
[Sponsors] 
April 14, 2021, 03:13 
Imbalances during wall boiling simulation

#1 
New Member
Thomas
Join Date: Mar 2018
Location: Germany
Posts: 18
Rep Power: 6 
Hello everyone,
I am simulating subcooled wall boiling of water (steady state) using the RPI model within a pipe (axisymmetric and equidistant mesh dx=dy=2mm with 5 degree rotation and symmetry boundary conditions). As a basis I used the wall boiling tutorial supplied in the ANSYS Learning Hub. I exchanged the domain from the Tutorial using a pipe with slightly adjusted dimensions (increased diameter, decreased length), increased the inlet velocity and increased the Liquid.Temperature as the constant heat flux at the outer walls was not enough for the liquid to reach saturation temperature, and thus no evaporation occured. While I was now able to reach the saturation temperature and water to evaporate into the vapour phase, I have difficulties reaching Imbalances below 1%. For Energy I get an Imbalance of 1.5% and Mass Imbalance for the liquid at 4.5% and they are not decreasing anymore with further timesteps. All my equations (momentum, mass, heat transfer and turbulence (KE)) reached the conservation target below RMS=1E06. I had a look at this ANSYS FAQ in this forum but I am not sure how could I decrease those imbalances or if they even are relevant. While I understand that my global imbalances show me the difference between "what goes in, goes out" I question if I need to reach the Imbalance below 1% for those two sizes. I mean at my Inlet I have the liquid.vf defined as almost 1 (1vapour.vf with vapour.vf defined as 1e7 as a nucleation starter for the rpi model) and at my outlet i expect more of the vapour phase due to evaporation. Shouldn't the Imbalance be expected for the mass of the liquid, as some of it is evaporated? If not, how may I be able to reduce it further? And what about my energy imbalance? Thanks in advance! 

April 14, 2021, 15:53 

#2 
Senior Member
Join Date: Jun 2009
Posts: 1,575
Rep Power: 28 
Not sure I understood your question completely; however, the imbalance of any of the equations should always approach 0 for a converged solution.
If one fluid changes phase from liquid > gas, it should be accounted for in the imbalance as a mass sink.. The mass must be accounted for at all times.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

April 15, 2021, 03:08 

#3 
New Member
Thomas
Join Date: Mar 2018
Location: Germany
Posts: 18
Rep Power: 6 
Dear opaque,
thanks for your answer. I checked my results now with the imbalance and can confirm the imbalances. While at my Inlet i have the following: massFlow()@inlet 0.105802 [kg s^1] and at the outlet: massFlow()@out 0.110642 [kg s^1] So its a rather large difference in mass flows. After 2000 iterations my Imbalances resolve to: ++  MassLiquid  ++ Boundary Sources : heatedwall 1.4360E04 Boundary : inlet 1.0580E01 Boundary : out 1.1064E01 Domain Src (Pos) : Default Domain 2.0982E09  Domain Imbalance : 4.9833E03 ++  HEnergyLiquid  ++ Boundary : heatedwall 4.4416E+02 Boundary Sources : heatedwall 6.7892E01 Boundary : inlet 1.5623E+03 Boundary : out 1.1410E+03 Domain Src (Pos) : Default Domain 3.4780E03  Domain Imbalance : 2.3556E+01 ++  Normalised Imbalance Summary  ++  Equation  Maximum Flow  Imbalance (%)  ++  UMomVapour  1.2025E+02  0.0000   VMomVapour  1.2025E+02  0.0000   WMomVapour  1.2025E+02  0.0010   UMomLiquid  1.2025E+02  0.0000   VMomLiquid  1.2025E+02  0.0000   WMomLiquid  1.2025E+02  0.0359   MassVapour  1.1064E01  0.1297   MassLiquid  1.1064E01  4.5040  ++++ ++++  HEnergyLiquid  1.5623E+03  1.5078  ++++ Running it longer doesn't resolve the issue as the imbalances are constant from 400 iterations onwards. I added my setup in the attachement. Where do you think the problem arose from? Kind regards! 

