CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Turbulence modeling in CFX (http://www.cfd-online.com/Forums/cfx/86254-turbulence-modeling-cfx.html)

Chander March 17, 2011 16:53

Turbulence modeling in CFX
 
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 k-epsilon, k-omega 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 k-epsilon model and ┴utomatic wall treatment'for k-omega 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

ghorrocks March 18, 2011 07:41

Quote:

which model should be followed in my case
Well given that you have not described what you are doing that is not possible. A bit more explanation would help.

Chander March 21, 2011 06:18

1 Attachment(s)
@ 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 x-y-z with k-epsilon and komega model. k-epsilon 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 1e-6).

2. Then I have tried a finer uniform mesh in x-y-z direction (cell size about half of the first mesh). For this mesh, the k-epsilon 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 non-uniform mesh with fine mesh near walls . I tried to keep y+ around 2-3. For this mesh k-epsilon model shows lack of convergence, komega model also shows lack of convergence but the residuals are lower than k-epsilon 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 k-epsilon.

So now, how should I proceed to tackle this issue. I want to get complete convergence for 2-3 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?

pratikmehta March 21, 2011 16:26

have you calculated the Re number of your system. seems like a low Re problem. Which fluid are you using

Chander March 21, 2011 16:59

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.

ghorrocks March 24, 2011 21:43

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.

Chander March 25, 2011 05:33

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?

ghorrocks March 27, 2011 18:14

Quote:

I am thinking if presence of many interfaces in my fluid domain is the cause of loss of numerical stability.
Unlikely. Try to make the mesh size similar on both sides of the interface. That is about the only thing to watch for with interfaces.

Chander April 1, 2011 05:40

Quote:

Originally Posted by ghorrocks (Post 301171)
Unlikely. Try to make the mesh size similar on both sides of the interface. That is about the only thing to watch for with interfaces.

Glenn,
I have done this but still there is issue with convergence. The residuals just don't reduce below the convergence criteria of 1e-6. They still stabilize around 1e-5.
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 ?

jonny_b April 9, 2012 16:36

Hi Chander,

Your residuals of 1e-5 are, in my opinion, not bad. Trying to get residuals below 1e-6 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 1e-6 then one could say that the solution is good enough for what he or she is analyzing.

Check out the following section in the CFD-Online FAQ:

http://www.cfd-online.com/Wiki/Ansys_FAQ#My_steady_state_solution_converges_for_a _while_but_stops_converging_before_reaching_my_con vergence_criteria

Far April 10, 2012 03:45

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. 1e-03 was loose convergence criteria, but 1e-04, 1e-05 and 1e-06 were giving almost identical trends. It is for sure that 1e-05 is very tight convegence and results shouldn't change with lower convergence criteria.

lihui54312 April 12, 2012 04:32

Quote:

Originally Posted by Chander (Post 301018)
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?

I also think that the problem is not the change of turbulence model,yo can check the mesh(number and prism),and how to set other boundary.


All times are GMT -4. The time now is 20:25.