[ZQWY]

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 !

[Harpreet]

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.

[m2montazari]

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]

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.

Originally Posted by m2montazari

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]

do the adjust will have a influnce on the final results?

Originally Posted by Harpreet

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.

[m2montazari]

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

[ZQWY]

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?

[m2montazari]

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

[loicflouriot]

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

[delaneyluke]

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

[loicflouriot]

thanks for your advice

Loic

[aja1345]

Originally Posted by m2montazari

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

[pranab_jha]

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]

Originally Posted by pranab_jha

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.

[SabarishCEG]

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?

[somu]

Hello,
I am new user of fluent 14.5. I am working on Premixed combustion and for that using K-epsilon 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.

[Oula]

Hi to everyone who still looking for the answer

Check out the link below, it helps me to to resolve the turbulent viscosity ratio limitation

https://www.eureka.im/77.html

[Muneeb]

I am working on simulation of non premixed combustion of a gas turbine engine afterburner in FLUENT. when I run the simulation for ADIABATIC CASE in non premixed combustion (energy eqn 'OFF' , compressibility effects disabled) the solution is easily converged and reasonable results are obtained.

While I enable the compressibility effects in non premixed combustion window followed by recalculating the pdf table, the solution does not proceed beyond 05 iterations with error 'INCORRECT SPECIFIC HEAT VALUE' displaying for almost 100 times followed by divergence in AMG solver. (Note: I am dealing with a fuel; hydrocarbon named JP-8; chemical formula C31H48; molecular weight 420 KJ/kgmol: specific heat value 2200 J/KgK. This hydrocarbon is not available in the FLUENT database (thermodb file) therefore I am defining the fuel empirically by MANUALLY defining these values. I have also tried using various hypothetical low values of specific heat but no success. I tried with using a fuel from FLUENT database but in this case the problem of incorrect specific heat value is not encountered however convergence is still not achieved {maximum pdf table enthalpy exceeded in ------ cells}).

I tried to run the solution with species model OFF (combustion OFF), taking Air as ideal gas (compressible + energy Eqn ON), solution is converged and reasonable results are achieved. Problem is encountered only with enabling the compressibility effects while modeling non premixed combustion.

Further details are as follow:

Mesh size: 6 Million elements (hexahedral + tetrahedral)
steady state
standard k-epsilon turbulence model
radiation: OFF
periodic boundary conditions (axisymmetric 30 deg sector) with mass flow air and fuel inlets and pressure outlet
solver: Coupled (Courant number 0.3)

kindly advice how to proceed with compressibility effects enabled in modeling non premixed combustion in order to avoid the aforesaid errors. please also advice am I correctly defining the empirical fuel. Thanks in anticipation for any advice please.

[yuvarajp]

Originally Posted by ZQWY

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 !

hey, i'm also having the same issue now. did you get to know the issues and how to fix it?