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.

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

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?

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

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

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

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