
[Sponsors] 
Some questions about flow boiling simulation in Fluent 

LinkBack  Thread Tools  Search this Thread  Display Modes 
April 19, 2016, 22:31 
Some questions about flow boiling simulation in Fluent

#1 
New Member
Join Date: Apr 2012
Posts: 17
Rep Power: 9 
Hello everyone,
I am currently working on critical heat flux (CHF) simulation using Fluent. The purpose of my simulation is to verify whether Fluent can serve as a reliable tool to predict critical heat flux (in DNB regime) by comparing my simulation results with the experimental data of Celata et al. (Int. J. Heat Mass Transfer, 36, 12691285, 1993). I ran the simulation using the experimental parameters given in the reference mentioned above. My strategy is to start the simulation with an initial heat flux which is about 70% of a reported critical heat flux for a given set of parameters (e.g., if the reported critical heat flux is 52 MW/m2, then the initial heat flux is 35 MW/m2) and increase the heat flux by 0.5 MW/m2 each time when I get convergence for a certain heat flux. I am planning to increase the heat flux until a sudden temperature jump somewhere along the heated wall is observed. More details about the model setting are given below. Model Setting: Steady State Axisymmetric Eulerian Multiphase Model => Boiling Model => Critical Heat Flux (Primary Phase = Liquid Water; Secondary Phase = Water Vapor) Realizable kepsilon model with Enhanced Wall Function Phase Interactions: Drag (ishii) Lift (moraga) Wall Lubrication (antaletal) Turbulent Dispersion (burnsetal) Turbulent Interaction (troshikohassan) Heat Transfer Coefficient (ranzmarshall) Mass (Enable Correction Model and fix Surface Tension (enable Surface Tension Force Modeling) Interfacial Area (iasymmetric) Simulation Geometry: A rectangle with height of 1.25 mm and height of 200 mm Boundary Condition: Lower side = Axis First 100 mm of the upper side = Adiabatic Wall Remaining 100 mm of the upper side = Constant Heat Flux (starting from 37 MW/m2) Left side = mass flow inlet (0.1712904 kg/s, velocity is about 35.02 m/s, temperature = 304.02 degC) Right side = Pressure outlet (Gauge Pressure = 0 Pa; Operating Pressure = 2.58 MPa) Solver Settings: PressureVelocity Coupling = Coupled Courant Number = 1~20 Under Relaxation Factor (energy and volume fraction = 0.1~0.3, the others are typically between 0.30.5) Gradient: Least Squared Cell Based Discretization for all equations: QUICK Mesh Setting (Total Mesh Number = 20,000): Structured Mesh Mesh in the direction perpendicular to flow Total Mesh Count = 40 Thickness of first cell adjacent to wall = 0.0096 mm => corresponding Y+ ranges from 10~35; Mesh growth rate is < 1.2) Mesh in the direction parallel with flow Uniform Spacing Total mesh count = 500 I have the following questions that I wonder if there is anyone who can give me some advises. 1. Energy imbalance increases with increasing heat flux Even though I can get residuals for all questions below 1e6 for every case, the energy imbalance still gets higher and higher every time I raise the heat flux (e.g, the energy imbalance are heat flux of 37, 40 and 43 MW/m2 are 5e5, 7.3e4 and 3.8e3). I have made sure that the important physical quantities reach steady values in each case. But still, this problem happens. I was wondering what causes the problem. 2. The temperature at the outlet is always lower As can be expected, the wall temperature increases with the distance from the inlet. Nevertheless, the wall temperature at the cell right adjacent to outlet always shows a lower temperature (2030 degC lower than the cell upstream). The same results can also be found in Ansys Fluent’s tutorial “Modeling Nucleate Boiling Using ANSYS FLUENT”. Is this caused by some kind of constraint of pressure outlet boundary condition? 3. Convergence When the heat flux is relatively low, it is quite easy to get convergence. However, it will get harder and harder every time I increase the heat flux. When I raise the heat flux to 4.31E7 Wm2, I can no longer get convergence. So far, I have tried (a) enable or disable “coupled with volume fraction” option, (b) enable or disable “with higher terms underrelaxation” option, (c) start with “first order” discretization scheme and return to QUICK scheme, (d) start the simulation without “lift force” and turn it back on and (e) use the pseudo transient option and reduce the timescale factor to 0.001. But none of these methods works. The residuals keep fluctuating around 1E2. I really hope there is someone that can give me some advises. Any comment or suggestion would be highly appreciated. 

April 20, 2016, 14:59 

#2 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,583
Rep Power: 44 
2. The discretization schemes change at cells adjacent to boundaries. For example, with QUICK you need a downstream cell and there is no downstream cell available for a cell that is adjacent to an exit boundary. Hence the solver switches to a 1st order upwind scheme. This switch can cause little wiggles in the solution.
1&3 is really the same question about residuals. In general, residuals do not give information about convergence, so this really isn't a question of whether the solution is converged but really a question of why the residuals aren't decreasing. There are too many reasons for why residuals are not decreasing, but the first thing to check is your mesh. Is your mesh highquality? Does it have any skewed cells? Skewed cells can limit your residual reduction because it constantly introduces oscillations into your solution field every iteration. If you find that you are able to achieve residual reduction for some cases and not other cases, observe if there are dramatic changes in the solution field. It might be that your mesh resolution is insufficient for all your operating conditions. 