April 15, 2021, 05:06 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
You say you have read the FAQ, but the FAQ really is the starting point for this problem. Can you describe what happens when you do the suggestions on the FAQ?
FAQ: https://www.cfdonline.com/Wiki/Ansy...gence_criteria
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

April 15, 2021, 14:58 

#5 
New Member
Thomas
Join Date: Mar 2018
Location: Germany
Posts: 18
Rep Power: 6 
Dear ghorrocks,
I found the solution to my problem in a wrongly defined inlet velocity. It was calculated based on a volume flux divided by the Area of the inlet, instead of the area of the real pipe inlet. Thus my velocity was several magnitudes higher than it should really be. However this was what I checked from the FAQ before I found the error, maybe you may asses my reasoning there: 1. Suggestion reading the CFX Modelling guide Chapter 15 (now 16) for convergence problems. I dont have a startup probelm so I try the suggestions from later problems: 1.1.My MAX Resiudals are the following in the last timestep: ================================================== ==================== OUTER LOOP ITERATION = 1000 CPU SECONDS = 5.320E+02   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMomVapour  1.00  9.1E13  4.1E11  7.4E03 OK  VMomVapour  1.00  5.0E14  3.0E12  1.3E02 ok  WMomVapour  0.32  1.5E12  7.7E11  1.7E02 ok  UMomLiquid  1.00  1.2E08  3.8E07  1.5E02 ok  VMomLiquid  1.00  7.2E10  3.2E08  2.2E02 ok  WMomLiquid  1.00  2.2E07  9.1E06  1.1E03 OK  MassVapour  1.00  2.8E06  9.8E06  9.1E05 OK  MassLiquid  1.00  9.6E10  3.3E09  7.6 9.2E05 OK ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 11.1% of the faces, 18.5% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: outlet.   The fluid name is: Vapour.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++ ++++++  HEnergyLiquid  1.00  1.6E08  8.3E07  5.7 8.3E05 OK ++++++  KTurbKELiquid  1.00  2.9E08  1.1E06  5.7 9.2E05 OK  EDiss.KLiquid  1.00  3.5E09  1.6E07  7.1 1.3E05 OK ++++++ As the Momentum equations as well as the turbulence models MAX residuals are several magnitudes larger than the RMS Residuals, its possible to be a local problem. However those equations converge rather quickly. For the mass and energy equation the MAX residuals are probably global convergence problems. So according to table 16.2 in the ANSYS SolverModelling Guide I have to check: a) Large Timescale Effect, Most equations are solved with 0.0005 s The continuity equation is solved on a small timescale 1e10[s]. I start out with a larger one (1e7) for the first 200 or so iterations and then decrease to this value. This reduces the RMS residual of mass vapour to go under my convergence criteria. However no change for the Imbalances is observed. b) Turbulence Levels MAT visc gas = 1.86E5 [kg m^1 s^1] MAT visc liq = 1.07E4 [kg m^1 s^1] min max  Vapour.Eddy Viscosity  1.30E06  7.98E03   Liquid.Eddy Viscosity  4.51E05  2.77E01  INLET Reynolds = 368714 ==> turbulent. The max eddy vsicosity is as suggested by the modelling guide magnitude 1000 larger than the dynamic viscosity. c) Turbulence model selection I used the ke turbulence modell. While the turbulence models are rather well converged I think it is sufficient for this case and the given mesh. d) Advection Scheme I used high resolution for all my equations. I changed the Advection Schemes for Energy and Continuity both to specified blend factor of 0.75 (Run WB_ImbStudy002) > overall convergence of equations is worsening, also the Imbalance is much larger within 1000 iterations. At the beginning the Residuals of my w component of the momentum becomes "bouncy". (WB_ImbStudy003) Blend Factor 0.9: Initial Bouncy behavior of residuals w component in the momentum. (WB_ImbStudy00) Blend Factor 0.9 just for continuity: Intital Bouncy behavior of residuals w component in the momentum. 2. Checking if my solution is sufficiently converged: It is not. Thats why I wrote the question here. 3. Find the reason for bad convergence. > Checked the physics again and found the error of the inlet velocity, 

April 15, 2021, 15:11 

#6 
Senior Member
Join Date: Jun 2009
Posts: 1,575
Rep Power: 28 
Since you mention mixing advection schemes, my advice is NOT to that. You are looking for problems by doing so.
Pick the one you think is the best (based on your experience/testing/etc), and use it for all the equations. Advection transport is shared by all the equations, why would I approximate it differently for different variables? Food for thought..
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Tags 
evaporation, imbalances, rpi model 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[Commercial meshers] Fluent3DMeshToFoam  simvun  OpenFOAM Meshing & Mesh Conversion  50  January 19, 2020 15:33 
Centrifugal fan  j0hnny  CFX  13  October 1, 2019 13:55 
How to make UDFs for Nucleate Pool Boiling Simulation?  SIKJAE  Fluent UDF and Scheme Programming  1  August 4, 2018 07:07 
Multiphase wall boiling model  omaralyahia  CFX  4  July 14, 2015 21:41 
Coupling RPI wall boiling model with population balance model in Fluent  softice2006  Fluent Multiphase  0  February 1, 2015 15:55 