Transient Natural convection heat storage problem
Dear friends,
I am trying to model a 2D tank which is fully filled with liquid salt. The heat is transferred from bottom of the tank (constant heat flux) and the other three faces are adiabatic. The heat is transferred over 8 hours, and I am supposed to find out the temperature distribution in the tank after this time. I am using the transient model with PISO scheme, Body forced weighted pressure discretization, and first order momentum and energy discretization. I calculated the Raleigh number and it is in the order of 10^14. For the fluid properties including density, I entered the coefficients for the piecewisepolynomial model. I also used laminar as the viscous model. The problem is that the model does not converge for each time step. I understand that the Rayleigh number is high and in the steady state problems it is recommended to start the solution with a lower "g" and gradually increase it step by step. However, my problem is transient. Moreover, I am not sure what the appropriate time step is, as I have to run the simulation to get the solution at 8th hour and a very small time step e.g. 0.001, leads to very high run time. I really appreciate if you could please give me some recommendations. Thanks 
Quote:
2. Estimatation for time step for natural convection problems is dt = sqrt(L / (g * Beta * dT)), L  characteristic length, Beta  thermal expansion coefficient, dT  temperature difference. 3. Use Double Precision, BFW for Pressure discretization, URF = 0.7 for Pressure, 0.3 for Momentum. 4. Initialize your velocity field with small component opposite to g vector direction. 
Thank you very much for taking the time to answer my question.
Today, I tried to get help from your comments and run the system in the steady state mode for a simpler physic, i.e. two fixed temperature walls at the sides of the tank. I chose ke standard as the turbulence model, double precision, BFW for Pressure discretization, URF = 0.7 for Pressure, 0.3 for Momentum. The energy and continuity residuals are in the order of 1e10 and 1e05, respectively. However, the velocity and k,e residuals decrease first and then stabilize around 1e02. I checked the velocity vector plot and it seems the model shows the direction of vectors as expected, while the values are most probably inaccurate. The y+ values close to the walls are in the range of 3.5, and as I understand this is much lower than the recommended value, i.e 30. I was wondering if you could please give me some other recommendations to help me converge the solution. Moreover, should I increase the y+ values? I tried to coarsen the mesh, but it didn't help very much. 
Quote:

Thanks for your reply.
I also tried the transient solver. I am using ke model with standard wall function. The velocity residuals are still above the residual values. Should I use other turbulent models to reduce the residuals and have the y+ values inside the acceptable ranges? 
Quote:
convergence criterion, but are no longer decreasing and other solution monitors do not change either, the solution is converged. Low residuals do not automatically mean a correct solution, and high residuals do not automatically mean that solution is incorrect. Refer to section 29.22. Convergence and Stability of Fluent User's Guide. Based on your y+ value I suggest you to use scalable wall functions for ke model. For guidelines for solving natural convection flows refer to section 13.2.4. Natural Convection and BuoyancyDriven Flows of Fluent User's Guide. 
All times are GMT 4. The time now is 02:58. 