several volscalarfield named Y[i]

farzadmech · December 17, 2019, 20:20

Dear Friends

How can I define two(or several) volscalarfield named Y[i] with two members
Y[1] and Y[2]?

Many thanks
Farzad

clapointe · December 18, 2019, 09:54

Sounds similar to what is done for reacting solvers. So, something like this should be helpful :

Code:

PtrList<volScalarField> Y(2); //
forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Yi",
                runTime.timeName(),
		        mesh,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            i
        )
    );
}

Caelan

farzadmech · December 18, 2019, 10:59

Dear Caelan
Thanks for your response. I did what you have said and I got this error;

./createFields.H:132:9: error: no matching function for call to ‘Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject, Foam::label&)’
)
^

could you please check this error too?

Thanks,
Farzad

Daniel_Khazaei · December 18, 2019, 11:26

Quote:

Originally Posted by farzadmech

Dear Caelan
Thanks for your response. I did what you have said and I got this error;

./createFields.H:132:9: error: no matching function for call to ‘Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject, Foam::label&)’
)
^
could you please check this error too?

Thanks,
Farzad

The correct way of constructing a volScalarField:

PtrList<volScalarField> Y(2); //
forAll (Y, i)
{
Y.set
(
i,
new volScalarField
(
IOobject
(
"Yi",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::NO_WRITE
),

mesh,

dimensionedScalar("name", correct_dimension, initial_value)
)
);
}

clapointe · December 18, 2019, 12:12

Thanks to Daniel, who corrected my code snippet. I should have included that "i" was a placeholder that must be replaced with correct info to instantiate a volScalarField.

Caelan

farzadmech · December 18, 2019, 12:44

Dear Daniel
thanks, it worked. I have two other questions which is related to previous question;

1- If I want to put general initial condition instead of a number for whole domain what should I do?

2- I want to use Y[1] and Y[2] in below equation, but it give me error;

forAll(Y, i)
{
volScalarField& Yi = Y[i];
volScalarField& gammai = gamma[i];
fvScalarMatrix YEqn
(
fvm::ddt(Yi)
+ fvm::div(alphaPhic,Yi)
- fvm::laplacian(gammai, Yi)
==
kinematicCloud.SYi(i, Yi)
);
YEqn.relax();
YEqn.solve(mesh.solver("Yi"));
Yi.max(0.0);
}
}

error;

--> FOAM FATAL ERROR:
Field name Yi not found in schemes

From function bool Foam::cloudSolution::semiImplicit(const Foam::word&) const
in file clouds/Templates/KinematicCloud/cloudSolution/cloudSolution.C at line 217.

FOAM aborting

Is it related to kinematicCloud.SYi(i, Yi)???

Thanks,
Farzad

Quote:

Originally Posted by Daniel_Khazaei

The correct way of constructing a volScalarField:

PtrList<volScalarField> Y(2); //
forAll (Y, i)
{
Y.set
(
i,
new volScalarField
(
IOobject
(
"Yi",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::NO_WRITE
),

mesh,

dimensionedScalar("name", correct_dimension, initial_value)
)
);
}

clapointe · December 18, 2019, 17:26

As for 1), you can likely edit the fields once you create them with something like :

Code:

forAll(Y[i], celli)
{
    if (<insert condition here>)
    {
        Y[i][celli] = <insert value here>
    }
}

For 2), I am not sure what you are trying to do but it does appear to have a problem with your use of the kinematicCloud source term.

Caelan

farzadmech · December 19, 2019, 12:12

Dear Caelan
Thanks for your reply. I want to do something like this(could you please check it if it is feasible?);

First I want to read two fields named Yinit0 and Yinit1 from 0 folder using below code lines;

Code:

label N = 2;
    PtrList<volScalarField> Yinit(N);
    forAll (Yinit, i)
    {
        word nameYiniti ("Yinit" + name(i));
        (
            new volScalarField
            (
                IOobject
                (
                    nameYiniti,
                    runTime.timeName(),
                    mesh,
                    IOobject::MUST_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh
            )
        );		
    }

Then as I learnt from this thread, I can create two fields named Y[1] and Y[2] as below;

Code:

PtrList<volScalarField> Y(N); //
forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Yi",
                runTime.timeName(),
		        mesh,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
mesh,
dimensionedScalar("Y", dimless, 0.0)       
         )
    );
}

Now I want to put Y[0]=Yinit0 and Y[1]=Yinit1.
What should I do? and what should I do to red lines in above code?

