[Diro7]

The momentum equation in UEqn.H calls the function

turbulence->divDevReff(U)

which should return something like the divergence of the deviatoric part of the effective stress tensor (if I'm not wrong).

I never did it myself, but I'm pretty sure that if you look at the corresponding source code, you'll find it calls nu at some point.

Andrea

[mmohaqeqf]

Ok, below is my scalar transport equation with my desired source term added to my modified version of the simpleFoam:

while (simple.correctNonOrthogonal())
        {
            fvScalarMatrix DEqn
            (
                fvm::ddt(D)
              + fvm::div(phi, D)
              - fvm::laplacian(DT, D)
             ==
                sqrt((turbulence -> nu())/6)
                *sqrt(
                        pow((2*fvc::grad(U).ref().component(tensor::XX))-(2*fvc::grad(U).ref().component(tensor::YY)),2)
                      + pow((2*fvc::grad(U).ref().component(tensor::YY))-(2*fvc::grad(U).ref().component(tensor::ZZ)),2)
                      + pow((2*fvc::grad(U).ref().component(tensor::ZZ))-(2*fvc::grad(U).ref().component(tensor::XX)),2)
                      + 6*pow((fvc::grad(U).ref().component(tensor::XY) + fvc::grad(U).ref().component(tensor::YX)),2)
                      + 6*pow((fvc::grad(U).ref().component(tensor::XZ) + fvc::grad(U).ref().component(tensor::ZX)),2)
                      + 6*pow((fvc::grad(U).ref().component(tensor::YZ) + fvc::grad(U).ref().component(tensor::ZY)),2)
                     )
                + fvOptions(D)
            );

It compiles without error.
But when I apply it to a simple pipe flow (straight converging pipe), it spits out following error:

--> FOAM FATAL ERROR:

    [D[0 0 -1 1 0 0 0] ] + [(sqrt((nu|6))*sqrt((((((pow(((2*grad(U).component(0))-(2*grad(U).component(4))),2)+pow(((2*grad(U).component(4))-(2*grad(U).component(8))),2))+pow(((2*grad(U).component(8))-(2*grad(U).component(0))),2))+(6*pow((grad(U).component(1)+grad(U).component(3)),2)))+(6*pow((grad(U).component(2)+grad(U).component(6)),2)))+(6*pow((grad(U).component(5)+grad(U).component(7)),2)))))[0 1 -1.5 0 0 0 0] ]

    From void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = double]
    in file /opt/OpenFOAM/OpenFOAM-v2006/src/finiteVolume/lnInclude/fvMatrix.C at line 1352.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::exitOrAbort(int, bool) at ??:?
#2  void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::DimensionedField<double, Foam::volMesh> const&, char const*) at ??:?
#3  ? at ??:?
#4  ? at ??:?
#5  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#6  ? at ??:?
Aborted (core dumped)

Do you have any idea what might have gone wrong?

[ancolli]

Originally Posted by mmohaqeqf

Ok, below is my scalar transport equation with my desired source term added to my modified version of the simpleFoam:

while (simple.correctNonOrthogonal())
        {
            fvScalarMatrix DEqn
            (
                fvm::ddt(D)
              + fvm::div(phi, D)
              - fvm::laplacian(DT, D)
             ==
                sqrt((turbulence -> nu())/6)
                *sqrt(
                        pow((2*fvc::grad(U).ref().component(tensor::XX))-(2*fvc::grad(U).ref().component(tensor::YY)),2)
                      + pow((2*fvc::grad(U).ref().component(tensor::YY))-(2*fvc::grad(U).ref().component(tensor::ZZ)),2)
                      + pow((2*fvc::grad(U).ref().component(tensor::ZZ))-(2*fvc::grad(U).ref().component(tensor::XX)),2)
                      + 6*pow((fvc::grad(U).ref().component(tensor::XY) + fvc::grad(U).ref().component(tensor::YX)),2)
                      + 6*pow((fvc::grad(U).ref().component(tensor::XZ) + fvc::grad(U).ref().component(tensor::ZX)),2)
                      + 6*pow((fvc::grad(U).ref().component(tensor::YZ) + fvc::grad(U).ref().component(tensor::ZY)),2)
                     )
                + fvOptions(D)
            );

It compiles without error.
But when I apply it to a simple pipe flow (straight converging pipe), it spits out following error:

--> FOAM FATAL ERROR:

