# Using ODE in OpenFoam

 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 9, 2007, 18:00 Using ODE in OpenFoam #1 Senior Member   Senthil Kabilan Join Date: Mar 2009 Posts: 113 Rep Power: 10 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& 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::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; } // ************************************************** *********************** // ahmmedshakil and Zhiheng Wang like this.

 October 19, 2007, 14:23 Hi, I figured out how to so #2 Senior Member   Senthil Kabilan Join Date: Mar 2009 Posts: 113 Rep Power: 10 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! Zhiheng Wang likes this.

 October 19, 2007, 14:56 Good work! Does the solution c #3 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 14 Good work! Does the solution compare well to the analytical result?

 February 19, 2008, 18:01 Hello there Does anyone kno #4 New Member   Bernardo D Flores Join Date: Mar 2009 Posts: 21 Rep Power: 10 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

 September 2, 2015, 19:30 #5 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 Hi, Can you please explain in more details the steps of solving an ODE in OpenFOAM? Thanks, Methma

 September 9, 2015, 07:30 #6 Senior Member   Hassan Kassem Join Date: May 2010 Location: Germany Posts: 236 Rep Power: 11 Did you try ODE test? Also check this tutorial meth likes this.

 September 14, 2015, 02:54 #7 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 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. 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

 September 14, 2015, 03:12 #8 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 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. 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

 September 14, 2015, 03:24 #9 Senior Member   Hassan Kassem Join Date: May 2010 Location: Germany Posts: 236 Rep Power: 11 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 meth likes this. __________________ @HIKassem | HassanKassem.me

 October 7, 2015, 01:17 #10 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 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

October 7, 2015, 06:17
#11
Senior Member

Hassan Kassem
Join Date: May 2010
Location: Germany
Posts: 236
Rep Power: 11
Quote:
 Originally Posted by meth 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;

Code:
```// define a dictionary first
dictionary forcesDict;

// create force object
forces f("forces", db(), forcesDict);
// calculate the forces
f.calcForcesMoment();
// finally you can get the forces and moment
vector F = f.forceEff();
vector M = f.momentEff();```
Best wishes,
Hassan

 October 7, 2015, 18:38 #12 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 Thanks a lot Hassan, I will go through the links you mentioned. I hope this is very helpful. Best, Methma

 October 29, 2015, 01:22 #13 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 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.

October 29, 2015, 05:01
#14
Senior Member

Hassan Kassem
Join Date: May 2010
Location: Germany
Posts: 236
Rep Power: 11
Quote:
 Originally Posted by meth 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

 October 30, 2015, 03:37 #15 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 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

 October 30, 2015, 03:51 #16 Senior Member   Hassan Kassem Join Date: May 2010 Location: Germany Posts: 236 Rep Power: 11 If you have mesh or time reference pass it, if not try the velocity Field U.dB() meth likes this. __________________ @HIKassem | HassanKassem.me

October 31, 2015, 23:47
#17
Member

methma Rajamuni
Join Date: Jul 2015
Location: Victoria, Australia
Posts: 36
Rep Power: 4
Quote:
 Originally Posted by hk318i 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

 November 1, 2015, 19:28 #18 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 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 hk318i likes this.

 November 2, 2015, 19:25 #19 Member   methma Rajamuni Join Date: Jul 2015 Location: Victoria, Australia Posts: 36 Rep Power: 4 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

 November 5, 2015, 06:29 #20 Senior Member   Hassan Kassem Join Date: May 2010 Location: Germany Posts: 236 Rep Power: 11 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 meth likes this.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post tangd OpenFOAM Running, Solving & CFD 33 May 23, 2010 16:36 martapajon OpenFOAM Native Meshers: blockMesh 7 January 21, 2008 13:52 jaswi OpenFOAM 0 August 3, 2007 13:11 mbeaudoin OpenFOAM Installation 2 April 28, 2006 08:54 navaladi OpenFOAM 3 March 28, 2006 09:08

All times are GMT -4. The time now is 03:36.