[t.oliveira]

Dear all,

I have got the simulation results for the velocity field along time.

Now I need to compute the integral of U over a plane (that is not a patch) defined by its basePoint and normalVector.

I have exhausted all the possibilities I could imagine using execFlowFunctionObjects and swak4Foam.

Could you please shed some light on how to do it?

Thanks,

Thomas

[tomf]

I think this should it be possible with ParaView?

[t.oliveira]

Originally Posted by tomf

I think this should it be possible with ParaView?

It probably is. However, AFAIK, the workflow through ParaView is not scalable to many timesteps. Moreover, I would like to repeat that for a series of numerical experiments.

[tomf]

Maybe sample could work, probably still requires ParaView, but this may reduce the workload:
Use sample to generate vtk file for each time step only with U variable > Optionally use the foamSequenceVTKFiles script to rename the files in sequenced order > start ParaView > Open the sequenced files > integrateVariables > save Data (all time steps).

This may need some additional work to get everything in one file. I do not know about current OpenFOAM tools that do this right now. If anyone does, feel free to comment.

Regards,
Tom

[t.oliveira]

Originally Posted by t.oliveira

I need to compute the integral of U over a plane defined by its basePoint and normalVector. Could you please shed some light on how to do it?

Use the following function object:

functions
{
    flux
    {
        type            faceSource;
        functionObjectLibs ("libfieldFunctionObjects.so");

        enabled         true;
        outputControl   outputTime;
        surfaceFormat   off;

        // Output to log&file (true) or to file only
        log             true;
        // Output field values as well
        valueOutput     true;
        // Type of source: patch/faceZone/sampledSurface
        source          sampledSurface;        
        //// if sampledSurface: dictionary with a sampledSurface
        //// Note: will not sample surface fields.
        sampledSurfaceDict
        {           
            type            plane;
            basePoint       (8.1e-4 0 0);
            normalVector    (1 0 0);
            interpolate       false;
        }
        operation       areaNormalIntegrate;
        fields
        (
            U
        );
    }
}

I saved it in a file called system/integrateOnSurfaceDict, instead of writing it on the bottom of controlDict, just to keep it more organised.

Use it executing:

execFlowFunctionObjects -dict system/integrateOnSurfaceDict -noFlow

To find out this solution, I started looking some examples on /src/postProcessing/functionObjects. It is a good starting point.

I tried also using cuttingPlane instead of plane, and interpolate true, and got slightly different results. If I put the plane over a patch, the usage of plane and interpolate false gave the same result as running

patchIntegrate U <patchName>

Best wishes,

Thomas

[t.oliveira]

Originally Posted by tomf

start ParaView > Open the sequenced files > integrateVariables > save Data (all time steps)

Thank you, Tom!

[tomf]

Thank you for pointing out the sampledSurface option, was not aware of that. I thought only patches and faceZones were possible.

[alimea]

Originally Posted by t.oliveira

Use the following function object:

functions
{
    flux
    {
        type            faceSource;
        functionObjectLibs ("libfieldFunctionObjects.so");

        enabled         true;
        outputControl   outputTime;
        surfaceFormat   off;

        // Output to log&file (true) or to file only
        log             true;
        // Output field values as well
        valueOutput     true;
        // Type of source: patch/faceZone/sampledSurface
        source          sampledSurface;        
        //// if sampledSurface: dictionary with a sampledSurface
        //// Note: will not sample surface fields.
        sampledSurfaceDict
        {           
            type            plane;
            basePoint       (8.1e-4 0 0);
            normalVector    (1 0 0);
            interpolate       false;
        }
        operation       areaNormalIntegrate;
        fields
        (
            U
        );
    }
}

I saved it in a file called system/integrateOnSurfaceDict, instead of writing it on the bottom of controlDict, just to keep it more organised.

Use it executing:

execFlowFunctionObjects -dict system/integrateOnSurfaceDict -noFlow

To find out this solution, I started looking some examples on /src/postProcessing/functionObjects. It is a good starting point.

I tried also using cuttingPlane instead of plane, and interpolate true, and got slightly different results. If I put the plane over a patch, the usage of plane and interpolate false gave the same result as running

patchIntegrate U <patchName>

Best wishes,

Thomas

Hi
I want to calculate the heat flux over a plane. I have computed gradT before that. Is your code appropriate for my goal?
What about calculation of flux over a cylinder perimeter?
Thanks

[t.oliveira]

Originally Posted by t.oliveira

Use the following function object:
[...]
Use it executing:
[...]

This is an updated version that works with OpenFOAM 5.x:

functions
{
    flux
    {
        functionObjectLibs ("libfieldFunctionObjects.so");
        type             surfaceFieldValue;

        enabled          true;
        writeControl     outputTime;
        writeInterval    1;
        writeFields      false;

        name myName;

        // regionType: patch/faceZone/sampledSurface
        regionType sampledSurface;

        sampledSurfaceDict
        {
            type                  plane;
            planeType             pointAndNormal;
            pointAndNormalDict
            {
                point  (0.1 0 0);
                normal (1 0 0);
            };
            interpolate false;
        }

        // Operation: areaAverage/sum/weightedAverage/...
        operation    areaNormalIntegrate;
        fields
        (
            U
        );
    }
}

Use it executing:

postProcess -fields "(U)" -dict system/integrateOnSurfaceDict

Best wishes,

Thomas

[cdunn6754]

There is no 'flux' function in my installation. I checked the other versions and it's not there either. Is that something that you made?

