CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   "turbulent viscosity limited to viscosity ratio" (http://www.cfd-online.com/Forums/fluent/48211-turbulent-viscosity-limited-viscosity-ratio.html)

olivier May 12, 2008 09:44

"turbulent viscosity limited to viscosity ratio"
 
Hi, I do a calculation with species transport. For a calculation for first order all is ok but for second order I have the following sentence after each iteration "turbulent viscosity limited to viscosity ratio of 1e5 in 3(or 4) cells." Where does this problem come from (mesh,under-relaxation factors...)? Thanks for yours answers...

wyzh May 12, 2008 10:23

Re: "turbulent viscosity limited to viscosity rati
 
You can modify the Maximum Tub.Viscosity Ratio in FLUENT: Solve---Controls---Limits

olivier May 13, 2008 05:31

Re: "turbulent viscosity limited to viscosity rati
 
Thank you, but do you think is ok to obtain a turbulent viscosity ratio greater than 10000 ? Actually my calculation don't converge.


kbs May 13, 2008 07:06

Re: "turbulent viscosity limited to viscosity rati
 
hey oliver I have same problem as yours what turbulence model you tried ? is it k-epsilon ?

olivier May 13, 2008 07:48

Re: "turbulent viscosity limited to viscosity rati
 
Yes it's the k-epsilon model.

bohis May 13, 2008 09:28

Re: "turbulent viscosity limited to viscosity rati
 
either bad mesh or k-epsilon is a traitor

wyzh May 13, 2008 11:58

Re: "turbulent viscosity limited to viscosity rati
 
I am a beginner of FLUENT. I think that your calculation is convergent or not has nothing to do with the "turbulent viscosity limited to viscosity ratio" . And the result may be credible ,although "turbulent viscosity limited to viscosity ratio" is displayed during your iteration.

Ant May 14, 2008 02:03

Re: "turbulent viscosity limited to viscosity rati
 
Oliver,

The message you receive is more often due to bad mesh. If you are sure that the mesh quality is good just check if there is any jumps in the mesh size (particularly in regions of high gradients).

One way if to create a point using maximum value of tubulent viscosity ratio (TVR). Then create planes passing through the point and see how the mesh and TVR look like on these planes. The jump in mesh usually happens when you have a multi-block structured mesh.

Regards, Ant


olivier May 14, 2008 04:11

Re: "turbulent viscosity limited to viscosity rati
 
Thank you, I think the problem is probably due to the mesh. But I have this message for a Second Order calculation and not for a First Order. If the mesh is bad, will the message have to appear in every case?

Ant May 14, 2008 09:48

Re: "turbulent viscosity limited to viscosity rati
 
Oliver,

The message need not appear in each case. This could be because the absolute quality of mesh in your simulation could be good (Equiangle Skew), but there could be huge jump in the mesh in critical regions. With second order the error in gradients in these regions would be magnified.

Suggest you plot planes and see where there is jump in mesh. Probably near inlets/outlets. You could have tiny inlet pipe connected to a huge domain. The mesh along the length for the inlet pipe could be fine and could turn out to be coarse immediately into the domain.

Regards, Ant


All times are GMT -4. The time now is 06:57.