
[Sponsors] 
Transient Natural convection heat storage problem 

LinkBack  Thread Tools  Search this Thread  Display Modes 
December 20, 2016, 18:07 
Transient Natural convection heat storage problem

#1 
New Member
Saeb
Join Date: Dec 2016
Posts: 6
Rep Power: 8 
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 

December 21, 2016, 00:11 

#2  
Senior Member
Join Date: Feb 2011
Posts: 495
Rep Power: 17 
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. 

December 21, 2016, 15:32 

#3 
New Member
Saeb
Join Date: Dec 2016
Posts: 6
Rep Power: 8 
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. 

December 21, 2016, 16:09 

#4  
Senior Member
Join Date: Feb 2011
Posts: 495
Rep Power: 17 
Quote:


December 21, 2016, 16:28 

#5 
New Member
Saeb
Join Date: Dec 2016
Posts: 6
Rep Power: 8 
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? 

December 22, 2016, 01:15 

#6  
Senior Member
Join Date: Feb 2011
Posts: 495
Rep Power: 17 
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. 

Tags 
buoyancy, convergence, heat storage, natural convection, transient 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Heat transfer between two closed cavities with natural convection  Czarulla  FLUENT  2  August 5, 2020 12:36 
Heat transfer, natural convection: Heat sink <> Air  SvenH  OpenFOAM Running, Solving & CFD  10  March 11, 2020 04:40 
convergenceof natural convection prob. in cfx  cpkewat  CFX  15  January 31, 2014 06:29 
natural convection problem with radiation  jorien  CFX  0  October 14, 2011 09:26 
natural convection problem for a CHT problem  SeHee  CFX  2  June 10, 2007 06:29 