hi,

I am solving 3d flow of species in closed domain.I am using standard k-e model for turbulence.It is a unsteady problem. After few time steps it displayed that turbulent viscosity ratio exceed the maximum limit.I have seen that upto few steps the turbulent viscosity ratio is constant.After that turb. Viscosity ratio builds up at each timestep at goes to the maximum limit within 10 time steps. Ofcourse this implies the K and intensity is getting increased.How can I control the turbulence properties. I am using time step of 10^-4 and velocity is 0.003m/s.Inlet K and e are calculaed based on Intensity and Hydraulic Dia.

Thank you .

Balaji

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.

Thank you for your response.

I tried in coupled Solver it's working fine but the residuals are not coming down it is around 10^-1 for continuity and velocities.

The FAS scheme I could find only in coupled explicit solvers.

Thank you

well for some time the continuity residuals will be at the place you have mentioned, or in fact they may increase slightly in the start, but if you observe almost all the other residuals will be coming down. if this is the case you are on correct path, just wait, once other residuals fall below some certain level continuity residuals will also fall, though slowly but they will.

Simple fix - try and run the first 50-100 iterations using the S-A turbulence model then switch to the k-epsilon.

-Riaan

[peter.pan]

Hi,

What effect does very high reynolds number flows have on the turbulence viscosity ratio? Is it safe to increase the upper limit in cases which involve Re in the range of 1000000 to 9000000?

Thanks,
peetak