Thanks
Farzad

Quote:

Originally Posted by clapointe

As for 1), you can likely edit the fields once you create them with something like :

Code:

forAll(Y[i], celli)
{
    if (<insert condition here>)
    {
        Y[i][celli] = <insert value here>
    }
}

For 2), I am not sure what you are trying to do but it does appear to have a problem with your use of the kinematicCloud source term.

Caelan

clapointe · December 19, 2019, 12:29

Can you not do something like this?

Code:

Y[0] = Y0init;
Y[1] = Y1init;

Caelan

farzadmech · December 19, 2019, 12:39

Dear Caelan
I will do that right away, but what should I do to these below lines?

Code:


mesh,
dimensionedScalar("name", correct_dimension, initial_value)

Here we have given name, dimension and value. Should I omit it(How? it gives me error), or should I keep it and just put

Code:

Y[0] = Y0init;
Y[1] = Y1init;

Farzad

Quote:

Originally Posted by clapointe

Can you not do something like this?

Code:

Y[0] = Y0init;
Y[1] = Y1init;

Caelan

clapointe · December 19, 2019, 12:43

As established previously you cannot omit it. However, all of the necessary info is explained in that line. You just need to fill in the blanks (correct dimensions, (dummy) initial value).

Caelan

farzadmech · December 19, 2019, 12:49

Dear Caelan
I did what you suggested me;

Code:

label N = 2;
    PtrList<volScalarField> Yinit(N);
    forAll (Yinit, i)
    {
        word nameYiniti ("Yinit" + name(i));
        (
            new volScalarField
            (
                IOobject
                (
                    nameYiniti,
                    runTime.timeName(),
                    mesh,
                    IOobject::MUST_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh
            )
        );		
    }

cccccccccccccccccccccccccccccccccccccccccccccccccc cccccccccccccc

Code:

PtrList<volScalarField> Y(N); //
forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Yi",
                runTime.timeName(),
		        mesh,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
                mesh,
                 dimensionedScalar("Y", dimless, 0.0)       
        )
    );
}

cccccccccccccccccccccccccccccccccccccccccccccccccc cccccccccccccc

Code:

In file included from /home/thomas/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/postProcess.H:135:0,
                 from DPMFoamBFD.C:59:
./createFields.H: In function ‘int main(int, char**)’:
./createFields.H:140:8: error: ‘Yinit0’ was not declared in this scope
 Y[0] = Yinit0;
        ^
In file included from DPMFoamBFD.C:66:0:
createFields.H:140:8: error: ‘Yinit0’ was not declared in this scope
 Y[0] = Yinit0;

Quote:

Originally Posted by clapointe

As established previously you cannot omit it. However, all of the necessary info is explained in that line. You just need to fill in the blanks (correct dimensions, (dummy) initial value).

Caelan

clapointe · December 19, 2019, 12:55

I wrote it following the code you wanted, but you declared the init vars as part of a Ptr list. So you need to access the individual fields as e.g. :

Code:

Y[0] = Yinit[0];

Caelan

Daniel_Khazaei · December 19, 2019, 13:11

Well I'm not getting what exactly you are trying to do here...
If Y[i] is supposed to be initialized immediately from Yinit[i] which is being read from the case 0 directory, then why not defining Y[i] using IOobject::MUST_READ at first place?

I think you already know that this piece of code is defining Y[i] and initilize it with an initial dimension and value that can be altered any where in the code.

