Using ODE in OpenFoam
 

Hi,

I am new to OpenFoam and was trying to use the ODE
solver. I took a look at the ODETest but was not able to understand how the equations are cast. can some one show me how I can solve a simple system like the following?

C --- INITIAL VALUES
X=0.0D0
Y(1)=2.0D0
Y(2)=-0.66D0
C --- ENDPOINT OF INTEGRATION
XEND=2.0D0
XDELTA=0.2
C --- SYSTEM OF EQUATIONS
F(1)=Y(2)
F(2)=((1-Y(1)**2)*Y(2)-Y(1))/2.0


ODETest
\*---------------------------------------------------------------------------*/

#include "argList.H"
#include "IOmanip.H"
#include "ODE.H"
#include "ODESolver.H"
#include "RK.H"

using namespace Foam;

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

class testODE
:
public ODE
{

public:

testODE()
{}

label nEqns() const
{
return 4;
}

void derivatives
(
const scalar x,
const scalarField& y,
scalarField& dydx
) const
{
dydx[0] = -y[1];
dydx[1] = y[0] - (1.0/x)*y[1];
dydx[2] = y[1] - (2.0/x)*y[2];
dydx[3] = y[2] - (3.0/x)*y[3];
}

void jacobian
(
const scalar x,
const scalarField& y,
scalarField& dfdx,
Matrix<scalar>& dfdy
) const
{
dfdx[0] = 0.0;
dfdx[1] = (1.0/sqr(x))*y[1];
dfdx[2] = (2.0/sqr(x))*y[2];
dfdx[3] = (3.0/sqr(x))*y[3];

dfdy[0][0] = 0.0;
dfdy[0][1] = -1.0;
dfdy[0][2] = 0.0;
dfdy[0][3] = 0.0;

dfdy[1][0] = 1.0;
dfdy[1][1] = -1.0/x;
dfdy[1][2] = 0.0;
dfdy[1][3] = 0.0;

dfdy[2][0] = 0.0;
dfdy[2][1] = 1.0;
dfdy[2][2] = -2.0/x;
dfdy[2][3] = 0.0;

dfdy[3][0] = 0.0;
dfdy[3][1] = 0.0;
dfdy[3][2] = 1.0;
dfdy[3][3] = -3.0/x;
}
};


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Main program:

int main(int argc, char *argv[])
{
argList::validArgs.clear();
argList::validArgs.append("ODESolver");
argList args(argc, argv);

word ODESolverName(args.args()[1]);

testODE ode;
autoPtr<odesolver> odeSolver = ODESolver::New(ODESolverName, ode);

scalar xStart = 1.0;
scalarField yStart(ode.nEqns());
yStart[0] = ::Foam::j0(xStart);
yStart[1] = ::Foam::j1(xStart);
yStart[2] = ::Foam::jn(2, xStart);
yStart[3] = ::Foam::jn(3, xStart);

scalarField dyStart(ode.nEqns());
ode.derivatives(xStart, yStart, dyStart);

Info<< setw(10) << "eps" << setw(12) << "hEst";
Info<< setw(13) << "hDid" << setw(14) << "hNext" << endl;
Info<< setprecision(6);

for (label i=0; i<15; i++)
{
scalar eps = ::Foam::exp(-scalar(i + 1));

scalar x = xStart;
scalarField y = yStart;
scalarField dydx = dyStart;

scalarField yScale(ode.nEqns(), 1.0);
scalar hEst = 0.6;
scalar hDid, hNext;
odeSolver->solve(ode, x, y, dydx, eps, yScale, hEst, hDid, hNext);

Info<< scientific << setw(13) << eps;
Info<< fixed << setw(11) << hEst;
Info<< setw(13) << hDid << setw(13) << hNext
<< setw(13) << y[0] << setw(13) << y[1]
<< setw(13) << y[2] << setw(13) << y[3]
<< endl;
}

scalar x = xStart;
scalar xEnd = x + 1.0;
scalarField y = yStart;

scalarField yEnd(ode.nEqns());
yEnd[0] = ::Foam::j0(xEnd);
yEnd[1] = ::Foam::j1(xEnd);
yEnd[2] = ::Foam::jn(2, xEnd);
yEnd[3] = ::Foam::jn(3, xEnd);

scalar hEst = 0.5;

odeSolver->solve(ode, x, xEnd, y, 1e-4, hEst);
Info<< nl << "Analytical: y(2.0) = " << yEnd << endl;
Info << "Numerical: y(2.0) = " << y << ", hEst = " << hEst << endl;

Info << "\nEnd\n" << endl;

return 0;
}


// ************************************************** *********************** //

Hi, I figured out how to so
 

Hi,

I figured out how to solve ODE's using the above driver.

1) Change the dimension of the system.

abel nEqns() const
{
return 4;
}


2) Change the following equations accordingly

{
dydx[0] = -y[1];
dydx[1] = y[0] - (1.0/x)*y[1];
dydx[2] = y[1] - (2.0/x)*y[2];
dydx[3] = y[2] - (3.0/x)*y[3];
}

3) Specifiy the " scalar xStart " , " scalar xEnd " and you can specify the initial values for yStart's if required.

