CFD Online Discussion Forums - Compute fluid accellaration

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

- OpenFOAM Post-Processing (https://www.cfd-online.com/Forums/openfoam-post-processing/)

- - Compute fluid accellaration (https://www.cfd-online.com/Forums/openfoam-post-processing/184482-compute-fluid-accellaration.html)

Compute fluid accellaration

Hi all,

How can I compute the fluid acceleration from the velocity field? Or in other words I want to calculate the material derivative of the velocity vector field.

Hi,

For example, there is fvc::DDt (https://cpp.openfoam.org/v4/a10924.h...6817560484a801).

Hi Alexey,

Thanks for you quick reply. I take it from your answer that one has to write a custom application to compute the material derivative. I am not really familiar with OpenFOAM programming. Is there no way to calculate the material derivative with probe functions or in Paraview?

Hi,

There is codedFunctionObject and in your case it could be as simple as

Code:

    acceleration

    {

        libs ("libutilityFunctionObjects.so");



        type coded;

        // Name of on-the-fly generated functionObject

        name calculateDDt;

        codeWrite

        #{

            // Lookup U and phi

            const volVectorField& U = mesh().lookupObject<volVectorField>("U");

            const surfaceScalarField& phi = mesh().lookupObject<surfaceScalarField>("phi");

            // Write

            volVectorField t("DDt(U)", fvc::DDt(phi, U));

            t.write();

        #}

    }

Maybe somebody else knows how to calculate it in ParaView (yet, guess, it is more complicated).

Hi Alexey,

Thanks for the code. I added the code to my controlDict in the functions section.

With OF3.0+ I got a fatal error:

Code:

--> FOAM FATAL ERROR: 

Unknown function type coded



Valid functions are : 



4

(

patchProbes

probes

sets

surfaces

)

I tried OF1612+ and it works, but during solution only the material derivative is been written in the result directories. All other fields like U are not.

Any thoughts on these issues will be much appreciated.

A further update. I managed to run the code with OF3+. Some changes were necessary.

Code:

acceleration

    {

        functionObjectLibs ("libutilityFunctionObjects.so"); // This needed changing from libs to functionObjectLibs



        type coded;

        // Name of on-the-fly generated functionObject

        redirectType banana; //average; // needed to add redirectType, but the name doesn't seem to affect anything

        name calculateDDt;

        //outputControl runTime;

        code//Write // had to be changed from codeWrite to code

        #{

            // Lookup U and phi

            const volVectorField& U = mesh().lookupObject<volVectorField>("U");

            const surfaceScalarField& phi = mesh().lookupObject<surfaceScalarField>("phi");

            // Write

            volVectorField t("DDt(U)", fvc::DDt(phi, U));

            t.write();

        #};

    }

Now the behaviour during solution is the same as OF1612+. Only the material derivative is written as a result.

Is DDt(U) written on every time step? Add this:

Code:

writeControl writeTime;

Here's configuration, tested on OpenFOAM 4.x:

Code:

    acceleration

    {

        libs ("libutilityFunctionObjects.so");



        type coded;

        name            calculateDDt;

        writeControl    writeTime;

        codeWrite

        #{

            // Lookup U and phi

            const volVectorField& U = mesh().lookupObject<volVectorField>("U");

            const surfaceScalarField& phi = mesh().lookupObject<surfaceScalarField>("phi");

            // Write

            volVectorField t("DDt(U)", fvc::DDt(phi, U));

            t.write();

        #};

    }

Hi Alexey,

I tried to compile OF4.1 but run into errors, so I couldn't test your code. However, I managed to get a solution in OF3+ and OF1612+.

For OF3+ this is my controlDict:

Code:

/*--------------------------------*- C++ -*---------------------------------*\

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

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

|  \    /   O peration     | Version:  3.0                                   |

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

|    \/     M anipulation  |                                                 |

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





FoamFile

{

    version         3.0;

    format          ascii;

    class           dictionary;

    object          controlDict;

    location        "system";

}



libs            ( "libwaveAbsorption.so" "libwaveGeneration.so" );



write        0.5; // create a variable with the desired output interval



allowSystemOperations 1;



application     interFoam;



startFrom       latestTime;



startTime       0;



stopAt          endTime;



endTime         100.0;



deltaT          1e-05;



writeControl    runTime;



writeInterval   $write; // use the variable declared above here



purgeWrite      0;



writeFormat     ascii;



writePrecision  8;



writeCompression uncompressed;



timeFormat      general;



timePrecision   8;



runTimeModifiable true;



adjustTimeStep  yes;



maxCo           1;



maxAlphaCo      1;



maxDeltaT       0.05;





functions

{

    #include        "ProbeData"



    acceleration // The code was tested in OF3+ running serial and parallel case

    {

        functionObjectLibs ("libutilityFunctionObjects.so");



        type coded;

