Conservatively Smoothing a Source Term
 

Hello all,

I am attempting to solve a conjugate heat transfer problem where viscous heating plays an important role in the overall process. I am solving the energy equation as follows:



Due to the nature of the problem, the viscous heating term varies many orders of magnitude over the width of a few cells, and causes some instabilities / oscillations when solving for the temperature. To combat this, I am hoping to implement some sort of smoothing algorithm which conserves the overall amount of viscous heating, but distributes it within a wider area to make the computation more stable. For instance in 1D, assuming a uniform grid spacing, this smoothing algorithm might turn a field that looks like this:

[ 1 1 1 10 1 1 1 ]

Into one which looks like this:

[ 1 2 3 4 3 2 1 ]

Ideally, the "width" of the spread would be controllable by the user. I am sure such an algorithm exists already, but I am not sure what the correct search terms would be, and my initial efforts to find such a method have not yielded any good leads.

If anyone has a suggestion for a method I might try, I would be grateful. Additionally, any other strategies I might try to increase the stability of the problem would be appreciated.

Thanks,
Kellis

Hello,

You can try to first interpolate to the faces and then avarage over the faces of the cell. The code would look like this:

This will smooth the source a bit

You can solve diffusion equation in pseudo-time, like that:




dimensionedScalar pseudoDeltaT ("dT", dimTime, 1.0);
dimensionedScalar Dphi ("Dphi", dimLength*dimLength/dimTime, 1.0);



solve
(
fvm::Sp(1.0/pseudoDeltaT, Phi)
- fvc::Sp(1.0/pseudoDeltaT, Phi)
- fvm::laplacian(Dphi, Phi)



);

What's the purpose of

fvm::Sp(1.0/pseudoDeltaT, Phi)
- fvc::Sp(1.0/pseudoDeltaT, Phi)

Numerical stability of the equations?

If you use diffusion equation w/o temporal term, then your Phi distribution will be smoothed across a whole domain. But with adjustment of ratio between "pseudoDeltaT" and Dphi you can tune how many cells around initial field will be affected during one pseudo iteration.

That's interesting. Can you recommend someone regarding about the method?

This is a simple idea, which arises from the concept of numerical diffusion of convection equation.


http://www.mathematik.tu-dortmund.de.../Transport.pdf


Or just walk around this personal page: http://www.mathematik.tu-dortmund.de/~kuzmin/

I used code from the CFDEMcoupling library to do something similar. You can copy the function from this GitHub repository. There are some user-defined lengths and lower/upper limits you can use to tune the diffusion.