Code:

PtrList<volScalarField> Y(N);
forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Y" + name(i),
                runTime.timeName(),
                mesh,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            mesh,
            dimensionedScalar("Y", dimless, 0.0)       
        )
    );
}

If for some unknown reason you need to define Y[i] as NO_READ and then initialize it with Yinit[i], you can always do:

Code:

PtrList<volScalarField> Y(N); //
forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Y" + name(i),
                runTime.timeName(),
                mesh,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            Yinit[i],
            Yinit[i].boundaryField().types()
        )
    );
}

Be-careful, as if you need to solve for Y[i] anywhere in the code then you have to apply physical boundary conditions.
In the above code, I assumed that Yinit[i] which is being read from the disk is providing correct boundary conditions.

farzadmech · December 19, 2019, 13:30

Dear Daniel
What I am trying to do is this;
I want to create two volScalarFields Y[0] and Y[1] which must be read from Y0 and Y1 respectively(from 0 folder). So what are you saying me is that both creating volScalarField and Reading can be done with a just 1 piece of code? Could you please give me this piece of code(meanwhile I am trying to do it myself).

Farzad

Quote:

Originally Posted by Daniel_Khazaei

Well I'm not getting what exactly you are trying to do here...
If Y[i] is supposed to be initialized immediately from Yinit[i] which is being read from the case 0 directory, then why not defining Y[i] using IOobject::MUST_READ at first place?

I think you already know that this piece of code is defining Y[i] and initilize it with an initial dimension and value that can be altered any where in the code.

Code:

PtrList<volScalarField> Y(N);
forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Y" + name(i),
                runTime.timeName(),
                mesh,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            mesh,
            dimensionedScalar("Y", dimless, 0.0)       
        )
    );
}

If for some unknown reason you need to define Y[i] as NO_READ and then initialize it with Yinit[i], you can always do:

Code:

PtrList<volScalarField> Y(N); //
forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Y" + name(i),
                runTime.timeName(),
                mesh,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            Yinit[i],
            Yinit[i].boundaryField().types()
        )
    );
}

Be-careful, as if you need to solve for Y[i] anywhere in the code then you have to apply physical boundary conditions.
In the above code, I assumed that Yinit[i] which is being read from the disk is providing correct boundary conditions.

Daniel_Khazaei · December 19, 2019, 14:23

Quote:

Originally Posted by farzadmech

Dear Daniel
What I am trying to do is this;
I want to create two volScalarFields Y[0] and Y[1] which must be read from Y0 and Y1 respectively(from 0 folder). So what are you saying me is that both creating volScalarField and Reading can be done with a just 1 piece of code? Could you please give me this piece of code(meanwhile I am trying to do it myself).
Farzad

This will create a list of pointers that hold memory address of your volScalarField objects:

Code:

PtrList<volScalarField> Y(N);

Now you can initialize this list using:

Code:

forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Y" + name(i),
                runTime.timeName(),
                mesh,
                IOobject::AUTO_READ,
                IOobject::AUTO_WRITE
            ),
            mesh
        )
    );
}

This will create N number of volScalarFields that reads Y0...YN from case/0 directory.

farzadmech · December 19, 2019, 14:51

Dear Daniel
It worked and I pass that error. Thanks!

Just for researchers who are looking to our conversation there is typo which the correct one is in below;

Code:

forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Y" + name(i),
                runTime.timeName(),
                mesh,
                IOobject::MUST_READ,
                IOobject::AUTO_WRITE
            ),
            mesh
        )
    );
}

Quote:

Originally Posted by Daniel_Khazaei

This will create a list of pointers that hold memory address of your volScalarField objects:

Code:

PtrList<volScalarField> Y(N);

Now you can initialize this list using:

Code:

forAll (Y, i)
{
    Y.set
    (
        i,
        new volScalarField
        (
            IOobject
            (
                "Y" + name(i),
                runTime.timeName(),
                mesh,
                IOobject::AUTO_READ,
                IOobject::AUTO_WRITE
            ),
            mesh
        )
    );
}

This will create N number of volScalarFields that reads Y0...YN from case/0 directory.

December 17, 2019, 20:20	several volscalarfield named Y[i]	#1
farzadmech Senior Member Farzad Faraji Join Date: Nov 2019 Posts: 204 Rep Power: 7	Dear Friends How can I define two(or several) volscalarfield named Y[i] with two members Y[1] and Y[2]? Many thanks Farzad

December 18, 2019, 09:54		#2
clapointe Senior Member Join Date: Aug 2015 Posts: 494 Rep Power: 14	Sounds similar to what is done for reacting solvers. So, something like this should be helpful : Code: PtrList<volScalarField> Y(2); // forAll (Y, i) { Y.set ( i, new volScalarField ( IOobject ( "Yi", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), i ) ); } Caelan farzadmech likes this.

