[nero235]

Hello friends,

I would like to share some experience regarding the problems which may or may not occur when running OpenFOAM multiphase solvers on sHM meshes with activated turbulence models. This isn't necessarily limited to multiphase solvers but can also occur when using single-phase solvers like simpleFoam etc.

Here are some boundary conditions to reproduce the problem

• Mesh has to generated with sHM (version irrelevant)
• Cells at the wall have to be finer compared to the internal cell size (as seen in the left part of the attached image). It doesn't matter however how many cells are in between the layers (nCellsBetweenLevels)
• Activated turbulence: k-epsilon models
• Solver version <= 2.2.2 (haven't tested recent versions)

As seen in the left domain where there are different cell sizes, I assume that the transition between the cells is critical and the cause of the high bounding values of k & epsilon.

As far as the question about numerical schemes goes I can say: it doesn't matter! I tested every scheme combination there is:

• upwind (divSchemes, k & epsilon)
• Gauss linearLimited 1 (divSchemes, k & epsilon)
• cellMDLimited leastSquares 1 (gradSchemes, default)
• limited 0.333 (laplacian & snGradSchemes, default)

I've also tested different k-epsilon models. It may help for some time using limiting schemes and the realizableKE model, but the probability is very high that the solver still crashes because of the bounding values or a ever rising Co which will result in a decreasing time step.

I tested the same case on both meshes as seen below. The result was that the solver always crashed with the left mesh with "bounding" warnings at each time step and the case with the right mesh continued to run, with only one "bounding" warning which was at the beginning of the simulation.

As far as I am concerned, the only solution to the described problem is to use one cell size for the complete domain. I am open to other tips and I hope that this post helps someone.

Regards, Sebastian

[TobM]

Hi Sebastian,

have you checked y+ in the first near wall cell layer? The standard wall functions don't like a y+< 30 to 50. I observed very strange behaviour in the near wall region in cases where the near wall resolution was too high.
Do you use wall functions at all?

Just a few thoughts about your problem, maybe you have already considered these points.

[nero235]

Originally Posted by TobM

Hi Sebastian,

have you checked y+ in the first near wall cell layer? The standard wall functions don't like a y+< 30 to 50. I observed very strange behaviour in the near wall region in cases where the near wall resolution was too high.
Do you use wall functions at all?

Just a few thoughts about your problem, maybe you have already considered these points.

Yes, I have checked the y+ values. Problem is when solving multiphase flow the y+ can't be pin-pointed to one specific value. It ranges in my case from 0.7 to 210.
It's acceptable for the air to use the Low-Re wall treatment, since the kinematic viscosity is high. When considering the fluids (liquid metals & slag in my case) the kinematic viscosity drops dramatically and therefore the y+ is rather high. Since I don't assume the gas velocities to be in the range of the liquids I used wall functions (High-Re wall treatment).

I guess there is no way to stay out of a specific range in my case.