Feel free to contact if not clear!

Good work! Does the solution c
 

Good work! Does the solution compare well to the analytical result?

Hello there Does anyone kno
 

Hello there

Does anyone knows how to integrate the ODE on OpenFOAM, i.e., using a solver like icoFoam and a ODE system serving as input on icoFOAM inlets to be solved at each time step.

Any pointers are greatly appreciated

Regards

Hi,

Can you please explain in more details the steps of solving an ODE in OpenFOAM?

Thanks,

Methma

Did you try ODE test?

Also check this tutorial

Hi Hassan :),

I went through the tutorial you mentioned. I changed the ODETest.C file so that it contains my equations. After that I run the wmake command to complete the C file. It was compiled by making dependency list for source file. But I don't know how to get the results of the ODE solver:confused:. Can you please help me? I am new to OpenFOAM. I really need to understand this.

My final goal is to work on fluid structure interface (Study on vortex induced vibration of a sphere/cylinder on free stream). There I need to solve the structure motion ODE in each time step.

Thank you.

Methma

Hi Hassan :),

I went through the tutorial you mentioned. I changed the TestODE.C file so that it contains my equations. After that I run the wmake command to complete the C file. It was compiled by making dependency list for source file. But I don't know how to get the results of the ODE solver:confused:. When I compile the C file does it run automatically or do I need to run it separately? Can you please help me? I am new to OpenFOAM. I really need to understand this.

My final goal is to work on fluid structure interface (Study on vortex induced vibration of a sphere/cylinder on free stream). There I need to solve the structure motion ODE in each time step.

Thank you.

Methma

Hello,

I am working on similar project but for 3D wings.
The results of the ODE system are stored in y (in TestODE) which basically the initial conditions yStart.

Best wishes,
Hassan

Hi Hassan,

I went through the ODETest files and figured out how it works. I have implemented the ODE solver for the solid motion inside the icoFoam solver. Now, I need to take the force data to solve the solid motion solver in each time step. I went through the force.C and force.H files, but still have no idea how to use them to take the force data. I know the force.C file was written to write the force data, but I don't know how to edit those files to get the force data inside the icoFoam solver. I am not quite familiar with the library files and how OpenFoam uses the library files when we run a solver. So can you please help me on this?

Thanks.

Methma

Hello Methma,

That is a great progress, well done.
Regarding the forces class, it is not only for writing. You can use it to get the forces directly [LINK].
There is a very good example for that in OpenFOAM source in sixDoFRigidBody [LINK] library. Here is a snippet of this library;

Best wishes,
Hassan

:) Thanks a lot Hassan, I will go through the links you mentioned. I hope this is very helpful.

Best,

Methma

Hi Hassan,

I need your help again. I still could not do it. I have not quite understood how to deal with objectRegestry.

I know I have to give the corresponding objectRegestry as an argument to the force class when we construct a force object f. I have a little knowledge on objectRegistry class. I need to compute the force on the sphere boundary. So how should I initialise the objectRegestry and use it? Can you please give me some ideas on this.

I greatly appreciate your help.

Thank you.

Methma.

You don't have to initialise an objectRegestry, you all need to pass the current objectRegestry to construct the forces object. The solution is quite easy, you can pass a reference to time or mesh [LINK]. Actually both are objectRegestry objects. Also, if you have access to any field like velocity, you can get reference to objectRegestry using db() function.

Bw,
Hassan

hi Hassan,

When I simple db() as an argument to the force object in the compilation of the solver it pop up the following error

vivicoFoam.C: In function ‘int main(int, char**)’:
vivicoFoam.C:137:27: error: ‘db’ was not declared in this scope
forces f("forces", db(), forcesDict);

It seems like it does not automatically take the db() function of the objectRegistry object. So, how can I fix that?

Thanks,

Methma

If you have mesh or time reference pass it, if not try the velocity Field U.dB()

Thank you very much Hassan :) , It works, I think now things get clear and clear for me.

Best,

Methma

Hassan,

Thank you very much, with your help I did it. Now I am able to calculate the forces on the solid. So, I can move into the next step of the solver.

Thanks again :)

Best,

Methma

I want to impose a dirichlet boundary condition in Openfoam on the inlet patch with a time varying value calculated in each time step. For a example U = ( 1 y 0), where y is a value that I am calculating in each time step inside the solver. I know I have to use fixedValue type boundary condition which is uniform. Is there any inbuilt boundary condition which I can directly use or, do I need to create my own one? If I have to create a new boundary condition can you please give me some ideas and references.

Thank you :)

Methma

Hi Methma,

There are few options you have to tackle this case. First, you can create a new BC which calculates the velocity. For that you can check the time varying BCs. Your second option is to use codeStream to implement such BC. Your third option is to calculate this BC directly with the solver and updated each time step. This option discussed many times in this forum and you will find many useful tips on how to do it.
I will not go with the last option unless it is the only way because the BC will be solver dependent.

Bw,
Hassan