    [D[0 0 -1 1 0 0 0] ] + [(sqrt((nu|6))*sqrt((((((pow(((2*grad(U).component(0))-(2*grad(U).component(4))),2)+pow(((2*grad(U).component(4))-(2*grad(U).component(8))),2))+pow(((2*grad(U).component(8))-(2*grad(U).component(0))),2))+(6*pow((grad(U).component(1)+grad(U).component(3)),2)))+(6*pow((grad(U).component(2)+grad(U).component(6)),2)))+(6*pow((grad(U).component(5)+grad(U).component(7)),2)))))[0 1 -1.5 0 0 0 0] ]

    From void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = double]
    in file /opt/OpenFOAM/OpenFOAM-v2006/src/finiteVolume/lnInclude/fvMatrix.C at line 1352.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::exitOrAbort(int, bool) at ??:?
#2  void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::DimensionedField<double, Foam::volMesh> const&, char const*) at ??:?
#3  ? at ??:?
#4  ? at ??:?
#5  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#6  ? at ??:?
Aborted (core dumped)

Do you have any idea what might have gone wrong?

It is complaining about dimensional units, you must ensure the same dimensional units for each term you add. your left hand side has dimensional units of Kelvin per second and ur new term meters per second^1.5. Section 4.2.6 https://cfd.direct/openfoam/user-gui...c-file-format/

[mmohaqeqf]

Ok, thanks;


It seems like I am not gonna give up asking questions :-)


Based on what you said, assuming that D in my case is unitless, I cannot use a scalar as a source term in my right hand side, because a scalar is unitless, while the left hand side would have a unit of 1/time, right?
Meaning that I should first define a dimensioned scalar with the unit of 1/time and then use it in the right hand side as a source term, right?

[mmohaqeqf]

I wanted to thank you both, Alejandro and Andrea for your help guys;


My new solver with a scalar transport equation is compiling fine and my sample pipe flow simulation runs successfully.

[mmohaqeqf]

Hi Alejandro (ancolli);


I have a question about the dimensions in OpenFOAM, related to my new solver discussed here;


Say I have a scalar transport equation (transported scalar is D) with zero diffusion (so pure convection), that has a source term which has the form:


Source = C * (mag(U))^0.185


Note that this source term has been obtained experimentally and thus the C and 0.185 are empirical constants.


What I would do is to set the dimension of D as (assuming C is unitless):


[0 0.185 1.185 0 0 0 0]


to make sure both RHS and LHS of the transport eqn are of the same dimension. (Note that the LHS would have the dimension of D divided by time)
The solver compiles fine and I can successfully run it on a sample pipe flow.
The problem starts when I want to load it up in paraview. Paraview doesn't like this dimension in D file (i.e. [0 0.185 1.185 0 0 0 0]).


How can I work around it?

[jherb]

If you write your own code for the source term, you could e.g. use the value() method to get dimensionless cell values. Or you access the fields e. g. as volScalarField which neither does have dimension.


Or you change your equation to Source = C * (mag(U)/C2)^0.185 with C2 being a uniformDimensionedScalarField. See https://github.com/OpenFOAM/OpenFOAM...sionedFields.H

[ancolli]

Originally Posted by mmohaqeqf

Hi Alejandro (ancolli);


I have a question about the dimensions in OpenFOAM, related to my new solver discussed here;


Say I have a scalar transport equation (transported scalar is D) with zero diffusion (so pure convection), that has a source term which has the form:


Source = C * (mag(U))^0.185


Note that this source term has been obtained experimentally and thus the C and 0.185 are empirical constants.


What I would do is to set the dimension of D as (assuming C is unitless):


[0 0.185 1.185 0 0 0 0]


to make sure both RHS and LHS of the transport eqn are of the same dimension. (Note that the LHS would have the dimension of D divided by time)
The solver compiles fine and I can successfully run it on a sample pipe flow.
The problem starts when I want to load it up in paraview. Paraview doesn't like this dimension in D file (i.e. [0 0.185 1.185 0 0 0 0]).


How can I work around it?

Sorry, i just saw ur post ( i did not receive a notification....)
U can not assume that C is unitless... u should give dimensions to C. Then paraview will not complain, and like this ur problem is well posed

const dimensionedScalar C("C",dimensionSet(kg,m,s,K,mol,A,cd), 1000);//[kg m s K mol A cd] C = 1000

[Iain_symthe]

I have case where I want to specify a volumetric heat source (W/m3) as a function of space say heSource[i] = 1.0*x[i]*V[i]; I am trying to see if there is a way to integrate the volumetric heat source over volume so that I know what the total power is in Watts.

[EpicMega]

Hey can,anybody help me to have source term as a function of space in laplacian foam