Dear Fluent Users

I am modeling a large tank 3m x .9m x .85 m with an inlet pipe of 70mm dia on top surface and outlet of 50mm dia in the bottom surface. On an average I have meshed the total volume using tet/hybrid -Tgrid meshing scheme. First I had meshed the edges to a size of 30mm approx. The pipes were meshed to Cooper Scheme. Finally I land up with 2,42,000 approx cells.

Now I am using turbulent flow k-epsilon model with inlet as velocity inlet (-0.89m/s, Turbulent Intesity 3.89%, Hydraulic Dia=0.07). Outlet is pressure outlet with (Static Pressure=0, Backflow Turbulent Intensity 3.73%, Hydraulic Dia=0.05). I am modeling the flow of molten steel in the tank. (Density=6997 kg/m3, Viscosity=5.55e-03).

Using Segregated solver, Second Order Upwind for Momentum, K and epsilon, Pressure-Standard, Pressure-Velocity Coupling -SIMPLE, Under relaxation factors-Default).

Here is my problem. After few iterations the solver starts giving the message Turbulent Viscosity limited to Viscosity Ratio of 1.0e+05 in 11-18 cells. This keeps continuing.

Can anyone help me to find out why this keeps happening. Is it because the cells are too large. What might be the correct size. When I ran the same problem with first order upwind scheme. It did not give me the message. But with first order upwind it is taking quite long time to reach the convergence criteria of 1e-06 for all.

Thanks in advance for suggestions. If anyone interested I would be glad to send the journal and case file.

Help me !

Rajeev

(1). You can refine the mesh locally to see how it affects the iteration. (2). And the use of higher-order schemes will definitely slow down the convergence, based on my experience. (3). So, you should study the flow field solution and the mesh distribution to see whether you can improve the mesh in some ways.(if that is causing the problem.)

About the message Turbulent Viscosity limited to Viscosity Ratio of 1.0e+05 in 11-18 cells.

Go to Solve>Controls>Limits

The setting for Turbulent Viscosity limits is 1.0e+05

According to my experience ther ight size for a simulation depend on...what you are simulating. Here is a simple metod to reach a good grade of meshing.

1) start with a mesh not too fine, not to coarse, basically trying to have a n° of cell in each zone so as to be sensitive to the shape and phisical effects of the zone shape.

2) before starting simulation choose a control parameter... ( e.g. mass-flow-rate through an exit or a control surface )

3) start simulation and let it go until you reach good residulas AND the control paramenter curve is flat ( or almost flat )

4) ADAPT THE MESH using region or boundary, or other parameter adaption method

5) start again the simulation and let it go until you reach good residuals AND the good control paramenter behaviour

6) repeat the adaption step and simulation until you have NO CHANGES OF THE CONTROL PARAMETER after an adaption. Thats the correct size of the mesh.

7) additionally you can choose to repeat simulation fron scratch with the same - now adapted - mesh. You should notice no difference in the control parameter value after convergence is reached.

It is really important to choose a good parameter ( I use usually 3-4 control parameters ) . About the viscosity ratio, I too do not know how to modify the mesh in ordert to remove the message.

Hi,

We speak of mesh adaption, but seem to ignore boundary layer adaption (I know, the boundary layer is a mesh too, but it seems we ignore it in these discussions sometimes). In other words, its important to examine a control parameter in the boundary as well as in the mean flow. If you double the mesh size, you may not get a huge overall difference in the control parameter, (say, the torque on a blade), but that does not mean that the boundary layer is o.k., even if the general mesh is. Any comments?

(1). I think, you are right. (2). Now I remember that when I was refining the mesh, it only refine the mesh outside the boundary layer mesh(I hope that this is still the case, because I have not used the code for a while now). (3). Anyway, the unstructured mesh was nice to handle complex geometry, but it is a mess to control it. It is a good idea to create a good mesh right from the begining based on the physics of the solution. (that means you must have some experiences in the problem to be solved) (4). By the way, the mesh in the boundary layer is very important to get the correct viscous effect. Unfortunately, this requirement can be very difficult for most commercial cfd codes. ICEMCFD mesh code can be a good choice, but it is very difficult to use.