When I run it I get a warning that that function 'flux' doesn't exist.

EDIT:
Really sorry this worked great. I messed up copying your functionObject text.

[manafaero]

when iam running the script iam getting error

[2] --> FOAM FATAL IO ERROR:
[2] keyword sourceName is undefined in dictionary "IOstream.functions.flux"
[2]
[2] file: IOstream.functions.flux[13]
[13]
[13] --> FOAM FATAL IO ERROR:
from line 0 to line 0.
[2]
[2] From function dictionary::lookupEntry(const word&, bool, bool) const
[2] in file db/dictionary/dictionary.C at line 442.
[2]
FOAM parallel run exiting
[2]
[6]
[6] [8]
[8]
[8] --> FOAM FATAL IO ERROR:
[8] keyword sourceName is undefined in dictionary "IOstream.functions.flux"
[8]
[8] file: IOstream.functions.flux from line 0 to line 0.

please help

[t.oliveira]

No 'sourceName' was required when I ran it. Did you try providing a sourceName? The syntax for it is similarly to how 'name' is provided.

[Skymaas]

What if one is to find the flux for each cell, at a specific plane? I did get this to work but the output i get is the flux for the entire plane.

[t.oliveira]

Dear Martin,


I looked for "areaNormalIntegrate" in OF source code and found the file .src/functionObjects/field/fieldValues/surfaceFieldValue/surfaceFieldValue.C.


This may give you a clue on how to do it.


I would first try to replace "operation areaNormalIntegrate;" with operation none;" to see what I get. From the source code, it seems that this operation would write the field.



Kind regards,
Thomas

[Skymaas]

Hey Thomas,
I tried the following code. By doing it this way, i can specify which cells, in the y-direction, i want to extract information from.

const volVectorField& C = mesh.C();             

forAll(U, celli)
{
   const vector& Ci = C[celli];            
   if (mag(Ci.x() - 0.35) <= 0.003)
       {


       }
}

The only thing i´m able to extract is the velocities. What i need is either the flux or area of each cell - It is a 2D simulation so i would get the area in length.
Can you give me a pointer of how to extract this? I tried mesh.magSf().boundaryField() but it didn´t work.



/Martin

[t.oliveira]

Are these faces internal or external? mesh.magSf().boundaryField() gives access to external faces.

[Skymaas]

It is internal, so that would explain why the mesh.magSf().boundaryField() doesn´t work.
I got it working to some extend. I am able to extract the volume and velocity for each cell, at position x. Now i also want to know the mean velocity at this plane, is there a way to get that?

[t.oliveira]

Dear Martin,


It is important to use the forum in a way to make it also helpful for other users that look for a question in the future.


For this, it is better if:
- one starts a new question ("how do I get the flux on each cell on a plane") if this is different from the original one ("Calculate flux across surface");


- one reports what they got/found out. Did you try "operation none;"? What what the result? What did you use for internal faces instead of "mesh.magSf().boundaryField() ".


As for your question, isn't the mean velocity equal to the flux over the area?

[Skymaas]

Hey Thomas,
I actually did open a new thread, but no one responded to it so that is why I asked in this thread. Also, I got the code(posted before the previous) to work, simply by asking for the variable that i want (U[celli], V[celli] ect.)
No, velocity would be the flux multiplied by the area, since flux is velocity over area. I believe i know where you are going with this, but the main problem is how to extract it.

[dieg01mp]

Originally Posted by t.oliveira

This is an updated version that works with OpenFOAM 5.x:

functions
{
    flux
    {
        functionObjectLibs ("libfieldFunctionObjects.so");
        type             surfaceFieldValue;

        enabled          true;
        writeControl     outputTime;
        writeInterval    1;
        writeFields      false;

        name myName;

        // regionType: patch/faceZone/sampledSurface
        regionType sampledSurface;

        sampledSurfaceDict
        {
            type                  plane;
            planeType             pointAndNormal;
            pointAndNormalDict
            {
                point  (0.1 0 0);
                normal (1 0 0);
            };
            interpolate false;
        }

        // Operation: areaAverage/sum/weightedAverage/...
        operation    areaNormalIntegrate;
        fields
        (
            U
        );
    }
}

Use it executing:

postProcess -fields "(U)" -dict system/integrateOnSurfaceDict

Best wishes,

Thomas

I'm actually not using the command for getting the flux for every simulation. Once i'm running various simulations automatically, i just implemented this code on the controlDict file wich actually calculates the flux at the end of every saved iteration. What i want to do is to continue with the code in the controlDict file but to get only the flux for the latest time.