[wangziyang]

hi everyone!

i recently try to output a volVectorField CC_ in a turbulent moedel DCMM.C

but when i complie .c programm, it show show the following error:

DCmM.C: In member function ‘virtual void Foam::incompressible::LESNonlinearModels::DCMM::correct(const Foam::tmp<Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh>
 >&)’:DCMM.C:291:6: error: expected primary-expression before ‘)’ token
      );

my output code is as follows:

void DCMM::correct
(
    const tmp<volTensorField>& gradU
)
{
    LESNonlinearModel::correct(gradU);

    updateSubGridScaleFields(gradU());

 const volVectorField CC_=CC(gradU);  // CC is a function of gradU, also is a volVectorField
       CC_
	 (
        IOobject
        (
            "CC_",
            runTime_.timeName(),
            mesh_,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh_,
		
     );      //  expected primary-expression?? why?? 

}

how can i solve the problem?

i need help

thanks

[HPE]

You try to construct CC_ twice?

[wangziyang]

hi HPE

thanks for your reply!

how can i "construct" twice? i am a newer in openfoam, i can't understand what's your saying

best wishes

ziyang

[HPE]

An object with the same name and the same type cannot be constructed more than once in its scope in C++. Pay attention to the two opers you did for CC_.

[akashpatel95]

Originally Posted by wangziyang

hi everyone!

i recently try to output a volVectorField CC_ in a turbulent moedel DCMM.C

but when i complie .c programm, it show show the following error:

DCmM.C: In member function ‘virtual void Foam::incompressible::LESNonlinearModels::DCMM::correct(const Foam::tmp<Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> >&)’:DCMM.C:291:6: error: expected primary-expression before ‘)’ token      );

my output code is as follows:

void DCMM::correct(    const tmp<volTensorField>& gradU){    LESNonlinearModel::correct(gradU);    updateSubGridScaleFields(gradU()); const volVectorField CC_=CC(gradU);  // CC is a function of gradU, also is a volVectorField       CC_     (        IOobject        (            "CC_",            runTime_.timeName(),            mesh_,            IOobject::NO_READ,            IOobject::AUTO_WRITE        ),        mesh_,             );      //  expected primary-expression?? why?? }

how can i solve the problem?

i need help

thanks

volVectorField
CC_
(
IOobject
(
"CC_",
runTime_.timeName(),
mesh_,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh_,
dimensionedVector("0",dimLength/dimTime,Zero)
);


This will create empty volVectorField defined on mesh with all fields as zero and dimension as m/s. If you need dimension less fields simply swap "dimLength/dimTime" by "dimless"


Also it seems that you have already declared volVectorField CC_ in the line above which constructs an object named CC_. You cannot create another object with same name immediately below.

[wangziyang]

thanks for your reply! akashpatel95

i will try again

best wishes

ziyang

[frobaux]

Originally Posted by wangziyang

DCmM.C: In member function ‘virtual void  error: expected primary-expression before ‘)’}

Well, This error, I got it a lot. It happens most of the time when you called

myFunction(a,b, )

(There is a comma => so before the ')', we expect another primary expression, which is missing.)


What you should do is something like, as akashpatel95 said:

Originally Posted by akashpatel95

volVectorField
       CC_
     (
        IOobject
        (
            "CC_",
            runTime_.timeName(),
            mesh_,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
         mesh_,
         dimensionedVector("0",dimLength/dimTime,Zero)
        );

Then you fill it

//then, you fill it with the output of your function

CC_=CC(gradU);


//then you write it manually

CC_.write(); // this write directly the fields, so most of the time at each time step => to use only in the debugging steps

[wangziyang]

thanks for your reply! frobaux

it works well according to your guidance!

but i want to output the CC_ fields based on ControlDict , for example, output CC_ every 0.001s

i try to insert the code " if (runTime.writeTime())" ,but produce the error

"error: ‘runTime’ was not declared in this scope
if (runTime.outputTime())"

i think i may be need insert the "creatTime.H" and "writeTime.H"

how can i output the field every 0.001s?

best wishes

ziyang

[akashpatel95]

Originally Posted by wangziyang

i try to insert the code " if (runTime.writeTime())" ,but produce the error

First you need to create runTime object using
Foam::Time runTime(Foam::Time::controlDictName, args);

Then, you can use it like this (This will make sure that your CC_ field is only written when you want according to controlDict, in this case, every 0.001 seconds).

if(runTime.write()) {
CC_.write();
}

[frobaux]

Well, I'm not sure of that but

- if you used the IOobject::AUTO_WRITE options, it should work automatically according to the main parameters of your controlDict (writeControl and writeInterval)
- you can also add a subdictionnary in your controlDict file

functions
{

     myOutputObject
    {
        type writeObjects;
        functionObjectLibs ( "libutilityFunctionObjects.so" );
        objects
        (
                "CC_"
        );
        writeControl     adjustableRunTime;
        writeInterval    0.001;
    
    }
}

The third possibility is the solution given by akashpatel95.: You recreate a runTime.



