CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

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

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree16Likes
  • 12 Post By m2montazari
  • 1 Post By m2montazari
  • 2 Post By delaneyluke
  • 1 Post By pranab_jha

Reply
 
LinkBack Thread Tools Display Modes
Old   September 9, 2011, 08:37
Unhappy 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: 5
ZQWY is on a distinguished road
Hello,
I want to use eulerian two-phase model to simulate a airlift membrane bioreactor, the viscous model is standard k-epsilon. 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 k-epsilon 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 !
ZQWY is offline   Reply With Quote

Old   September 9, 2011, 08:56
Default
  #2
New Member
 
Harpreet
Join Date: May 2011
Posts: 21
Rep Power: 6
Harpreet is on a distinguished road
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.
Harpreet is offline   Reply With Quote

Old   September 9, 2011, 09:57
Default
  #3
Senior Member
 
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 108
Rep Power: 7
m2montazari is on a distinguished road
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 solve-control-limit 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 under-relaxation of turbulent variables to sth like(0.6,0.6,0.5)in solve-control-solution in first timestep/iteration of solution.
yours,
mohammad
m2montazari is offline   Reply With Quote

Old   September 9, 2011, 10:33
Smile Thank u for your help,but the problem still confused me.```````````
  #4
New Member
 
zhangqing
Join Date: Sep 2011
Posts: 5
Rep Power: 5
ZQWY is on a distinguished road
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 two-phase model and standard k-epsila model,the results will be divergent or the mass cann't be conserverted.

Quote:
Originally Posted by m2montazari View Post
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 solve-control-limit 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 under-relaxation of turbulent variables to sth like(0.6,0.6,0.5)in solve-control-solution in first timestep/iteration of solution.
yours,
mohammad
ZQWY is offline   Reply With Quote

Old   September 9, 2011, 10:37
Smile Thank u for your tips,i will try
  #5
New Member
 
zhangqing
Join Date: Sep 2011
Posts: 5
Rep Power: 5
ZQWY is on a distinguished road
do the adjust will have a influnce on the final results?


Quote:
Originally Posted by Harpreet View Post
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.
ZQWY is offline   Reply With Quote

Old   September 9, 2011, 11:13
Default
  #6
Senior Member
 
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 108
Rep Power: 7
m2montazari is on a distinguished road
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 under-relaxations. 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
i_khaef110 likes this.
m2montazari is offline   Reply With Quote

Old   September 10, 2011, 10:07
Default
  #7
New Member
 
zhangqing
Join Date: Sep 2011
Posts: 5
Rep Power: 5
ZQWY is on a distinguished road
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?
ZQWY is offline   Reply With Quote

Old   September 11, 2011, 01:29
Default
  #8
Senior Member
 
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 108
Rep Power: 7
m2montazari is on a distinguished road
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
m2montazari is offline   Reply With Quote

Old   May 27, 2012, 08:54
Default
  #9
New Member
 
Loic Flouriot
Join Date: May 2012
Location: Cranfield University
Posts: 3
Rep Power: 5
loicflouriot is on a distinguished road
Hello,

I'm trying to do a simulation about boundary layer ingestion by a S-duct.
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 k-w 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 k-epsilon RNG. But the k-w 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
loicflouriot is offline   Reply With Quote

Old   May 30, 2012, 05:19
Default
  #10
Senior Member
 
Join Date: Mar 2009
Location: Indiana, US
Posts: 185
Rep Power: 8
delaneyluke is on a distinguished road
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 k-epsilon for a while untill your solution has approached convergence and then switch to K-omega and complete.

Regards
Luke
pranab_jha and alimoh1987 like this.
delaneyluke is offline   Reply With Quote

Old   June 4, 2012, 07:23
Default
  #11
New Member
 
Loic Flouriot
Join Date: May 2012
Location: Cranfield University
Posts: 3
Rep Power: 5
loicflouriot is on a distinguished road
thanks for your advice

Loic
loicflouriot is offline   Reply With Quote

Old   February 8, 2014, 10:56
Default
  #12
Senior Member
 
Aja
Join Date: Nov 2013
Location: Iran
Posts: 100
Rep Power: 3
aja1345 is on a distinguished road
Quote:
Originally Posted by m2montazari View Post
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 solve-control-limit 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 under-relaxation of turbulent variables to sth like(0.6,0.6,0.5)in solve-control-solution in first timestep/iteration of solution.
yours,
mohammad
Hi
How to distinguish the maximum turbulent viscosity?
Until Not so much.
tancks
aja1345 is offline   Reply With Quote

Old   June 10, 2015, 12:10
Default
  #13
Member
 
pranab_jha's Avatar
 
Pranab N Jha
Join Date: Nov 2009
Location: Houston, TX
Posts: 83
Rep Power: 7
pranab_jha is on a distinguished road
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 poor-quality mesh to polyhedra. After this, convergence improved. I was using the Realizable k-epsilon model with scalable wall model.
sircorp likes this.
pranab_jha is offline   Reply With Quote

Old   June 11, 2015, 19:11
Default
  #14
Member
 
Shane
Join Date: Oct 2009
Posts: 52
Rep Power: 7
sircorp is on a distinguished road
Quote:
Originally Posted by pranab_jha View Post
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 poor-quality mesh to polyhedra. After this, convergence improved. I was using the Realizable k-epsilon model with scalable wall model.
Thanks Pranab.

Mesh & geometry are are all about "Parameters Optimization" to make sure parameters fits within Fluent Range else Message.
sircorp is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
reversed flow at pressure inlet and turbulent viscosity is limited.... cfdiscool FLUENT 10 June 10, 2015 06:15
RSM+2nd ordedr causes turbulent viscosity limited to viscosity ratio of.... khsiavash Main CFD Forum 7 October 19, 2011 06:21
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
"turbulent viscosity limited to viscosity ratio" olivier FLUENT 9 May 14, 2008 09:48


All times are GMT -4. The time now is 18:31.