I am trying to simulate forced convection heated pipe problem in openfoam using bouoyant pimple foam
I don't know why but i'm getting this error on running buoyantPimpleFoam
courant number is increasing continuosuly and Temperrature is reaching negative values which in turn is terminationg the solution process
- Switched the flow to laminar as it is easier to debug and the problem statement also doesn't seem to have any constraints specified regarding this. You may enable turbulence in our case and check if the turbulence parameters are defined correctly.
- Changed the values in the prgh file to match the ones in the problem statement.
- For the heated section, since the wall flux and the thermal conductivity of the fluid is given, there's an easier way to specify wall flux boundary condition. The tempearture gradient at heated surface can be calculated using Q/k.
- In the controlDict, I've enable dynamic time-stepping so that your simulation automatically calculates the time-step based on the specified maximum Courant number (maxCo 0.5). I've also changed the endTime and write just so that I can check the simulation for a small time frame. Please feel free to change that.
- The major change that I made though was in the thermophysicalProperties file. In your case files, you had used the Boussinesq eqution of state. This equation of state only works well within a certain termperature range (min-max temperature in the domain). In your case, since the system is constantly getting heated, the range of temperature in your domain will keep increasing as time goes on. I have currently set the case up with perfectGas equation of state (P=rho*R*T). I'm not sure if the ideal gas law holds for the given temperature range, but you can check other equations of state available in OpenFOAM.