CFD Online Discussion Forums - Unknown character in name of output variable when using coded function object

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

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

- - Unknown character in name of output variable when using coded function object (https://www.cfd-online.com/Forums/openfoam-post-processing/229456-unknown-character-name-output-variable-when-using-coded-function-object.html)

Unknown character in name of output variable when using coded function object

Hello everyone,

I work with OpenFOAM v7 and the solver compressibleInterFoam.
I am studying a water/air flow in a cylinder.
For the post-processing, I want to be able to visualize the dynamic viscosity (mu) on Paraview.
When running the solver, there are multiple variables in the output directories, but mu isn't one of them.
So I use a coded function object :

Code:

myFunctionMu

    {

        type                            coded;

        libs                             ("libutilityFunctionObjects.so");

        name                           writingMu;

        codeWrite

        #{

            const volScalarField& mu = mesh().lookupObject<volScalarField>("thermo:mu");

            mu().write();

        #};

    }

Base on the template found here : https://cpp.openfoam.org/v7/classFoa...ionObject.html

This works, the mu files are written in the output directories.
The problem is the name of those files, because they contain an unknown character (image is attached). If I try to copy it here it gives : thermomu
It is a problem because I can't visualize them in Paraview, while I can with other objects I output (e.g. yPlus).

I tried putting just "mu" instead of "thermo:mu", but when I run the solver there is an error message :

Code:

request for volScalarField mu from objectRegistry region0 failed

    available objects of type volScalarField are



39

(

thermo:alpha.air

alpha.air_0

thermo:mu

alpha.water_0

thermo:alpha.water

interfaceProperties:K

thermo:psi

nut

K

K_0

alpha.water

yPlus

p_rgh_0

T.air

thermo:psi.water

rho

T.water

p_rgh

gh

thermo:psi.air

thermo:rho.water_0

delta

enstrophy

alphat

thermo:rho.air

rho_0

p

T

thermo:rho.water

T_0

alpha.air

thermo:mu.water

e.air

thermo:rho.air_0

Co

(alpha.water*div(phi))

thermo:mu.air

e.water

thermo:alpha

)

I also tried removing the parentheses here :

Code:

mu.write();

or changing the name of the constant but the problem remains.

Is there a problem in my code ? If not, is this a bug ? If yes, is there a way to change the name of the output files to be able to read them in Paraview ?

Additional question but relevant only if I solve the main (mu) problem first : Ideally, I also want to get the kinematic viscosity (nu) but it isn't in the list of the available volScalarField. Can I output them using a coded function object or an other type of function object dividing mu by rho ?

Thank you in advance,

-Philomène

Hi Philomène,

Your code looks fine. It is weird that the colon symbol cannot be displayed properly, since it is a legal character for filenames in Linux. There are two ways you can try:
1. rename the file after running the simulation
2. change your code to

Code:

const volScalarField& mu = mesh().lookupObject<volScalarField>("thermo:mu");

volScalarField Mu

    (

        IOobject

        (

            "mu", // any name you want

            runTime.timeName(),

            mesh,

            IOobject::NO_READ,

            IOobject::AUTO_WRITE

        ),

        mu

    );

Mu.write();

You can only run the above code when it's time to write to be more efficient.

Regarding nu, you just need to find out rho as you did for mu, calculate mu/rho and then write it out using the code above. You can output both using a single function object. Just add more lines to the code section.

Hello Wenyuan, thanks you for your help!

I am running OpenFoam on WSL (Windows Subsystem for Linux) and using Paraview on Windows 10, maybe the error comes from here.
Renaming the files after running the simulation will indeed be my last option.

I tried running the simulation with your code but I have an error message and I don't understand why :

Code:

/mnt/c/Users/vergnol/Documents/liquid_piston/Simulations/SIMULATIONS_3D/SIMU_70_rho_mu/system/controlDict.functions.myFunctionMu: In member function ‘virtual bool Foam::writingMuFunctionObject::write()’:

/mnt/c/Users/vergnol/Documents/liquid_piston/Simulations/SIMULATIONS_3D/SIMU_70_rho_mu/system/controlDict.functions.myFunctionMu:81:7: error: ‘runTime’ was not declared in this scope

/mnt/c/Users/vergnol/Documents/liquid_piston/Simulations/SIMULATIONS_3D/SIMU_70_rho_mu/system/controlDict.functions.myFunctionMu:81:7: note: suggested alternative: ‘dimTime’

make: *** [Make/linux64GccDPInt32Opt/functionObjectTemplate.o] Error 1

[0]

[0]

[0] --> FOAM FATAL IO ERROR:

[0] Failed wmake "dynamicCode/writingMu/platforms/linux64GccDPInt32Opt/lib/libwritingMu_33240e2602611f4d17313e6bfbc54de6c82bead9.so"

[0]

[0]

[0] file: /mnt/c/Users/vergnol/Documents/liquid_piston/Simulations/SIMULATIONS_3D/SIMU_70_rho_mu/system/controlDict.functions.myFunctionMu from line 70 to line 74.