December 18, 2019, 10:59	thanks	#3
farzadmech Senior Member Farzad Faraji Join Date: Nov 2019 Posts: 204 Rep Power: 7	Dear Caelan Thanks for your response. I did what you have said and I got this error; ./createFields.H:132:9: error: no matching function for call to ‘Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject, Foam::label&)’ ) ^ could you please check this error too? Thanks, Farzad

December 18, 2019, 12:12		#5
clapointe Senior Member Join Date: Aug 2015 Posts: 494 Rep Power: 14	Thanks to Daniel, who corrected my code snippet. I should have included that "i" was a placeholder that must be replaced with correct info to instantiate a volScalarField. Caelan farzadmech likes this.

December 18, 2019, 17:26		#7
clapointe Senior Member Join Date: Aug 2015 Posts: 494 Rep Power: 14	As for 1), you can likely edit the fields once you create them with something like : Code: forAll(Y[i], celli) { if (<insert condition here>) { Y[i][celli] = <insert value here> } } For 2), I am not sure what you are trying to do but it does appear to have a problem with your use of the kinematicCloud source term. Caelan farzadmech likes this.

December 19, 2019, 12:29		#9
clapointe Senior Member Join Date: Aug 2015 Posts: 494 Rep Power: 14	Can you not do something like this? Code: Y[0] = Y0init; Y[1] = Y1init; Caelan

December 19, 2019, 12:43		#11
clapointe Senior Member Join Date: Aug 2015 Posts: 494 Rep Power: 14	As established previously you cannot omit it. However, all of the necessary info is explained in that line. You just need to fill in the blanks (correct dimensions, (dummy) initial value). Caelan

December 19, 2019, 12:55		#13
clapointe Senior Member Join Date: Aug 2015 Posts: 494 Rep Power: 14	I wrote it following the code you wanted, but you declared the init vars as part of a Ptr list. So you need to access the individual fields as e.g. : Code: Y[0] = Yinit[0]; Caelan farzadmech likes this.

December 19, 2019, 13:11		#14
Daniel_Khazaei Senior Member Daniel Join Date: Mar 2013 Location: Noshahr, Iran Posts: 348 Rep Power: 21	Well I'm not getting what exactly you are trying to do here... If Y[i] is supposed to be initialized immediately from Yinit[i] which is being read from the case 0 directory, then why not defining Y[i] using IOobject::MUST_READ at first place? I think you already know that this piece of code is defining Y[i] and initilize it with an initial dimension and value that can be altered any where in the code. Code: PtrList<volScalarField> Y(N); forAll (Y, i) { Y.set ( i, new volScalarField ( IOobject ( "Y" + name(i), runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), mesh, dimensionedScalar("Y", dimless, 0.0) ) ); } If for some unknown reason you need to define Y[i] as NO_READ and then initialize it with Yinit[i], you can always do: Code: PtrList<volScalarField> Y(N); // forAll (Y, i) { Y.set ( i, new volScalarField ( IOobject ( "Y" + name(i), runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), Yinit[i], Yinit[i].boundaryField().types() ) ); } Be-careful, as if you need to solve for Y[i] anywhere in the code then you have to apply physical boundary conditions. In the above code, I assumed that Yinit[i] which is being read from the disk is providing correct boundary conditions. farzadmech likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
y+ and u+ values with low-Re RANS turbulence models: utility + testcase	florian_krause	OpenFOAM	114	August 23, 2023 05:37
Near wall treatment in k-omega SST	Arnoldinho	OpenFOAM Running, Solving & CFD	38	March 8, 2017 13:48
[OpenFOAM] Native ParaView Reader Bugs	tj22	ParaView	270	January 4, 2016 11:39
writing execFlowFunctionObjects	immortality	OpenFOAM Post-Processing	30	September 15, 2013 06:16
Problem with compile the setParabolicInlet	ivanyao	OpenFOAM Running, Solving & CFD	6	September 5, 2008 20:50