Hi,

this is not an easy to setup simulation, also it may look like this on the first glance.

Why?

1) Vortices leading to air entrainment are rather small flow structures of thin diameter and having substantial velocity gradients over the diameter of the vortex. This velocity gradients need to be fairly good resolved in order to resolve the low pressure occuring in the center of the vortex leading to the air entrainement. For that a very fine mesh resolution is required.

2) Usually such vortices - if they are not artificially and by geometric design measures stabilized - are not stationary in space. So the vortex is moving around / precessing and that makes it even harder to establish a well resolved numerical mesh with fine mesh resolution at the vortex center. It might be suitable to use adaptive mesh refinement, but without a coarsening algorithm there is the danger, that the geometrical space more and more fills with refined mesh cells, making the simulation rather very expensive.

3) Standard 2-equation turbulence models are by default not capable of capturing the strong velocity gradients in flows with strong streamline curvature / rotation. A SST k-omega-based turbulence model with curvature correction is at least recommended.

4) It has to be made sure, that the turbulence conditions at the free surface between liquid and air are capturing the physical valid conditions. Usually a fine mesh resolution at the free surface is required for that in addition with turbulence model damping terms at the free surface, i.e. the turbulent kinetic energy at the free surface needs to be dampended to zero or small values.

Regards,

Dr. Th. Frank.

Thomas Frank

Hi,

At first i want to thank you for your generous response Mr.frank.

related to first part of your statements I should mention that my tank's dimensions are 5 meters of length ,2.2 meters of height and 1.6 meters of width and with this dimensions I have chosen the finest cell size for my structured sweep hexahedral mesh as 0.008 meter for tanks mesh and 0.0056 meter for pipe mesh regarding my system RAM and minimizing my aspect ratio. These selections give me about 100000 mesh cells.

Do you think this number is enough for mesh cell size??

or do you think it would be more helpful to choose unstructured tetrahedral mesh??

On the other hand in respect to third part of your statements, I use LES model with WALE sub-grid scale model and i would like to know your opinion about it.

And about the last part of your points mentioned i understood that in general fine mesh is required, i will reconsider the mesh cell size but is there a chance for me to ask how can I check the turbulent kinetic energy??

Amirhossein Taghizadeh : Do you think this number is enough for mesh cell size??

Most likely not. It will depend on the circulation flow velocity in your observed vortex and consequently on the diameter of the vortex. If the vortex measures approx. 8cm in diameter, where the characteristic "dimple" in the free surface can be observed, than this diameter is just resolved with just 10 cells : 10*0,008m =0.08m. 10 cells will for sure not enough to resolve a velocity profile from (minus max. circumferential velocity) --> (zero) --> (max. circumferential velocity). The velocity profile within the core of the vortex needs to be resolved with at least 40 cells, if not even more.

Tetrahedral cells --> results in more cells, with less accuracy and more "gradient smearing" by introduced numerical viscosity. But the hex cells not necessarily need to be equally spaced everywhere.

LES model with WALE should be fine if you can afford everywhere in the domain LES-grade mesh cell sizes and corresponding small time steps. Otherwise I would consider SBES model (stress-blended eddy simulation).

I have extreme doubt, that a Large Eddy Simulation is in any case meaningful on such a large extended domain and with just 100.000 cells in the mesh. The result probably needs to be discarded. If you add to the mesh 2 orders of magnitude, it might become more meaningful, i.e. using 10-30 Mill. mesh elements.

Turbulence kinetic energy: Can be derived from time-averaged flow field information and derived Reynolds stresses as Fluent is providing it from time-averaged solution for LES simulations. The subgrid scale turbulent kinetic energy should be available from the WALE model, but it probably does not contribute much, if the mesh is sufficiently resolved.

Regards,

Dr. Th. Frank.