During iteration it appears this message: turbulent viscosity limited to viscosity ratio of 1e05 in 37 cells. Can someone explain me the meaning of this message and if I have to do something? Furthemore there is reversed flow in the outlet, problably caused by the extension of the domain; it affects the final result? Thank you very much to everyone bye bye

Hi, the message means that the ratio of the turbulent viscosity and the laminar viscosity exceeds 100000. The ratio defines a limitation between the two viscosities that you can change in the limitation panel of fluent. But this is not recommandable. You have to take care that the limitation is not around the examination area of your flow. When it is in the first iteration steps you should wait some further steps and it will disapear by itself. The reversed flow can affect your solution if it is nearby your interessting flow area because you don't resolve the real situation of e.g. a separtion.

Thank you so much Bob; anyway the warning message has disappeared after about 100 iterations and regarding the backflow at outlet it's not near the region of interest so as you said it doesn't affect the solution so much. Thank you

search a bit on this forum, long time ago i wrote a big reply mentioning how to tackle this.

Although the warning has disappeared, you may want to plot your turbulent viscosity ratios at various planes, and verify that they are still not too high.

Thank you Chetan Kadakia for the post but how much is high? I mean what value of turbulent viscosity ratio is considered too high? thank you very much in advance for your response

I use pressure outlet BC for my simulation and "used" to get reversed flow warning in the problem setup. I got around with it by tweaking with back-flow volume fraction. At times it helped me to get rid of..

The second way to have simulation free of reversed flow is to look into aspect ratio. Let it not exceed 5:1. The safety limit is 3:1 in my opinion..however CPU demands are something which user has to bear in the mind.

Last but not the least one can also reduce the URF to enhance stability at the cost of the time. But it helps to boost stability.

As pointed by zxaar he already wrote a lot about tubulent viscosity ration so I will not bother much. However in my opinion the way I got rid of turbulent viscosity ratio errors is by cell aspect ratio. But it is a problem dependent situation.

In few of the cases when you are getting this error one may also look to perform undteady simualtion if he is wroking with steady state solution. KP

It's hard to say... maybe a 1000? I'm not really sure.

You have to plot it and compare. Plus it is problem dependent. Flow in a jet engine versus flow in a pipe will obviously vary.

In the near wall region, you will high molecular viscosity, and therefore not necessarily a high ratio. But perhaps in the wake where you are away from surfaces, and vortex shedding is high, you may have higher turbulent viscosities in that region.

Plot contours of this value just to take a look at it. If your problem is 3D you will need to create a plane or two. You can email me a picture of the contour, if you want my judgement.

[engahmed]

Hi Elizabeth,
I know your simulation was long time ago but I am facing the same problems now, reversed flow ant turbulence viscosity ratio limited to ....
so may I know how did you get rid of your problem, I have tried a lot of the suggestions in the forum here but with no sucess
Thanx in advance

[shivakumar]

Hi all,

I'm getting the same problem, initially it is decreasing for some iterations later increasing. How do I overcome from this??


Thank you.

[hwangpo]

Originally Posted by shivakumar

Hi all,

I'm getting the same problem, initially it is decreasing for some iterations later increasing. How do I overcome from this??


Thank you.

http://www.cfd-online.com/Forums/flu...tml#post122278

http://www.cfd-online.com/Forums/flu...ity-ratio.html

[karthikvv]

Me too getting the same problem

[shivakumar]

HI,

I was getting the same problem as mentioned earlier. That is just a warning and will not affect your final results.. But you need to maintain quality of your mesh. You can disable it by increasing the maximum turbulent viscosity ratio to greater extent.

Solution Controls-->Limits-->Maximum Turb. viscosity Ratio (add two or more zeroes.)..

I hope this helps..

Thanks.

[edoan]

Originally Posted by shivakumar

HI,

I was getting the same problem as mentioned earlier. That is just a warning and will not affect your final results.. But you need to maintain quality of your mesh. You can disable it by increasing the maximum turbulent viscosity ratio to greater extent.

Solution Controls-->Limits-->Maximum Turb. viscosity Ratio (add two or more zeroes.)..

I hope this helps..

Thanks.

Sorry but this is very bad advice. The warning in place because having that high of a viscosity ratio is not physical. This means there is something wrong with the setup, mesh, or boundary conditions etc. Increasing the limit will remove the error message but the unrealisitc, bad solution will still be there. I hope people reading this will have a deeper search into the forums because there are a lot of good tips to resolve common errors that cause this warning. Above hwangpo has linked 2 good threads on this topic which are a great starting place