        // Name of on-the-fly generated functionObject

        redirectType DDtU;

        name calculateDDt;

        writeInterval $write; // Re-use the write variable. This statement must be repeated here so that the output of all fields occurs at the same interval

        outputControl runTime; // This is also necessary in OF3+

        code//codeWrite does not work here in OF3+

        #{

            // Lookup U and phi

            const volVectorField& U = mesh().lookupObject<volVectorField>("U");

            const surfaceScalarField& phi = mesh().lookupObject<surfaceScalarField>("phi");

            // Write

            volVectorField t("DDt(U)", fvc::DDt(phi, U));

            t.write();

        #};

    } 

    

}

For OF1612+ the controlDict is this:

Code:

/*--------------------------------*- C++ -*---------------------------------*\

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

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

|  \    /   O peration     | Version:  3.0                                   |

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

|    \/     M anipulation  |                                                 |

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





FoamFile

{

    version         3.0;

    format          ascii;

    class           dictionary;

    object          controlDict;

    location        "system";

}



libs            ( "libwaveAbsorption.so" "libwaveGeneration.so" );



write        0.5;



allowSystemOperations 1;



application     interFoam;



startFrom       latestTime;



startTime       0;



stopAt          endTime;



endTime         100.0;



deltaT          1e-05;



writeControl    runTime;



writeInterval   $write;



purgeWrite      0;



writeFormat     ascii;



writePrecision  8;



writeCompression uncompressed;



timeFormat      general;



timePrecision   8;



runTimeModifiable true;



adjustTimeStep  yes;



maxCo           1;



maxAlphaCo      1;



maxDeltaT       0.05;





functions

{

    #include        "ProbeData"



    acceleration // The code was tested in OF1612+ running serial and parallel case

    {

        functionObjectLibs ("libutilityFunctionObjects.so");



        type coded;

        // Name of on-the-fly generated functionObject

        redirectType DDtU;

        name calculateDDt;

        writeControl    runTime; //For OF1612+ writeControl is required not outputControl

        writeInterval   $write;

        codeWrite //For OF1612 the correct statement is codeWrite not code

        #{

            // Lookup U and phi

            const volVectorField& U = mesh().lookupObject<volVectorField>("U");

            const surfaceScalarField& phi = mesh().lookupObject<surfaceScalarField>("phi");

            // Write

            volVectorField t("DDt(U)", fvc::DDt(phi, U));

            t.write();

        #};

    } 

    

}

There are some small differences in the code for OF3+ and OF1612+. In both cases I found it necessary to use a variable "write" so I can write all fields at the same time interval. I tested the code in serial an parallel cases.

I am wondering if it is possible to write DDtU for a probe location?

You can:

1. Use probes function object. I think with correct order in functions dictionary it is possible to first write DDt(U) field and then probe it.

2. Use probes object directly in your coded function object. Though this way requires a little be more code, than just to write DDt(U).

Hi,

I ended up with the following implementation: https://github.com/mrklein/foam-case...ontrolDict#L43. I have tested it on OF 4.x, so maybe it needs adaptation for OF+3.0 and OF+1602.

Hi Alexey,

I managed to install OF4.1 and your code works very well. It also works in OF1612+ as is.

Now I tried to read the probe locations from a file in the system subfolder. I used the following code, but results in errors.

Code:

acceleration

    {

        libs ("libutilityFunctionObjects.so" "db.so");

        



        type            coded;

        name            calculateDDt;



        writeControl    writeTime; //timeStep;//

        writeInterval   1;

        



        codeOptions

        #{

            -I$(LIB_SRC)/sampling/lnInclude

        #};



        codeLibs

        #{

            -lsampling

        #};



        codeInclude

        #{

            #include "probes.H"

            #include "labelListIOList.H"

            #include "fvMesh.H"

            #include "fvCFD.H"

            #include "createTime.H"

            #include "readTimeControls.H"

        #};



        codeData

        #{

            autoPtr<probes> probes_;

        #};



        codeRead

        #{

            List<word> fields;

            fields.append("DDt(U)");

            List<vector> locations;

            // Locations to probe, could be refactored into reading dictionary

            // instead of constructing it by hand



            locations.append(vector(1e-3, 1e-3, 5e-3));

            locations.append(vector(  60,   -5.5,   -4.19  ));

            locations.append(vector(  60,   -5.5,   -3.966  ));

            locations.append(vector(  60,   -5.5,  -3.94  ));

            locations.append(vector(  60,   -5.5, -3.69  ));

            locations.append(vector(  60,   -5.5,   -3.44  ));

            locations.append(vector(  60,   -5.5,   -3.19  ));

            

            IOdictionary probes

            (

                IOobject

                (

                    "probeLocations",

                    runTime.system(),

                    mesh,

                    IOobject::MUST_READ,

                    IOobject::NO_WRITE

                )

            );

            dictionary conf;

            conf.add("fields", fields);

            conf.add("probeLocations", locations);



            // Initial acceleration field

            volVectorField t(

                IOobject("DDt(U)", time_.timeName(), mesh()),

                mesh(),

                dimensionedVector("0", dimVelocity/dimTime, Zero));

            t.write();



            probes_.reset(

                new probes(

                    "DDt(U)", time_, conf));

