[koala]

Hello,

I've got a simple question about the laplace equation combined with Neumann conditions. My case is a simple 3D box where Neumann conditions (zeroGradient) are applied to every face. The initial value for my variable T is set to 300. Now I'm trying to solve the equation

       solve
       (
           fvm::laplacian(k, T, "laplacian(k,T)")
       );

where k is a constant factor (> 0). The solution diverges directly after the first iteration step.

DICPCG:  Solving for pot, Initial residual = 0.6179873, Final residual = 8.546418e+08, No Iterations 20001

From my knowledge the variable T should be constant 300 since zeroGradient conditions are applied everywhere.

Is there a reason for this behavior? Is this problem maybe not well defined with the given BC?

Thanks for your help!

[student666]

I think it's correct to say that you're violating Cauchy's theorem. You can't define bc for first derivatives only.
Your calculation diverges because has infinite solutions.

Regards.

Sent from my ASUS_X008D using CFD Online Forum mobile app

[koala]

By Cauchy's theorem you mean the Cauchy–Kowalevski theorem?

Edit: If we assume the equation changes to

       solve
       (
           fvm::laplacian(k, T, "laplacian(k,T)") + S == 0
       );

and still apply only Neumann boundary conditions. Would this still violate Cauchy's theorem?

[alexeym]

1. Use Dirichlet BC on a single face. Similar to solution of Poisson equation for pressure in SIMPLE/PISO. I.e. in terms of OpenFOAM this is called setting reference cell.

2. Or you can go with this solution: https://math.stackexchange.com/quest...ary-conditions

There was another post on stackexchange concerning the problem, unfortunately I can not find it now, maybe you will be luckier.

[student666]

Solution exist if you set two gradients like this case.
https://www.dropbox.com/s/8gwaq3kgqa...umann.zip?dl=0

run

ideasUnvToFoam cad/Mesh_1.unv
laplacianFoam

[koala]

Thanks @alexeym now I understand the problem a bit more.
Thanks @student666 it converges indeed with the given Neumann conditions.

So if we assume a box with a source and a sink (e.g. the source is bigger than the sink) and Neumann conditions on all walls then my solution will always explode towards +infinity since there is no flux through the walls right?

In case of student666's proposed solution the solution converges since everything which is added due to the positive gradient is substracted due to the negative gradient?

[student666]

What kind of analysis you want to perform?

Sent from my ASUS_X008D using CFD Online Forum mobile app

[koala]

I'm trying to implement a potential equation for an electric potential which is basically the equation I provided above. A lot of papers I read about these potential equations (for my case) are saying that the boundary conditions are given by Neumann conditions (zeroGradient) since there's no potential flux across these borders. Further there is also a source and a sink given which are not of the same order.

So it seems like I'm misunderstanding something because under given equation (+ source/sink) and boundary conditions there's no stable simulation possible.

[student666]

I think you can use a very big domain with dirichlet bc in order that boundary are far away from your source and sink and the solution is not directly influenced by the bc. In this way your math formulation is correct

Sent from my ASUS_X008D using CFD Online Forum mobile app

[koala]

This approach is unfortunately not possible since the domain is limited in its size because it's included in some other domains. The source/sink is also close to the boundaries.

[student666]

Well, one last suggestion is that you define a very small patch, just a small face with a fixed value; sorry but more than this I can't be of help.
Good luck

Sent from my ASUS_X008D using CFD Online Forum mobile app