CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Internal flow simulation (

Kishore June 4, 2007 06:55

Internal flow simulation
i'm simulating internal flow through a duct which delivers it to a chamber where the flow splits into two and exits. when i'm running 3-d segregated implicit solver with spallart-allmaras model, the residuals of x,y,z velocity keep oscillating and never converge.. when i removed the chamber and simulated it only for duct, it converges... what can be the possible problem? either grid or boundary conditions? while it is solving , it says "reverse flow in __ faces" and "turbulent viscosity exceeds the limiting value"... what could be the possible cause of this..

your help in fixing this problem will be appreciated.. if u need further info regarding boundary conditions i can give..

AJ June 4, 2007 15:35

Re: Internal flow simulation
Try with refined mesh... you might get better results.... Can you try first with laminar flow only and then use turbulence... this could also enhance convergence...

Is the flow turbulent???

There could be lot of mixing happening in the box/chamber which causes the fluctuations....

How far are the ducts from the chamber? That could also affect convergence...


Kishore June 4, 2007 23:08

Re: Internal flow simulation
dear AJ , thanks for replying.. the flow is turbulent.....i tried refining the mesh using structured grid as much as possible but still there are flucuations.. as you said there is a lot of mixing happening in the chamber.. may be that leads to fluctuations. the duct is a L-shaped one and is connected to the chamber by a cube like volume at the end of the duct...

yesterday i tried running simulation without the chamber ,only with duct and that cube.. lot of reverse flow was occuring at the exit of that cube...

now my question is ,if there are fluctuations due to mixing, wont there be convergence? when should i stop iterating and plot results?

Prasad Dudhgaonkar June 5, 2007 05:17

Re: Internal flow simulation
Hi Kishore, Spalart-Allmaras model is considered to be unsuitable when the flow changes abruptly from a wall-bounded to a free shear flow. [Fluent 6.2 Help (11.2.4)] Probably your problem involves such behavior. This is supported by your experience of getting converged solution for a plain duct flow. So I suggest that changing turbulence model might help you get solution, probably a more accurate solution. Try RNG or realizable k-e. You will get rid of the warnings when you will get a converged solution.

Kishore June 5, 2007 05:36

Re: Internal flow simulation
hi prasad, thanks for ur valuable suggestion... will try that and will post my response on what happened.. but one thing, the flow is wall bound through out... i just truncated the duct and made that location as exit ur help in this wil be required and will surely be appreciated... thanks

Carlos June 5, 2007 18:57

Re: Internal flow simulation
Hi Kishore,

Its true that the Spalart Allmaras model is unlikely to give you a converged solution because it is the wrong type of model and it is in fact designed for external flows. As Prasad said the RNG k-e would work better and the k-omega model is good for internal flows if the Reynolds number is small enough. However, if your residuals are not converging then I would look at two things first:

1) Check the equiangle skewness of your grid, if the worst element is greater than 0.85 this could cause the oscillations. Make sure the grid is refined closer to areas where the flow variables change suddenly. The solver is much more likely to give you convergence if the difference in flow variables changes by a small amount from cell to cell. If at all possible use structured cells because they have smaller skew values.

2) Once you are sure the grid is adequate then it is best to use a solution strategy. I assume you want a second order solution to your problem - this is more accurate than a 1st order one. However, second order solutions are inherently more unstable than first order solutions so I use the following strategy. I usually turn OFF the residual monitors and run a 1st order standard k-e model for a few thousand iterations. This is the best way to get ultra small residuals because the sk-e model converges the most easily of all turbulence models. Once you have a solution, feed that into a 2nd order standard k-e model and again let it run for a few thousand iterations. The solution will be converged when the residuals have levelled off and they are flat. Next, use this solution and feed it to your final turbulence model, that could be RNG k-e or whatever you wish. Then you can either let is run until the residuals have levelled off, or you could turn the residual monitors on again. However, BEWARE! A convergence level of 10^-3 is quite large and it is highly unlikely to give a truly converged solution. 10^-4 will give a practically converged solution and this should be adequate for most purposes. However, as mentioned above, a converged solution by its very nature means that it will not change with further iterations and so if the residuals are flat (and low enough) then you have your solution.

Hope this helps and good luck!


Kishore June 5, 2007 23:24

Re: Internal flow simulation
hi carlos, thanks for your detailed and timely reply. as you said, i examined the equiangle skewness in my grid. the worst element was well below .85. i tried RNG model as prasad said. it cleared me two problems.. one, the turbulent viscosity which was exceeding its limits in my previous attempts didnt exceed this time... i didnt get reversed flow also... thanks to prasad. the problem which i still face is my residuals are still oscillating between 10^-2 and 10^-3 even after 5000 iterations.. now i'm running another 5000 iterations to see if it will converge. i will surely try ur strategy of running 1st order k-e , then second order k-e and then RNG... kindly help me to sort this out.. thanks, regards, kishore

Carlos June 6, 2007 12:11

Re: Internal flow simulation
Another way to achieve convergence is by relaxing the solution. If you try the methods above and they still don't work then you can reduce the under relaxation factors in the solution controls panel. I usually reduce pressure from 0.3 to 0.2 and momentum from 0.7 to 0.4. This usually dials out oscillations and aids convergence. Sometimes it is necessary to reduce the relaxion factors for k and epsilon from 0.8 to 0.5 if the above doesn't work.

This tactic is usually very effective but you must try the previously mentioned solution strategies first (recommended by Fluent). However, keep in mind that if you relax a solution, it takes longer to converge than a solution with the default under relaxation factors. Therefore it is wise to allow the solution to run for 5000 iterations until the residuals level off, with the convergence monitors turned off. In some cases you may see the residuals level off after say 2500 iterations and the residual levels are low enough (10^5 or less) to say that you have your solution.

Good luck,


Carlos June 6, 2007 12:17

Re: Internal flow simulation
Oh and one more thing to check. Did you scale the grid properly? If you created your CAD and mesh model in say millimeter's then you MUST scale the grid once you read it into Fluent. The default units are metres in Fluent because it uses SI units. However, the standard unit in engineering is mm's for accuracy purposes. Therefore use the grid->scale panel to scale your grid.

I just remembered helping a student once who couldn't get convergence because he didn't scale his grid. Its worth checking out because it makes a huge difference!



All times are GMT -4. The time now is 07:40.