            // Probe and write for time = 0

            probes_->write();

        #};



        codeWrite

        #{

            // Lookup U and phi

            const volVectorField& U = mesh().lookupObject<volVectorField>("U");

            const surfaceScalarField& phi = mesh().lookupObject<surfaceScalarField>("phi");

            // Write

            volVectorField t("DDt(U)", fvc::DDt(phi, U));

            t.write();

            // Write probes values

            probes_->write();

        #};



        codeEnd

        #{

            // To have probed value at the last time step

            const volVectorField& U = mesh().lookupObject<volVectorField>("U");

            const surfaceScalarField& phi = mesh().lookupObject<surfaceScalarField>("phi");

            volVectorField t("DDt(U)", fvc::DDt(phi, U));

            t.write();

            probes_->write();

        #};

    }

}

The dictionary file in the system subfolder is:

Code:

probeLocations

                (

                                (  60   -5.5   -4.19  )

                                (  60   -5.5   -3.966  )

                                (  60   -5.5   -3.94  )

                                (  60   -5.5   -3.69  )

                                (  60   -5.5   -3.44  )

                                (  60   -5.5   -3.19  )

                );

A second question; is it actually possible to write output to probes every time step, but write field data less frequently, say every 0.5 seconds?

Hi,

I have updated example (https://github.com/mrklein/foam-case...e-acceleration) with the following additions:

1. Added examples for creation of probes from probesDict file and probes sub-dictionary of controlDict.
2. To be able to probe acceleration field every time step and to write it every write time, I have moved probing code to execute method. So now write frequency is controlled by writeControl and probe frequency with executeControl.
3. Got rid of field lookups on every write/execute method call.

Tested it on OpenFOAM 4.x, do not know if it works on other FOAMs.

Quote:

Originally Posted by alexeym (Post 640313)

Hello,

I am looking for a function object so that I can calculate the acceleration field when running OpenFOAM as well. To me, it doesn't look like the code in the github link calculates the material derivative. Where is the dot product of the velocity and velocity gradient in the code? I also ran the code with some updates to suit OpenFOAM 1912 but it doesn't save anything in the postProcessing folder. It doesn't save anything in the time folders as well. Is someone able to help me with these please? This is the code I have used in my controlDict file.

Code:

    acceleration

    {

        libs ("libutilityFunctionObjects.so");



        type            coded;

        name            calculateDDt;



        executeControl  timeStep;

        executeInterval 1;

        writeControl    writeTime;



        codeOptions

        #{

            -I$FOAM_SRC/sampling/lnInclude

        #};



        codeLibs

        #{

            -lsampling

        #};



        codeInclude

        #{

            #include "probes.H"

        #};



        codeData

        #{

            autoPtr<probes> probes_;

            autoPtr<volVectorField> DDtU_;

            const volVectorField* UPtr_;

            const surfaceScalarField* phiPtr_;

        #};



        read

        #{

        /*

            // Constructing probes dictionary

            List<word> fields;

            fields.append("DDt(U)");

            List<vector> locations;

            locations.append(vector(1e-3, 1e-3, 5e-3));



            dictionary conf;

            conf.add("fields", fields);

            conf.add("probeLocations", locations);

        */

        /*

            // Reading probes dictionary, let's assume it is

            // system/probesDict

            IOdictionary conf(

                IOobject("probesDict", time_.system(), mesh(),

                         IOobject::MUST_READ));

        */

            // Getting probes dictionary from system/controlDict's

            // probes sub-dictionary.

            const dictionary& conf(time_.controlDict().subDict("probes"));



            UPtr_ = &(mesh().lookupObject<volVectorField>("U"));

            phiPtr_ = &(mesh().lookupObject<surfaceScalarField>("phi"));



            // Initial acceleration field

            DDtU_.reset(

                new volVectorField(

                    IOobject("DDt(U)", time_.timeName(), mesh()),

                    mesh(),

                    dimensionedVector("0", dimVelocity/dimTime, Zero)));

            DDtU_->checkIn();

            DDtU_->write();



            probes_.reset(

                new probes(

                    "DDt(U)", mesh(), conf));

            // Probe and write for time = 0

            probes_->write();

        #};



        execute

        #{

            // Write probes values

            DDtU_() = fvc::DDt(*phiPtr_, *UPtr_);

            probes_->write();

        #};



        write

        #{

            // Write

            DDtU_() = fvc::DDt(*phiPtr_, *UPtr_);

            DDtU_->write();

        #};



        end

        #{

            DDtU_() = fvc::DDt(*phiPtr_, *UPtr_);

            DDtU_->write();



            probes_->write();

        #};

    }

Also I have added the probe locations as per below.

Code:

probes

{

    fields

    (

        DDt(U)

    );



    probeLocations

    (

            ( 11 0.370 0 )

            ( 11 0.405 0 )

    );

}

Thanks in advance. Cheers