turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 511831 cells
Hello,
I want to use eulerian twophase model to simulate a airlift membrane bioreactor, the viscous model is standard kepsilon. The boundary conditions at the gas inlet are set by prescribing a fixed inlet velocity of 0.02m/s and a given gas fraction 1. the boundary conditions at the pressure outlet are set by gas backflow volume fraction is zero. I don't know why in the computation it always remind me that turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 511831 cells. some one say there is something wrong with mesh ,but when I only model water phase use laminar model ,it runs correct and the results are resonnable. There is another question that sometimes I use the dispersed standard kepsilon model, after setting the water phase' turbulence specification ,when I check the case, there is a recommendation "review the turbulence specification at boundary conditions. Default values be detected." I don't know what to do. Can someone help me,thank you ! 
i do also face similar problem. I think that it means, in some of the cells the turbulence is increasing beyond the prescribed value, therefore fluent is limiting the turlence in those cells. u could try with increasing the upper limit of the turbulence and also by adapting the cells where turbulene is higher.

hi,
turbulent viscosity limit occurs when the ratio of turbulent viscosity to dynamic viscosity is upper than the specified limit in fluent. if your case has a complicated flow with high turbulent flow, changing limit of turbulent viscosity limit in solvecontrollimit can help. but you cannot change it a lot. (high turbulent flow usually occurs in very high speed flows around bodies, like supersonic flow around high angle of attack airfoil) but if your case must not have high turbulent flow, check boundary conditions as mentioned in case check. in inlet and outlet you should specify turbulent variables of inlet flow and backflow. if you have an internal flow problem choose intensity=5 and hydrolic diameter of your case and if you have external flow, choose intensity=5 and viscosity ratio=5. then simply initialise domain with inlet and solve. dont forget about lowering underrelaxation of turbulent variables to sth like(0.6,0.6,0.5)in solvecontrolsolution in first timestep/iteration of solution. yours, mohammad 
Thank u for your help,but the problem still confused me.```````````
Thanks for your tips. There's a problem that whether changing limit of turbulent viscosity limit will affect the reliability of results, because someone said that it may only solves the problem of phenomena. And my flow problem is a internal flow,I have specified the turbulent variables for many times,but the same problem confused me. and my geometry is a simplified model, in the beginning I thought it was just a easy case, but now I really feel hopeless. It is very strange, as long as I use eularian twophase model and standard kepsila model,the results will be divergent or the mass cann't be conserverted.
Quote:

Thank u for your tips,i will try
do the adjust will have a influnce on the final results?
Quote:

hi,
if very high turbulent viscosity is the real answer, choosing upper limit is real solution. so just do that. but if not, try good boundary values for turbulence and good initializing and lowering underrelaxations. something I forgot was the mesh quality. poor meshes with high skewness make bad errors in solving turbulent equations. be sure you can solve problems easily. yours, mohammad 
hi,
I improved the mash quality and the problem solved, but there is another problem. after the residual curve became converged, I checked the flux report, the mass didn't conserve. Do you know the reason? 
hi,
let the iteration goes on until the residuals of all equations come down and the slope of their curves become zero. then check the mass conservation if it is out of normal error range, the solution is wrong. check the recommendations of previous post of me. yours, mohammad 
Hello,
I'm trying to do a simulation about boundary layer ingestion by a Sduct. I've done my meshing quite well I'll say (4% of cells are below 0,3 quality) and I've no errors and my coarse model I want to run on Fluent is a 1 million cells model. Then I put my mesh on Fluent and run a 12000 iterations. I chose the kw SST turbulence model where I've calculated the parameters (turbulent dissipation rate....). But after a few iterations (200) I've this posted message "turbulent viscosity ratio limited to 1.10^5 in XXX cells" I've red on the forum to change the turbulence model to the kepsilon RNG. But the kw SST model is very well adapted for boundary layer simulate right? So what other option do I have. For information I should obtain a strong separation of the boundary layer at the duct bend, and even a back flow in the area close to the inner surface of my duct. My Reynolds number is 6,26*10^6 by unit length Thanks for your help 
HI Loic,
You can do 2 things. First reduce your Under Relaxation Factors and run, the "turbulent viscosity ...." should disappear. 200 iterations is too soon, keep monitoring and notice if the no of cells "XXX" cells reduces with iterations Secondly you could run your case with kepsilon for a while untill your solution has approached convergence and then switch to Komega and complete. Regards Luke 
thanks for your advice
Loic 
Quote:
How to distinguish the maximum turbulent viscosity? Until Not so much. tancks 
Also, I have noted that most of the time the issue is with mesh quality. If you can work something to improve the quality, residuals will improve. I had similar issues recently and I used the 'repair' function in Fluent to change the poorquality mesh to polyhedra. After this, convergence improved. I was using the Realizable kepsilon model with scalable wall model.

Quote:
Mesh & geometry are are all about "Parameters Optimization" to make sure parameters fits within Fluent Range else Message. 
All times are GMT 4. The time now is 22:38. 