CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   How many cells need I have for this model? (http://www.cfd-online.com/Forums/fluent/28787-how-many-cells-need-i-have-model.html)

Jie August 6, 2001 10:58

How many cells need I have for this model?
 
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.

hvn August 6, 2001 11:48

Re: How many cells need I have for this model?
 
You could change the limit of the viscosity ratio in fluent.

Chinor August 6, 2001 17:18

Re: How many cells need I have for this model?
 
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?


Jie August 7, 2001 11:34

Re: How many cells need I have for this model?
 
I have a 2-D 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 pressure-inlet, I set turbulent viscosity ratio to 10.( I use the Spalart -Allmaras viscous model)

What should I do? If I use K-episilon model, commonly how much are the values of Turb. kinetic Energy and Turb. Dissipatioin Rate?

Thanks very much. ---Jie

Jie August 7, 2001 11:38

Re: How many cells need I have for this model?
 
I have a 2-D 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 pressure-inlet, I set turbulent viscosity ratio to 10.( I use the Spalart -Allmaras viscous model)

What should I do? If I use K-episilon model, commonly how much are the values of Turb. kinetic Energy and Turb. Dissipation Rate?

Thanks very much. ---Jie

Christian August 7, 2001 11:40

Re: How many cells need I have for this model?
 
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

Alain August 7, 2001 12:17

Re: How many cells need I have for this model?
 
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 k-eps 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



All times are GMT -4. The time now is 22:24.