[user369]

Hi,
I am new to CFD and OpenFOAM.
I am trying to learn OpenFOAM and creating a simple problem and solve it using OpenFOAM.
I would like to solve a steady-state 2d poisson problem, similar to
Laplacian(U) = 50 * (x + y)
where x and y are the coordinates of cell centers.

I am not sure how to represent the source term in the OpenFOAM program.
I have represented this equation in my solver application as

volScalarField x = U.mesh().C() & vector(1,0,0);
volScalarField y = U.mesh().C() & vector(0,1,0);
fvVectorMatrix UEqn
(
      fvm::laplacian(U) == 50 * (x + y)
);
UEqn.solve();

but, this throws error during compilation, where the error says something like
"note: no known conversion for argument 1 from ‘Foam::tmp<Foam::fvMatrix<Foam::Vector<double> > >’ to ‘const Foam::instant&’"

What is the right way to specify the source terms in the equation?

Thanks in advance.

[Cyp]

Hi! and welcome on board

your first error is obvious : You add x and y which are scalarFields whereas laplacian(U) is a vectorField !

You should define x and y as volVectorField !

Best,
Cyp

[user369]

Cyp,
Thanks a lot for the reply..

I have modified the problem to convert the scalar to vector.

volScalarField x = U.mesh().C() & vector(1,0,0);
volScalarField y = U.mesh().C() & vector(0,1,0);
dimensionedScalar fifty
(
    "fifty",
    dimensionSet(0, -2, -1, 0, 0, 0 ,0),
    50.0
);
fvVectorMatrix UEqn
(
    fvm::laplacian(U) == (fifty * (x + y)) * vector(1,0,0)
);

Now, the code compiles and runs without error.

But, if I try to modify the source term to contain exponential, it compiles correctly, but fails to run with the following error:

fvVectorMatrix UEqn
(
    fvm::laplacian(U) == (exp(fifty * (x + y))) * vector(1,0,0)
);

--> FOAM FATAL ERROR: 
Argument of trancendental function not dimensionless

    From function trans(const dimensionSet& ds)
    in file dimensionSet/dimensionSet.C at line 370.

What is the correct way to take exponential of the coordinates?

Also, is the above method the right way to compute the source term for the equation, or are there any better ways to compute and pass it to the equation?

Thank you.

[Cyp]

are you sure about your differential equation ? in my opinion, you have something wrong. indeed, the inside of exponential must be unitless! In the other side, your source term ought to have the same dimension than laplacian(U).

[user369]

Cyp,
My governing eqn. is a second order pde of the form

Laplacian(phi) = exp(fifty * (x + y))

where, x and y are the co-ordinates of the points on the 2D plate.

x and y are actually dimensionless quantities
I have used the following operations to extract these coordinates, which returns me a dimensional quantity in meters.

        volScalarField x = U.mesh().C() & vector(1,0,0);
        volScalarField y = U.mesh().C() & vector(0,1,0);

Is my way of extracting the coordinates wrong? I tried to print the extracted values and they match the actual coordinates of my mesh cell centers.

Thank you

[mirko]

Originally Posted by user369

Cyp,
My governing eqn. is a second order pde of the form

Laplacian(phi) = exp(fifty * (x + y))

where, x and y are the co-ordinates of the points on the 2D plate.

x and y are actually dimensionless quantities
I have used the following operations to extract these coordinates, which returns me a dimensional quantity in meters.

        volScalarField x = U.mesh().C() & vector(1,0,0);
        volScalarField y = U.mesh().C() & vector(0,1,0);

Is my way of extracting the coordinates wrong? I tried to print the extracted values and they match the actual coordinates of my mesh cell centers.

Thank you

Can you define `fifty' as inverse meters?

[user369]

Thanks Mirko.. taking the fifty as inverse meters worked.

[mirko]

Originally Posted by user369

Thanks Mirko.. taking the fifty as inverse meters worked.

Now, let me ask you for a favor:

Would it be possible for you to package and post the solver files? I promise not to criticize the coding style and/or lack of comments

[user369]

Sure..
I have attached the solver files..
I am completely new to OpenFoam (this is my first code written in openfoam).. so the code is pretty immature and dumb..

I will also be happy to hear suggestions and better alternatives for the code..

[user369]

Similar to the equation for the source term, I would also like to specify the equations for the boundary conditions, which depends on the coordinates of the cells, like,
boundary value at south edge is 100x; where x is the x-coordinate of the face center.

Where should I specify those equations? Do I need to set the boundaryField type as "calculated" and specify the equations in the solver? or should I add the equations in the dictionary file itself?

Thanks.

[mirko]

Originally Posted by user369

Similar to the equation for the source term, I would also like to specify the equations for the boundary conditions, which depends on the coordinates of the cells, like,
boundary value at south edge is 100x; where x is the x-coordinate of the face center.

Where should I specify those equations? Do I need to set the boundaryField type as "calculated" and specify the equations in the solver? or should I add the equations in the dictionary file itself?

Thanks.

I think that you will need to write your own boundary condition. The procedure should be similar to that of copying and modifying an OF solver.

Note: to get the y coordinate, this should work:
scalarField y = patch().Cf().component(1);

Remember to compile it using `> wmake libso', not just `> wmake'.

Good luck.

Mirko

[Bernhard]

For the boundary condition. It would save you a lot of time if you use the groovyBC library. You can use easy expressions for the value or the gradient of a variable at the boundary.

You now hard-coded the source term in your solver, but that really makes your solver case-specific, which is usually unwanted. You can also easily define a field (see createFields), which you use as a source term. This source-field can then be set in your case-directory 0/. (using funkySetFields)

By the way, funkySetFields and groovyBC are combined in swak4Foam.

[user369]

Mirko and Bernhard,
Thank you very much for the reply..

I will look into the swak4Foam library...

[mechy]

Originally Posted by user369

Sure..
I have attached the solver files..
I am completely new to OpenFoam (this is my first code written in openfoam).. so the code is pretty immature and dumb..

I will also be happy to hear suggestions and better alternatives for the code..

can you send me test case file for your solver?

also I think it better that you specify the U as a scalar not vector
why you specify U as a vector ?

Best Regards