CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Some questions about flow boiling simulation in Fluent

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 19, 2016, 22:31
Default Some questions about flow boiling simulation in Fluent
  #1
New Member
 
Join Date: Apr 2012
Posts: 17
Rep Power: 9
beastieboys6 is on a distinguished road
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, 1269-1285, 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 k-epsilon model with Enhanced Wall Function
Phase Interactions:
Drag (ishii)
Lift (moraga)
Wall Lubrication (antal-et-al)
Turbulent Dispersion (burns-et-al)
Turbulent Interaction (troshiko-hassan)
Heat Transfer Coefficient (ranz-marshall)
Mass (Enable Correction Model and fix
Surface Tension (enable Surface Tension Force Modeling)
Interfacial Area (ia-symmetric)

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:
Pressure-Velocity Coupling = Coupled
Courant Number = 1~20
Under Relaxation Factor (energy and volume fraction = 0.1~0.3, the others are typically between 0.3-0.5)
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 1e-6 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 5e-5, 7.3e-4 and 3.8e-3). 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 (20-30 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 Wm-2, 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 under-relaxation” 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 1E-2. I really hope there is someone that can give me some advises. Any comment or suggestion would be highly appreciated.
beastieboys6 is offline   Reply With Quote

Old   April 20, 2016, 14:59
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,583
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
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 high-quality? 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.
LuckyTran is offline   Reply With Quote

Old   April 22, 2016, 12:33
Default
  #3
New Member
 
Join Date: Apr 2012
Posts: 17
Rep Power: 9
beastieboys6 is on a distinguished road
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 1e-5, (b) acceptance level of energy and mass balance (energy imbalance: <0.05% and mass imbalance: <1e-7) 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.
beastieboys6 is offline   Reply With Quote

Old   April 22, 2016, 17:45
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,583
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
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 non-physical 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.
LuckyTran is offline   Reply With Quote

Old   April 26, 2016, 11:07
Default
  #5
New Member
 
Join Date: Apr 2012
Posts: 17
Rep Power: 9
beastieboys6 is on a distinguished road
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 = ~1e-7 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.
beastieboys6 is offline   Reply With Quote

Old   April 26, 2016, 11:10
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,583
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
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 P-V coupling and URF's have a much bigger influence on stability.
LuckyTran is offline   Reply With Quote

Old   November 27, 2016, 02:39
Question simulation boiling water
  #7
New Member
 
mohamad
Join Date: Oct 2013
Posts: 15
Rep Power: 8
mohamad.afsari is on a distinguished road
HI
what is the initial condition?
mohamad.afsari is offline   Reply With Quote

Old   September 2, 2017, 02:46
Default when can we use the LEE model
  #8
New Member
 
Join Date: Jun 2017
Posts: 1
Rep Power: 0
Mike.Smart.Kemp is on a distinguished road
when can we use the LEE model?
Mike.Smart.Kemp is offline   Reply With Quote

Old   November 21, 2017, 00:47
Default Horizontal flow boiling
  #9
Member
 
Ram Kumar Pal
Join Date: Apr 2015
Posts: 38
Rep Power: 6
rampal is on a distinguished road
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.
rampal is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Issues on the simulation of high-speed 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


All times are GMT -4. The time now is 21:34.