Coupled problem NS/Heat Equation

[julien]

Hello
I would like to simulate a convective heat exchange between two aluminium plates and a water flow. I know the external temperature of the aluminium plates and the pressure difference at the border of the water flow. On the water I applied the heat equation coupled with the Navier Stokes equation. As long as I don’t active the “computed” convection, I obtain coherent results with only diffusive heat exchange. When I then active the computed convection the Heat solver diverges. I attached the .sif files without activated convection term, additionally you will find the .sif file with activated convection (Option NS Convect=true, Convection = Computed ). Could any of you give me a hint about some other options I might have missed?

Thanks in advance

Cheers,

[raback]

It was not totally clear to me whether you tried activating these flags only one in time. Activating "NS Convect" adds the nonlinear convective term in the Navier-Stokes equation while "Convection = Computed" takes the velocity field into use in the heat solver. The former is a more common reason for divergence (high Re number) than the latter. In fact, the heat equation should be quite robust with respect to the convection field. The fact the there are problems could indicate that the velocity field is ok. Also you should ensure that temperature is set at the inflow.

-Peter

[Christian]

Dear Peter,

thanks for your comments, we hadn't completely understood the NSConvect option (I thought that only enabling a buoyancy body force would enable the natural convection term). Now disabling that option at least led to convergency of the problem. BTW, inflow temperature is set.

Now there is a second problem with the one-way coupling (NSConvect=False, Convection=Computed): We see some instabilities in the temperature field that usually should only occur at Pecklet numbers > 1, however, we see them down to about 1e-3. I attached two pictures of the temperature profile along a cut. For the differencial pressure of 0.001Pa everything is very smooth, as would be expected. No instabilities. However, for the 1Pa case (Pe about 0.5) the temperature profile shows two negative peaks below 40°C, while the lowest BC temperature is 40°C. Cna you give us some hints how to overcome that, as refining the mesh so strongly is not an option for that case.

Thanks a lot and all the best wishes,

Christian

[raback]

Eliminating the intertial terms with "NS Convect = False" probably makes the coupled system more instable. I didn't mean that you should keep it this way, it was merely to test what the true reason for the divergence was. So the remedy here would be to change the setting for the N-S so that it will be more robust. Some relaxation and enforcing Picard linearization (by making the conditions for Newton iteration impossible) might work. Often in natural convection its best to use relaxation in both, just one nonlinear iteration and use the bullets in the coupled system level by setting the "Steady State Max Iterations" to high enough value.

-Peter

[dekoder87]

I had similar problem. When I set NS Convect=False I had got convergence in Navier Stokes equation, but my results were very inrealistic. I have solved part of problem.
For the convection calculation in material properties you need to set reference temperature.
Body force need to have Boussinesq to be set true.
Bubbles need to be set False. (This is used for compressible material model, default is incompressible)
Stabilisation need to be set True.
NS Convect = True
Convection = Computed

[dekoder87]

Finally I have managed to calculate nonlinear coupled heat equation and Navier-Stokes.
I want to share my experience to help people working with elmer.
First of all to calculate coupled case it is good to use transcient simulation. After high number of time steps when you get good convengence last time step is same as steady state should be. in my case I have set up 4000 time steps intervals and time step size 2 s.
As raback has written I have set up relaxation = 0.2 in non-linear solver settings and forced Picard itterations to achieve convergence. Also setting just one non-linear itteration for Navier-Stokes and Heat equation was helpful.
I have set up stabilisation=true, bubbles=false, compresibility model=incompresible, NS convect=true, Convection=Computed. I have set up reference temperature as 293 for air in material properties. To achieve faster convergence I have choosen BiCGStabl linear solver with maximum nr of 2000 itterations and ILU3 preconditioning, but one may choose different settings to tune up convergence. Maximum nr of steady state itteration was set up to 1000. This settings allowed me to achieve slowly convergence in few first time steps, but once converged my calculation speed up in next time steps.
Initial Condition for simulation are helping to get good initial guess for field of temperature, pressure and velocity which is helping to achieve good convergence.
Also good boundary conditions are essential, if they are wrong convergence will be affected.
I hope that this tips will be helpful.
I apologize for mistakes in my english language.