[carolee]

Hi everybody,
I am new to openfoam, I am studying a laminar flow of water in a cylindrical tube with velocity 1m / s using simpleFoam and I need to add a source term in the momentum equation which is a force in the same direction of flow which should increase the velocity of the fluid flow a little bit, I tried with this method but the velocity remains at the same value and the flow becomes non-laminar, please who can help me to solve this problem

dimensionedVector F("F", dimensionSet(0,1,-2,0,0,0,0), vector(0,0,30));

tmp<fvVectorMatrix> tUEqn
(
fvm::div(phi, U)
+ MRF.DDt(U)
+ turbulence->divDevReff(U)
- fvm::laplacian(mu, U)
==
fvOptions(U)
+ F

);

fvVectorMatrix& UEqn = tUEqn.ref();

[carolee]

any reply will be appreciated, I really want help

[Hgholami]

Hello
may you can use temple of bodyForce() in fsi of foam-extend4.0 (unsTotalLagrangianSolid.C).

bodyForce() = dimensionedVector(solidProperties().lookup("g"));

fvVectorMatrix DEqn
(
rho_*fvm::d2dt2(D_)
== fvm::laplacian(2*muf_ + lambdaf_, D_, "laplacian(DD,D)")
+ fvc::div
(
mesh().Sf()
& (
- (muf_ + lambdaf_)*gradDf_
+ muf_*gradDf_.T()
+ lambdaf_*(I*tr(gradDf_))
)
)
+ rho_*bodyForce()
);

[carolee]

thank you gholami for your reply

[pferro]

Hello,


For instance you can :
1 : declare a volVectorField mySource.

2 : loop over the cells and fill mySource. Here you can loop on a specific zone of your mesh.

3 : add in the left member of Ueqn the source mySource.

Good luck !

[pferro]

Hello,

Please find below some details of a possible implementation. Note that I didn't have tested the code since I am directly writing it here. Also note that there are other ways for doing it.

I assume that we use an incompressible solver such as simpleFoam or pimpleFoam. In this case each member of the momentum equation is divided by rho. As rho is uniform the solver use the kinematic viscosity and a modified pressure : [p/rho] = m^2 / s^2.

The source term in the momentum equation has the dimension of an acceleration i.e = m/s^2.

First step : creating the momentum source

In createField.H of the solver we declare a volVectorField and we call it force.

volVectorField force
(
IOobject
(
"force",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh,
dimensionedVector("0", dimVelocity/dimTime, Zero)
);

On the code above we use

AUTO_WRITE

this will be useful for visualizing the field in paraview.

Second step : filing the momentum source

The force volVectorField is initialized in createField.H and is equal to 0 on the whole mesh. Now we need to fill it according to what we want to do. Thus we need to create a loop over cells. For example we can do that in the UEqn.H file. This means that the source will be updated for each SIMPLE loop.

forAll(mesh.cells(),cellI)
{
// here do whatever you want to do
// for example we calculate force only if x > 0.5
// you can obtain cell center coordinates

const vector& cCenterCoor = mesh.C()[cellI];

// and create a test on the cell position
scalar xMax = 0.5 ;
if ( (pos(cCenterCoor[0] - xMax) )
{
force[cellI] = vector(1.,-1.,0.05); // again it's an example
}
else
{
force[cellI] = vector(0.,0.,0.); // if the condition above is not valid then the source remains zero
}
}
;

Third step : adding the source in Ueqn

Very simple :

fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi,U)
+ turbulence->divDevReff(U)
- force
==
fvOptions(U)
);

Final step : compile

wmake

Good luck !

Paulin

[Mahmoud Abbaszadeh]

Originally Posted by pferro

Hello,

Please find below some details of a possible implementation. Note that I didn't have tested the code since I am directly writing it here. Also note that there are other ways for doing it.

I assume that we use an incompressible solver such as simpleFoam or pimpleFoam. In this case each member of the momentum equation is divided by rho. As rho is uniform the solver use the kinematic viscosity and a modified pressure : [p/rho] = m^2 / s^2.

The source term in the momentum equation has the dimension of an acceleration i.e = m/s^2.

First step : creating the momentum source

In createField.H of the solver we declare a volVectorField and we call it force.



On the code above we use this will be useful for visualizing the field in paraview.

Second step : filing the momentum source

The force volVectorField is initialized in createField.H and is equal to 0 on the whole mesh. Now we need to fill it according to what we want to do. Thus we need to create a loop over cells. For example we can do that in the UEqn.H file. This means that the source will be updated for each SIMPLE loop.



Third step : adding the source in Ueqn

Very simple :


Final step : compile



Good luck !

Paulin

Hi Paulin,

I am wondering why you have not used fvOptions to introduce the body force into your equations?