
[Sponsors] 
March 17, 2011, 16:53 
Turbulence modeling in CFX

#1 
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6 
Hi,
I am modeling a component which has complex flow physics. Various flow features are present: jet like flow, flow impingement, flow separation and recirculation. I am using CFX and getting convergence has been a big issue for me. I have tried using kepsilon, komega and SST model and I have convergence in a few cases and not in others ( especially in finer meshes). I am going through the turbulence and near wall modeling theory in CFX. As u all would be aware, CFX uses 'scalable wall functions'with kepsilon model and Áutomatic wall treatment'for komega based models. OIs this the same with other major CFD codes like FLUENT? Now I am not sure what approach (i.e which model) should be followed in my case and which approach will work for finer meshes also. I would welcome any suggestions and discussion to solve this problem. Best, Chander 

March 18, 2011, 07:41 

#2  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,045
Rep Power: 86 
Quote:


March 21, 2011, 06:18 

#3 
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6 
@ ghorrocks, thanks for replying
here is the situation: I am modeling water flow (steady state) inside a computational domain where jet flow, impingement on porous media, flow over backward and forward facing steps and recirculation are encountered. I am attaching a picture of my domain which also shows streamlines from one of the converged cases. The green colored part is a porous domain. Now I have tried the following: 1. A uniform mesh in xyz with kepsilon and komega model. kepsilon model converges very easily for this mesh while for komega, shows lack of convergence (i.e the residuals keep oscillating at a level above the convergence criteria which is 1e6). 2. Then I have tried a finer uniform mesh in xyz direction (cell size about half of the first mesh). For this mesh, the kepsilon model fails completely and the simulation gives out a message 'ERROR #004100018 has occurred in subroutine FINMES. Message: Fatal overflow in linear solver.' However, komega model simulation does not fail but shows lack of convergence for higher flow rates. 3. Lastly, I have tried with nonuniform mesh with fine mesh near walls . I tried to keep y+ around 23. For this mesh kepsilon model shows lack of convergence, komega model also shows lack of convergence but the residuals are lower than kepsilon model. I also tried SST model but it there the lack of convergence is most severe i.e. the residuals keep oscillating at level higher than komega and kepsilon. So now, how should I proceed to tackle this issue. I want to get complete convergence for 23 meshes with one model so that I can also analyse grid convergence and proceed with further analysis. Also, are the turbulence models in other codes like fluent similar? 

March 21, 2011, 16:26 

#4 
Member
Pratik Mehta
Join Date: Mar 2009
Posts: 32
Rep Power: 8 
have you calculated the Re number of your system. seems like a low Re problem. Which fluid are you using


March 21, 2011, 16:59 

#5 
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6 
Hello Pratik,
Re number at entrance is in excess of 11000. Yes, from the dimensions of the problem, it initially was not expected that the flow will be turbulent. But it turned out to be so. In fact, this problem cannot be handled with laminar model at all. Fluid is water. 

March 24, 2011, 21:43 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,045
Rep Power: 86 
Sounds like the SST model is the one to use here, unless you have a good reason to do otherwise. But I don't think your convergence problems are due to turbulence models.
Fluent has pretty much the same turbulence models as they are both owned by ANSYS. 

March 25, 2011, 05:33 

#7 
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6 
Glenn,
Thanks for replying to this thread. Yes, CFX manual also recommends SST model. However, it shows the least promise of going towards convergence when I try to use it. As you have seen in my other thread on interfaces, I am thinking if presence of many interfaces in my fluid domain is the cause of loss of numerical stability. I am trying now to minimize these interfaces and combine the meshes in ICEM before importing to CFX. What else I could look at for possible sources of the problem? 

March 27, 2011, 18:14 

#8  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,045
Rep Power: 86 
Quote:


April 1, 2011, 05:40 

#9  
Senior Member
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 6 
Quote:
I have done this but still there is issue with convergence. The residuals just don't reduce below the convergence criteria of 1e6. They still stabilize around 1e5. What else I could do? I also have a backward facing step in outlet pipe geometry and forward facing step in inlet pipe geometry. Could these be the cause ? 

April 9, 2012, 16:36 

#10 
Member
jonathan
Join Date: Jun 2009
Posts: 47
Rep Power: 9 
Hi Chander,
Your residuals of 1e5 are, in my opinion, not bad. Trying to get residuals below 1e6 is tough for any problem. You should not be just focusing on the residuals but rather monitor the quanties of interest that you are trying to obtain from the solution. For instance, if one were performing the classic case of flow about and airfoil, he or she would want to monitor the pressure distribution or lift and drag coefficients resulting from the solution. If these values flatten out even though the residuals are still above 1e6 then one could say that the solution is good enough for what he or she is analyzing. Check out the following section in the CFDOnline FAQ: http://www.cfdonline.com/Wiki/Ansys_FAQ#My_steady_state_solution_converges_for_a _while_but_stops_converging_before_reaching_my_con vergence_criteria 

April 10, 2012, 03:45 

#11 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,990
Blog Entries: 6
Rep Power: 39 
I have recently come across a presentation (internal) where ANSYS CFX was benchmarked for different flow schemes (first order, second order and high resolution) and different convergence criteria. The main conclusions were:
1. High resolution scheme giving identical results as compared to 2nd order 2. 1e03 was loose convergence criteria, but 1e04, 1e05 and 1e06 were giving almost identical trends. It is for sure that 1e05 is very tight convegence and results shouldn't change with lower convergence criteria. Last edited by Far; April 10, 2012 at 04:34. 

April 12, 2012, 04:32 

#12  
New Member
lihui
Join Date: Jun 2010
Posts: 12
Rep Power: 7 
Quote:


Tags 
cfx, turbulence 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Modeling a Fan by the Multiple reference frame (MRF) method in CFX.  saisanthoshm88  CFX  7  February 14, 2011 05:52 
Problems with Turbulence Modeling  ezsoal  OpenFOAM Running, Solving & CFD  4  November 26, 2009 16:12 
turbulence model in CFX, seperated flow  F. Bhuiyan  CFX  3  August 9, 2009 23:28 
May Focus Area: Turbulence Modeling  Jonas Larsson  CFDWiki  0  May 2, 2006 11:48 
Use of 1 equation turbulence model in CFX 4.3  Niels Deen  CFX  0  July 19, 2000 08:50 