Hi everybody.

I use the Fluent to simulate an external flow. But after some Iterations, it appears the warning "turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 135 cells"

So, somebody could suggest to me what is the problem and how to solve it.

Thannks a lot! Skylife

There are lots of things that could cause this. The two most common reasons are that it's a meshing problem, or that it's not a big deal. If it's early in your solution, and the number of cells decreases to zero, then you probably don't have a problem.

If it doesn't seem to be dropping, then its probably a meshing problem and you need to go into your model and find where the problem is. Do Plot->Contours, choose the default-interior, or whatever you've called your volume, turn off node values, and turn off auto range. Plot a range of about 1e3 to 1e5, and make sure clip to range is on. Also, make sure plot grid is on, so you know where in the model you're looking at. You can play around with the lower end of the range to nail down exactly where the problem is. Once you know where the problem is, you probably need to re-evaluate your mesh in this region (typically you want a finer mesh in this area if this is the problem).

There are other things involved with this error, but those are the two most common. There has been a lot of discussion on this error in the past, and if what I said above doesn't help, then I recommend searching the forum. There's a lot of good information in there, and I couldn't possibly re-type it all, or even remember it all.

Hope this helps, and good luck, Jason

Thanks Jason so much! I am searching for error location in calculation domain. And I will try to find information in forum. I hope I can avoid this problem and share experience.

Thanks once more!

Skylife

once i posted a big message on this issue, i am pasting that message again, you can read this:

{

well this is one common problem lot of people have asked about it before. i will try to summarize the approach i take to solve this problem.

first of all, the very basic cause of this warning is the wrong set up of boundary conditions. So if you are sure that nothing is wrong with the set up of the problem, you can follow the following things.

The origin of the problem lies in the fact that if the solver calculates the value of k and e or omega (in two equation models) wrongly, its very likely it will calculate turbulent viscosity wrongly and thus we get the warning. In the ideal condition, as the solution converges the warning should go away and we all live happily ever after. But generally this does not have so happy ending. The reason is mainly we have a case which is very large and convergence is already difficult and which is exacerbated by the wrong calculations of turbulent quantities. So what are the remedies for it.

The usual remedy is to switch to coupled solver, and work with it, and this usually solves the problem. But my personal thinking is that if the case is incompressible the coupled solver may not work well there. But yes this is one solution. The second solution which is far more stable is, and if you fail to get the solution from coupled solver too, switch to FAS, increase the number of pre post iterations, make the coarsening levels to 4, (4 is more than enough). And this converges almost every problem, but there are case where you might fail to get convergence.

Anyway if you are stuck with segregated solver (like me), what are the options.

First of all if we consider that the divergence is because of turbulence quantities, we may want to force the convergence on these quantities before we move to next iteration.

The way I do is this, I change the multigrid options for k, e to V cycle, make the pres sweeps to 1 post sweeps to 2, and chose Bicgstab as smoother. And let it run.

Sometimes I just want to first get the best approaximation of k,e for the flow field I have, for this I usually switch off the solver for momentum equations and just solve for k,e or k, omega till I get warning free turbulent field, then I switch on all the equations and go on to iterate further.

This approach works well, but it has one problem. if the mesh size is very large say around 3 million cells then even to first get the turbulent quantities to converge might take day or two. So what to do in this case.

Whenever I have to do calculations for the cases around 2-3 million cells, I make two meshes one very very coarse, with same boundary conditions as finer mesh (which is of course around 3 million cells). Now first I get converged solution on coarse mesh, which I can get in hour or two. Then go to file->interpolate, and write the data for corresponding zones, and then when you read the fine mesh read this initial guess from same file->interpolate->read.

And here switch off the momentum calculations do some calculations only for turbulent quantites, (if u get viscocity warning, it will soon go away, though I never got warning here since the solution is already converged), so after say 3-4 calculations switch on solver for all the quantities and go on to iterate, you will get converged solution.

(well on coarse grid you can use FAS to force convergence, its quite handy there).

Hope this will be useful.

}

Possibly valuable insight zxaar. However, I am just curious. How does one know that these are the general troubleshooting practices. I mean, did you get these guidelines from some references or is it your own finding?

No i nevr read these things anywhere, but since i have been doing lot of turbulent anaylsis, i have to use almost every model and almost every possible kind of mesh. once i had to do a k-omega model with around 3 million cells and this ratio warning was given by solver and the number of cell for which there was warning was going down but it never gone completely, then i had to think ways to get the solution for that mesh, (i always have this thinking that if you do not get convergence easily then just force the convergence), so i try to find the ways to get converged solution for it. so all that i wrote is my experience, i think others can learn from it.

how generate grid in turbulent flow over an obstacle for good results. please suggest me for the same. thanking you baheti

how generate grid in turbulent flow over an obstacle for good results. please suggest me for the same. thanking you baheti

hello

How i can calculate free - stream velocity at a

turbulenc flow?

thankyou

[rnisson]

If the solution is converging with residuals at 1*10^-4, does this really matter?