April 22, 2016, 12:33 

#3 
New Member
Join Date: Apr 2012
Posts: 17
Rep Power: 9 
Thanks so much for your reply.
Your response to my second question really solve a doubt that I have for a long time. On the other hand, I judged the convergence based on the following criteria: (1) residuals below at least 1e5, (b) acceptance level of energy and mass balance (energy imbalance: <0.05% and mass imbalance: <1e7) and (3) constant values of important physical quantities, such as temperature and vapor volume fraction. I learned this from your informative posts on this forum. Thanks again. I used structure mesh for my simulation (please see the attached file Mesh.jpg). I have tried three different mesh sizes. In each case, the mesh setting in the vertical direction is the same. However, I change the mesh size in the horizontal direction (the attached file mentioned above shows the coarsest mesh). I am not sure if the aspect ratio of the mesh is good enough. However, the other attached file Results.jpg shows that the results are almost the same for the three different meshes I used. When the heat flux is below 42 MW/m2, the plot of vapor volume fraction on the heated wall is quite smooth. Nevertheless, at heat flux of 43 MW/m2, the plot looks a bit twisted, especially near the outlet. When the heat flux is raised to 43.1 MW/m2, the simulation diverges and drastic jump in vapor volume fraction is observed in the locations near the outlet. Also, Fluent shows the warning message that some of the cells reaches lowest or highest temperatures. It would be highly appreciated if you can give me some advise. Thanks for your reply again. 

April 22, 2016, 17:45 

#4 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,583
Rep Power: 44 
I think your problem is that you have a long duct.
Your 1mm mesh will have an aspect ratio of ~100, is somewhat coarse but what is more important is to properly resolve the rapid change in volume fraction near the outlet. By the way, is the volume fraction change expected? In simulations of long ducts, I've experienced nonphysical sudden jumps (basically discontinuities) in the solution near outlet boundary conditions. In my case, I knew there could not be any discontinuities and that it was purely a numerical problem. Getting rid of the discontinuities however, took a lot of work. Basically, I reduced the urf's to really low values and very very slowly increased the urf's back to the defaults. Unfortunately, really long ducts take a long time to converge and I spent a lot of time playing with this. One of the things I tried while tinkering was refining and coarsening the mesh in the streamwise direction (which didn't change anything). I always had the sudden jump problem, and always near the exit boundary (but about ~30 cells inside the domain, not directly adjacent to the boundary). I varied the mesh spacing from an aspect ratio of 200 down to 20 with no difference in the final converged solution result. 

April 26, 2016, 11:07 

#5 
New Member
Join Date: Apr 2012
Posts: 17
Rep Power: 9 
Thanks so much for your reply. I really appreciate it.
Yes, I am expecting drastic change in tempreature and vapor volume fraction near the outlet. When the heat flux reaches a critical point, there will be a film of vapor constantly present on the wall surface, which in turn deterioates the performance of heat transfer significantly. I've trield to reduce the timescale factor down to 0.001 (ds = ~1e7 s) and gotten a gradual reduction in residuals. But at some point, there is always a sudden jump in redusiduals and the calculations starts to diverge. I was wondering do you have experience in changing the parameters of AMG solver? Do you think it would be for getting convergence? Again, thanks for you time. I can always learn something from your posts. 

April 26, 2016, 11:10 

#6 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,583
Rep Power: 44 
The AMG settings generally do not help that much with divergence. The settings for the COUPLED solver are a little more aggressive than SIMPLE. Try copying the settings over from SIMPLE.
Even better though is to switch over to SIMPLE/PISO entirely rather than adjusting the AMG. The PV coupling and URF's have a much bigger influence on stability. 

November 27, 2016, 02:39 
simulation boiling water

#7 
New Member
mohamad
Join Date: Oct 2013
Posts: 15
Rep Power: 8 
HI
what is the initial condition? 

September 2, 2017, 02:46 
when can we use the LEE model

#8 
New Member
Join Date: Jun 2017
Posts: 1
Rep Power: 0 
when can we use the LEE model?


November 21, 2017, 00:47 
Horizontal flow boiling

#9 
Member
Ram Kumar Pal
Join Date: Apr 2015
Posts: 38
Rep Power: 6 
Hi Friends, I'm doing horizontal flow boiling simulation in fluent, but not getting converged solution. I'm using eulerian wall boiling model for this problem. Have anyone done this type of problem ? I need your valuable help to solve this problem. If anyone have article related to horizontal flow boiling, kindly share.
I have successfully done this for vertical pipe flow. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Issues on the simulation of highspeed compressible flow within turbomachinery  dowlee  OpenFOAM Running, Solving & CFD  8  October 25, 2016 20:48 
FLuent simulation of taylor couette flow of concentric cylinder geometry.  rshbhb  FLUENT  53  November 5, 2014 20:07 
Hypersonic Flow simulation using Fluent  beanlee999  FLUENT  15  October 14, 2014 01:30 
Fluent Reversed Flow for a cascade simulation  manukamin  FLUENT  9  January 26, 2013 03:29 
Boiling simulation using Fluent  Jake Lee  FLUENT  0  February 10, 2005 03:09 