[0]

[0]     From function void Foam::codedBase::createLibrary(Foam::dynamicCode&, const Foam::dynamicCodeContext&) const

[0]     in file db/dynamicLibrary/codedBase/codedBase.C at line 206.

[0]

FOAM parallel run exiting

The error seems to be that "runTime" is not previously defined.
Should I add something in my controlDict ?
Here it is :

Code:

application     compressibleInterFoam;



startFrom       latestTime;



startTime       0;



stopAt          endTime;



endTime         21;



deltaT          0.001;



writeControl    timeStep;        



writeInterval   1;                        



purgeWrite      0;



writeFormat     ascii;



writePrecision  6;



writeCompression off;



timeFormat      general;



timePrecision   6;



runTimeModifiable true;



adjustTimeStep  yes;



maxCo           1;

maxAlphaCo      0.4;

maxDeltaT       0.01;



functions

{

        myFunctionMu

    {

        type                            coded;

        libs                             ("libutilityFunctionObjects.so");

        name                           writingMu;

        codeWrite

        #{

            const volScalarField& mu = mesh().lookupObject<volScalarField>("thermo:mu");

            volScalarField Mu

                        (

                                IOobject

                                (

                                        "mu", // any name you want

                                        runTime.timeName(),

                                        mesh,

                                        IOobject::NO_READ,

                                        IOobject::AUTO_WRITE

                                ),

                                mu

                        );

                Mu.write();

        #};

    }

}

Best,

-Philomène

Hi Philomène,

Now the problem is clear to me since colon is an illegal character for Windows filename.

Regarding the error, you can try

Code:

mesh.time().timeName()

BTW, you can also try to use the Linux subsystem to run ParaView.

Hi,

Yes you're right the problem occurs when naming the file on Windows! Thank you for helping me identify the source of the problem. I will run it with Ubuntu to solve this.

There is still a message error when I try your code though :

Code:

ln: ./lnInclude

/mnt/c/Users/vergnol/Documents/liquid_piston/Simulations/SIMULATIONS_3D/SIMU_70_rho_mu/system/controlDict.functions.myFunctionMu: In member function ‘virtual bool Foam::writingMuFunctionObject::write()’:

/mnt/c/Users/vergnol/Documents/liquid_piston/Simulations/SIMULATIONS_3D/SIMU_70_rho_mu/system/controlDict.functions.myFunctionMu:81:7: error: invalid use of member function ‘const Foam::fvMesh& Foam::writingMuFunctionObject::mesh() const’ (did you forget the ‘()’ ?)

make: *** [Make/linux64GccDPInt32Opt/functionObjectTemplate.o] Error 1

[0]

[0]

[0] --> FOAM FATAL IO ERROR:

[0] Failed wmake "dynamicCode/writingMu/platforms/linux64GccDPInt32Opt/lib/libwritingMu_d46f4e90ee27fdba7556000cf87a0f480bb19555.so"

[0]

[0]

[0] file: /mnt/c/Users/vergnol/Documents/liquid_piston/Simulations/SIMULATIONS_3D/SIMU_70_rho_mu/system/controlDict.functions.myFunctionMu from line 70 to line 74.

[0]

[0]     From function void Foam::codedBase::createLibrary(Foam::dynamicCode&, const Foam::dynamicCodeContext&) const

[0]     in file db/dynamicLibrary/codedBase/codedBase.C at line 206.

[0]

FOAM parallel run exiting

[0]

I am not familiar with the use of such code, so I still don't understand the error.

Anyways, you've helped me a lot, thank you!

Hi,

I should have tested the code before posting. I am sorry for that. The following code works with OpenFOAM-v1906 at least

Code:

codeWrite

#{

        if (mesh().time().writeTime())

            {

                const volScalarField& mu = mesh().lookupObject<volScalarField>("thermo:mu");

                volScalarField Mu

                (

                    IOobject

                    (

                        "mu", // any name you want

                        mesh().time().timeName(),

                        mesh(),

                        IOobject::NO_READ,

                        IOobject::AUTO_WRITE

                     ),

                     mu

                );

                Mu.write();

           }

#};

Wenyuan