Hi everybody !

I'm facing a small problem in Fluent. Whent I iterate using Spalart Allmaras viscosity model, at a certain point, I get an error message : turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 29830 cells.

Does anybody knows how to interpret that, and eventually how to fix it ?

http://www.cfd-online.com/Forum/flue...cgi?read=29389

Thanks !!

In the message you told me about, zxaar speak about the FAS... What is it ? I'm working with spalart allmeras. How can I do, if I can't change k, or epsilon ?

If you are using the coupled explicit solver, you can use the FAS multigrid method (grid coarsening). It is clearly written how to use this method, in the FLUENT manual.

If you are using the coupled implicit solver, then I recommend you to follow this method, which usually I do for steady problems (..thanks to Zxaar!).

1. If it is a 2-D model, start with a very coarse mesh,say, 5000, and if it is 3-D, start with, say, around 12,000

2. Run it for long (40,000 to 50,000 iterations , with low CFL, URFs)...it won't take much time(depends on your system) as the number of meshes are very less. Initially residuals may behave badly...just don't care! go ahead

3. If it shows divergence, or the TVR warning for long time, you can try reducing CFL and/or URFs and continue...if it still shows divergence/TVR warning, you can adapt the grids in the high TVR areas either with region or isovalue adaption. After adaption, you may see the no. of cells with TVR warning has been increased, but it will decrease soon. Still it doesn't solve your problem, you'd better re-mesh your geometry and try steps 1,2,3

4. If it shows convergence after 40,000 or 50,000 iterations, you can increase the CFL and /or URFs to accelerate the convergence.

There are no hard and fast rules to get the convergence and the expected values. You should play around with all the possible options.

regards

Rajesh

I'm using the coupled explicit solver... You said "FAS method"... What are theses letters for? (I didn't find "FAS" in the manual...)

Could you just tell me what are "low CFL", "URFs", "CFL", "TVR"... ? I didn't find them in the manual too...

Many thanks !!

Cyril

FAS is Full Approximation Storage. It is given as FAS itself in the fluent manual. (FLUENT 6.2)

CFL number is Courand-Friedrichs-Lewy number, called commonly as Courand number.

URF- Under Relaxation Factors.

TVR warning-the warning for high Turbulent Viscosity Ratio

Low CFL -: 0.1-0.5, you can try still smaller ones. When CFL No is small, your numerical calculations are more stable but the convergence rate will be slow. Low URFs -: you can start with 0.1 or smaller for all URFs

CFL No.(Courand No.), URFs are in SOLVE->CONTROLS->SOLUTION Panel.

Sorry for giving the abbreviations!

regards

Rajesh