But where is that part of code located/ called?

[wangziyang]

Originally Posted by frobaux

Well, I'm not sure of that but

- if you used the IOobject::AUTO_WRITE options, it should work automatically according to the main parameters of your controlDict (writeControl and writeInterval)
- you can also add a subdictionnary in your controlDict file

functions
{

     myOutputObject
    {
        type writeObjects;
        functionObjectLibs ( "libutilityFunctionObjects.so" );
        objects
        (
                "CC_"
        );
        writeControl     adjustableRunTime;
        writeInterval    0.001;
    
    }
}

The third possibility is the solution given by akashpatel95.: You recreate a runTime.



But where is that part of code located/ called?

Thanks very much for your reply！akashpatel95 and frobaux

my code is in a new SGS turbulent model.

The code i present to you is a part of DCNM .C programm (this new turbulent model)

the code is as follows:

// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //

void DCNM::correct
(
    const tmp<volTensorField>& gradU
)
{
	{
 //int main(int argc, char *argv[])
 // #include "setRootCase.H"
 //  #include "createTime.H"
	
      volVectorField     CC_    
	 (
        IOobject
        (
            "CC_",
            runTime_.timeName(),
            mesh_,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
            mesh_,
            dimensionedVector ("CC_",dimless,vector(0,0,0))
     );
            CC_=CC(gradU); // CC is a function of gradU, it has been calculated in private member function section

	    Foam::Time runTime(Foam::Time::controlDictName, args);

	if(runTime.write())
           {
	      CC_.write();
           }  
             
   } 
	
   
    LESNonlinearModel::correct(gradU);

    updateSubGridScaleFields(gradU());

}

but the code will make a error according the suggestion of akashpatel95,

  error: ‘args’ was not declared in this scope
   Foam::Time runTime(Foam::Time::controlDictName, args);

i think my output code is in tubulence model source program, so it can't use the "AUTO_WRITE",

and i also think akashpatel95's advice is right, but how can i solve the error ?

do i need insert any code to my program?

best wishes!

ziyang

[raumpolizei]

Hey, if this inside a turbulence model, you should be able to access the Time object with the following line (no need to create a new Time object, it is already present so lets use it):

const Time& t = this->time();

Regarding the writing part, try to use something like this(check the extended source code guide for more information):

if(t.writeTime()) // or t.outputTime()
{
    CC_.write();
}

[akashpatel95]

Originally Posted by wangziyang

my code is in a new SGS turbulent model.

If your code is inside a turbulence model, then you cannot create runTime object. The syntax I provided for runTime is for process happening inside main() function.

I think for source code, AUTO_WRITE should work just fine while declaring volVectorField

[frobaux]

Well, args is not defined in your scope.



Did you try to add what I suggest in your controlDict?


Not sure because I'm also quite a beginer in openFoam, but you have acess to time trough db or mesh_, so maybe try

if(db().time().write()) // or mesh_.time().write()
{
   ...
}

[wangziyang]

hi! frobaux and akashpate95

very thanks for your reply, and i also very sorry the late reply

according to your suggestions, i have solve my question, i want to share the solution here

first, it shoulid note that i work in of2.3, my purpose is to output the volVectorField CC_ in turbulence model program (eg Smagorinsky.C)


the first step, in priviate member faction, i insert the cord as followsin "updateSubGridScaleFields" part)

CC_=CC(gradU);
CC_.correctBoundaryConditions();

and i also define a volVectorField named CC in this part,and it will return the value to CC.

the second part, in Constructors part, insert the CC_ write code.(the code is memtioned before)

the last part,in Member faction part, insert the code " CC_=CC(gradU); "

meanwhile, in .H programe , CC and CC_ should declare.

ziyang

best wishes!