
[Sponsors] 
August 6, 2001, 10:58 
How many cells need I have for this model?

#1 
Guest
Posts: n/a

Hello, Everybody,
I meshed one nozzle model ( inlet radius 3.219 inches, outlet radius 12.4 inches) . How many cells need I have for convergence? In fact, I meshed this model with about 26600 cells. When I ran this model, Fluent said: turbulent viscosity limited to viscocity ratio of 1 e +5 in 19086 cells. How can I avoid this error? Thanks. 

August 6, 2001, 11:48 
Re: How many cells need I have for this model?

#2 
Guest
Posts: n/a

You could change the limit of the viscosity ratio in fluent.


August 6, 2001, 17:18 
Re: How many cells need I have for this model?

#3 
Guest
Posts: n/a

So, Fluent is telling you that you have turbulent viscosities in excess of 100,000 times laminar viscosity, in 70% of your model. So, instead of flowing air or gas, you are effectively flowing some syrup like substance through your device.
Sounds like it could be a poorly posed boundary condition. How did you set your turbulence quantities at your inlets? Is this a 3D model? If it is, you are most likely light on cell count. What kind of nozzle are you trying to simulate? 

August 7, 2001, 11:34 
Re: How many cells need I have for this model?

#4 
Guest
Posts: n/a

I have a 2D model of one parabolic nozzle, which has one inlet radius of 1.61 in, outlet radius of 6.2 in, and throat radius of 1.00 inch. What I need to do is to calculate the flow field when the inlet pressure is 1013250 Pa and the outlet pressure is 101325 Pa. For the wall of the nozzle, I set it to convective heat transfer boundary condition. For the pressureinlet, I set turbulent viscosity ratio to 10.( I use the Spalart Allmaras viscous model)
What should I do? If I use Kepisilon model, commonly how much are the values of Turb. kinetic Energy and Turb. Dissipatioin Rate? Thanks very much. Jie 

August 7, 2001, 11:38 
Re: How many cells need I have for this model?

#5 
Guest
Posts: n/a

I have a 2D model of one parabolic nozzle, which has one inlet radius of 1.61 in, outlet radius of 6.2 in, and throat radius of 1.00 inch. What I need to do is to calculate the flow field when the inlet pressure is 1013250 Pa and the outlet pressure is 101325 Pa. For the wall of the nozzle, I set it to convective heat transfer boundary condition. For the pressureinlet, I set turbulent viscosity ratio to 10.( I use the Spalart Allmaras viscous model)
What should I do? If I use Kepisilon model, commonly how much are the values of Turb. kinetic Energy and Turb. Dissipation Rate? Thanks very much. Jie 

August 7, 2001, 11:40 
Re: How many cells need I have for this model?

#6 
Guest
Posts: n/a

Hi. Have you checked your dimensions ? I had the same problem some time ago and I was busting books to figure out what the problem was (I allso tried here), only to discover that I had a dimension problem: I made the model in "m" instaed of "mm" > 1m became 1000m. Combined with a high turbulence at the inlet and outlet boundary, the ratio went sky high.
Christian 

August 7, 2001, 12:17 
Re: How many cells need I have for this model?

#7 
Guest
Posts: n/a

If you have that message at the begining of your calculation there can be several reasons :
1/ error in model size, you can chech it out in the menu grid/scale in order to see if the true size of your model is that you assume (cf. message of JIE), 2/ bad initialisation value of a keps model. As you use Pressure inlet, the velocity is zero so the default values of k and eps in the initialisation panel will be equal to zero. This give an infinite value for turbulente viscosity 3/ Mesh problem like right handed cells, 4/ bad geometry definition for an axisymetric case. If your geometry is axisymetric and you don't use the right coordinate system (I think that in FLUENT axis must be in the X direction, check out manual) 5/ divergence, underelax you equation or decrease CFL number (depending on the solver you use) you can also get a simpler solution to initialize your flow field (an euler or laminar solution for example) etc... At last, increasing clipping value in order to avoid an error message in generaly a bad idea. Error message are build in the code in order to show that you made a mistake. SA isn't a general model. It was designed for wall bounded flow in aerospace application. Some people use it with some success for turbomachinery application. Personnaly I won't use it for a nozzle. Best regards 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Low Reynolds kepsilon model  YJZ  ANSYS  1  August 20, 2010 13:57 
Highly Skewed Cells  chrisoturner  FLUENT  7  July 22, 2010 06:43 
UDF for Heat Exchanger model  francois louw  FLUENT  2  July 16, 2010 02:21 
species transport model or mixture model?  achaokaoyan  Main CFD Forum  0  July 10, 2010 10:52 
Advanced Turbulence Modeling in Fluent, Realizable kepsilon Model  Jonas Larsson  FLUENT  5  March 13, 2000 04:27 