CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Transient Natural convection heat storage problem (https://www.cfd-online.com/Forums/fluent/181769-transient-natural-convection-heat-storage-problem.html)

 sbesarati December 20, 2016 19:07

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 piecewise-polynomial 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

 Antanas December 21, 2016 01:11

Quote:
 Originally Posted by sbesarati (Post 630644) 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 piecewise-polynomial 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
1. Rayleigh numbers less than 10^8 indicate a buoyancy-induced laminar flow, with transition to turbulence occurring over the range of 10^8 < Ra <10^10. So your Ra number indicates that your flow is turbulent.

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.

 sbesarati December 21, 2016 16:32

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 k-e 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 1e-10 and 1e-05, respectively. However, the velocity and k,e residuals decrease first and then stabilize around 1e-02. 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.

 Antanas December 21, 2016 17:09

Quote:
 Originally Posted by sbesarati (Post 630828) 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 k-e 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 1e-10 and 1e-05, respectively. However, the velocity and k,e residuals decrease first and then stabilize around 1e-02. 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.
For bouyancy driven flows it is usually recommended to use transient solver. You don't have to take care of your near wall mesh unless you use standart wall functions for k-e model.

 sbesarati December 21, 2016 17:28

I also tried the transient solver. I am using k-e 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?

 Antanas December 22, 2016 02:15

Quote:
 Originally Posted by sbesarati (Post 630832) Thanks for your reply. I also tried the transient solver. I am using k-e 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?
There may be diffirent reasons why residuals don't decrease. Note that residual are not always good indicator of convergence. For example, if the residuals have met the specified convergence criterion but are still decreasing, the solution may not yet be converged. If the residuals never meet the
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 k-e model. For guidelines for solving natural convection flows refer to section 13.2.4. Natural Convection and Buoyancy-Driven Flows of Fluent User's Guide.

 All times are GMT -4. The time now is 02:58.