

    Coupled point location match (average 0) OK.



Mesh OK.



End

this is control dict:

Code:

application     icoFoam;



startFrom       startTime;



startTime       0;



stopAt          endTime;



endTime       4.8;



deltaT          0.001;



writeControl    timeStep;



writeInterval   20;



purgeWrite      0;



writeFormat     ascii;



writePrecision  6;



writeCompression off;



timeFormat      general;



timePrecision   6;



runTimeModifiable true;



libs (

    "libOpenFOAM.so"

    "libgroovyBC.so"

) ;

fvSchemes

Code:

ddtSchemes

{

    default         Euler;

}



gradSchemes

{

    default         Gauss linear;

    grad(p)         Gauss linear;

}



divSchemes

{

    default         none;

    div(phi,U)      Gauss linear;

}



laplacianSchemes

{

    default         none;

    laplacian(nu,U) Gauss linear orthogonal;

    laplacian((1|A(U)),p) Gauss linear orthogonal;

}



interpolationSchemes

{

    default         linear;

    interpolate(HbyA) linear;

}



snGradSchemes

{

    default         orthogonal;

}



fluxRequired

{

    default         no;

    p               ;

}

fvSolution

Code:

solvers

{

    p

    {

        solver          PCG;

        preconditioner  DIC;

        tolerance       1e-06;

        relTol          0;

    }



    U

    {

        solver          PBiCG;

        preconditioner  DILU;

        tolerance       1e-05;

        relTol          0;

    }

}



PISO

{

    nCorrectors     1;

    nNonOrthogonalCorrectors 0;

    pRefCell        0;

    pRefValue       0;

}

thank you

Which data set are you comparing against?

wall shear stress quantities

Since i have no idea what your Re or Co number are I will start to make some more suggestions based on what you have given. Your mesh is not completely orthogonal (is this a Gambit mesh?) so you should change your Laplacian Schemes to

Code:

laplacianSchemes

{

    default         none;

    laplacian(nu,U) Gauss linear corrected;

    laplacian((1|A(U)),p) Gauss linear corrected;

}

and your normal gradient schemes to something like

Code:

snGradSchemes

{

    default         corrected;

}

In theory if you cell Peclet number is > 2 you shoudl really be using something different than Gauss linear for divergence schemes so you may want to try linearUpwind or limitedLinear instead. I think the previous questions of "Which data set are you comparing against?" was referring to ...where are you getting these experimental/numerical values of shear that you are comparing to your simulation results?

thanks alot
I have changed what ever you mentioned but I found that I have not scaled the geometry and my dimensions are in meter but I need them to be in millimeter so I scaled them ,I have checked the solution in fluent with this scaled geometry with steady state boundary conditions it shows the right wall shear stress but as soon as I want to run it in openFoam with an unsteady boundary conditions it was diverged ,I post it here ,If it is possible take a look and help.

PHP Code:


		
			
http://www.cfd-online.com/Forums/openfoam-solving/133643-foam-error-printstack.html#post486858

yes it is a gambit mesh and I am getting these experimental/numerical values of shear from an article which they have been published.
thank you

Run your case again and attach the text file of the output to this post if it is small. You can attach txt files....so use the command

Code:

icoFoam >log.icoFoam.txt 2>&1

to capture all the errors and solver output. I suspect that you have a Co number that is too large or you have a boundary condition that is improperly set. Again, if you provide move information e.g. the boundary conditions you use....a better solution can be provided. to be clearer....when you ask for help....ask yourself.

Code:

what information is necessary to reproduce this issue?

if it means zipping up your case and posting a link to it on dropbox then that is a good idea.