
[Sponsors] 
turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 511831 cells 

LinkBack  Thread Tools  Display Modes 
September 9, 2011, 08:37 
turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 511831 cells

#1 
New Member
zhangqing
Join Date: Sep 2011
Posts: 5
Rep Power: 7 
Sponsored Links
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 ! 

Sponsored Links 
September 9, 2011, 08:56 

#2 
New Member
Harpreet
Join Date: May 2011
Posts: 21
Rep Power: 8 
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.


September 9, 2011, 09:57 

#3 
Senior Member
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 109
Rep Power: 9 
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 

September 9, 2011, 10:33 
Thank u for your help,but the problem still confused me.```````````

#4  
New Member
zhangqing
Join Date: Sep 2011
Posts: 5
Rep Power: 7 
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:


September 9, 2011, 10:37 
Thank u for your tips,i will try

#5  
New Member
zhangqing
Join Date: Sep 2011
Posts: 5
Rep Power: 7 
do the adjust will have a influnce on the final results?
Quote:


September 9, 2011, 11:13 

#6 
Senior Member
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 109
Rep Power: 9 
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 

September 10, 2011, 10:07 

#7 
New Member
zhangqing
Join Date: Sep 2011
Posts: 5
Rep Power: 7 
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? 

September 11, 2011, 01:29 

#8 
Senior Member
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 109
Rep Power: 9 
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 

May 27, 2012, 08:54 

#9 
New Member
Loic Flouriot
Join Date: May 2012
Location: Cranfield University
Posts: 3
Rep Power: 7 
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 

May 30, 2012, 05:19 

#10 
Senior Member
Join Date: Mar 2009
Location: Indiana, US
Posts: 185
Rep Power: 10 
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 

June 4, 2012, 07:23 

#11 
New Member
Loic Flouriot
Join Date: May 2012
Location: Cranfield University
Posts: 3
Rep Power: 7 
thanks for your advice
Loic 

February 8, 2014, 10:56 

#12  
Senior Member
Aja
Join Date: Nov 2013
Location: Hungary
Posts: 380
Rep Power: 6 
Quote:
How to distinguish the maximum turbulent viscosity? Until Not so much. tancks 

June 10, 2015, 12:10 

#13 
Member
Pranab N Jha
Join Date: Nov 2009
Location: Houston, TX
Posts: 86
Rep Power: 9 
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.


June 11, 2015, 19:11 

#14  
Member
Shane
Join Date: Oct 2009
Posts: 52
Rep Power: 9 
Quote:
Mesh & geometry are are all about "Parameters Optimization" to make sure parameters fits within Fluent Range else Message. 

May 31, 2016, 04:49 
Turbulent Viscosity ratio

#15 
New Member
Sabarish Narayan
Join Date: May 2016
Posts: 5
Rep Power: 3 
Hello,
I am currently working on a transient flow simulation wherein the inlet velocity varies with time and the inlet velocity is zero when the time is zero and then varies according to the flow time. But in the beginning 2 time steps i am getting the warning as turbulent viscosity is limited in so many cells and after the second time step it doesn't appear. My doubt is that how can there be such high turbulent viscosity when the inlet velocity starts from zero. is this an erroneous simulation? If it is how can I correct it? 

June 19, 2016, 03:00 
increase velocity affected by terbulence

#16 
New Member
Somnathde
Join Date: Jun 2016
Posts: 1
Rep Power: 0 
Hello,
I am new user of fluent 14.5. I am working on Premixed combustion and for that using Kepsilon standard model. But if I want to incorporate a velocity at any instant during cold flow reaction(unforced condition) that V=Vinlet_mean +Vturbulence, Vturbulence= 10% of mean velocity. How can i do that? Thanking you all in advance. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
RSM+2nd ordedr causes turbulent viscosity limited to viscosity ratio of....  khsiavash  Main CFD Forum  10  January 7, 2016 13:30 
"turbulent viscosity limited to viscosity ratio"  olivier  FLUENT  11  October 10, 2015 05:49 
reversed flow at pressure inlet and turbulent viscosity is limited....  cfdiscool  FLUENT  10  June 10, 2015 06:15 
pressure eq. "converges" after few time steps  maddalena  OpenFOAM Running, Solving & CFD  69  July 21, 2011 07:42 
setting value of turbulent intensity and turbulent viscosity ratio in wind tunnel  nuimlabib  Main CFD Forum  0  August 4, 2009 00:05 
Sponsored Links 