Can any one please tell me that what can be the cause for having reversed flow...?

I am simulating an anoxic tank...given BC as massflow inlet and outflow...but now getting error as

"reversed flow in 167 faces on outflow 17. turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 420116 cells...."

How can I resolve this issue...? what changes should I go for...?

Thanks in advance....!

---sushii.

Hello, I think that not the reversed flow is your problem but the limited viscosity ratio. If the reversed flow is far away from the area where you want to know the results then forget it. If its not then its better to increase your calculation area. One thing I would do is to change the bc outflow to pressure outlet. Do you calculate steady or unsteady ? If unsteady then try to decrease timestep size. Which one did u use? If steady then try to start with unsteady ( with small timesteps for a while ) and then switch to steady. Your calculating with gas i guess - if you need ideal gas don´t start with it, try to use constant density first and then switch to ideal gas.

A lot of tips i hope that will help you.

Gernot

Hi Gernot,

Thanks a lot for your reply,

I am running the solution in steady state...n with water as a material n not air...! the tank dimensions are very huge...as such "25m(length) X 4.5m(width) X 3m(depth)" while the inlet is at one corner from top is of "0.3m X 0.3m" and outlet is at other corner as a vertical notch..with dimensions "1m X 3m(deep)"...inlet is a mass flow inlet with 0.052kg/s so when thought of pressure outlet it will be so small value of pressure.....I think...!

So what can be the solution...n why the error is there...? for turbulent viscosity limitation...can we do something for it...?

Please reply...!

----- Sushii.

o.k the tank is very big, the velosity is small and the liquid is water ( one phase? )- then you should not have a problem with the turbulent viscosity. Maybe it is your initial conditions. Do you take the standard settings? If it is so then try to initialise again with a small value of velocity in your flow direction ( maybe 0.1m/sec), 0.0001 for turbulence kinetic energy and 0.01 for turbulence dissipation rate. If there is still limitation of turbulence viscosity in the first steps then go on calculating and have a look if the nummber of cells where it is limited comes down.

Hi Gernot,

I have set turbulent intensity as 5 and hydraulic dia as 0.3m should I change these settings...? and go for turbulence KE and dissipition rate...as mentioned in your prior reply...?

One more thing I am doing with model is I hv set three momentum sources inside the domain...which are used to model a submerged mixer in that tank...? so still your suggestion will be same...?

I hv solved for only tank..without momentum sources...then it got converged....!but as I introduced momentum source in it...else all kept same...it gave me such error...?

now what should be done...? please reply...!

Thanks,

---Sushii.

The values i proposed were just for initial conditions. If you have good convergence without momentum sources then forget it. I don´t have ever used momentum sorces. Does fluent abort the calculation or just give the error message and keeps on calculating? If fluent keeps on calculating let it run and have a look at the number of cells if they in- or decrease.

Hi Gernot,

yes your guess is right....Fluent is not at all aborting the calculations...it go on calculating..n no of cells....is not having any confirmed pattern..to increase or decrease...they vary all the time...but sintce frm initial few iteration..it is increasing...for very first itr..128 cells were there...n soon it reached...more than 21000...n it is varying ....! what can be the problem...I'm really confused ...with this stuff...!

I hv tried up to 2000+ itrs...it is Fluent is doing its work...but rev flow error is there...!

You need to think of the physics of the real device. Your tank is drained by a pipe. If that pipe extends into the tank and there are cross flow velocities at the pipe entrance, there will be recirculation there. If that is where you placed your "outlet" then FLUENT will in fact correctly predict inflow. Because there is nothing on the downstream side to slow the flow it can run away.

Try extending your domain to simulate at least a few pipe diameters further downstream. Ten is even better.

This is a classic setup error. You are in good company. - Andy R

Thanks Andy,

I tried with extended domain...n I wonder....It really worked...! Thanks for your suggestion...! still i havent got the expected results...but the error is no more there...with this modified case...!

by the way I cudn't get "This is a classic setup error. You are in good company"...what was that...?

anyway....Once again thanks to all....!

----sushii.

I used to do a lot of user support and training at a CFD company which shall remain nameless. Also built and ran a lot of grids. I myself learned that in rotational flows you need to extend your domain downstream far enough to avoid having a recirculation cross the boundary.

I answered lots of phone calls about "reverse flow" and occasionally saw it in my own problems. Thus you are in good company.

- Andy

Ohh..! that Way...!

Anyway...Thanks a lot Andy....!

If possible then mail me your e-mail ID to sushilkumar.sonar@gmail.com so that we can be in touch...!

Have a nice time...!

Regards, ---Sushii.

Hi,

You can write undermentioned command in fluent console panel.I got it from the www.fluentusers.com.

How can I supress the warning messages about reversed flow at certain boundaries or regarding limits on certain variables such as temperature or turbulent viscosity?

Answer:

These warning messages could indicate potential errors or inconsistencies in your problem definition within FLUENT. In other cases, they may appear only during the early convergence stages of your calculation. If you do want to supress these warning messages, do the following:

To supress the "reversed flow" warning messages, use the text interface command:

/solve/set/flow-warnings? no

or enter the following scheme command within the FLUENT console window:

(rpsetvar 'flow-warnings? #f)

To supress the "limiter" warning messages, use the text interface command:

/solve/set/limiter-warnings? no

or enter the following scheme command within the FLUENT console window:

(rpsetvar 'limiter-warnings? #f)

To re-enable these warning messages, replace "no" with "yes" in the text interface commands above and "#f" with "#t" in the scheme commands above.

Thanks a lot Tejas...!

---sushii..

Thanks a lot sushi....i'll try some solutions tha i've read. Hower i'm working on compressible turbulent swirling flows...so that i must initialitze flow field with k-eps. and only after i can use RSM so that can i change on running the settings?

thanks

valerio

Hi I am working on simulating a 3D rotor, using verified inhouse code, and the problem and the boundary condition are set up very well i guess, but for some reason i dont understand, i couldn't converge, i couldnt get a flow i can say, the inlet flow will keep on falling and the code crushes, it is a a single fan rotor of jet engine with 18 number of blades, about 2M nodes - structure, good mesh quality, i used smith turbulent model, solving in the relative frame of reference with even a CFL of 0.1, do you have any idea ? Thanks,