[tim13]

Hi,
I am doing a simulation of a 3D model of a train under a crosswind effect (or cross-flow). The flow in the model comes from the front and left inlet, and expected to cause a separation behind the body.

The mesh consists of a large box domain with hexahedral mesh and an inner box that contains the train in a tetra mesh and prism mesh.


I started the simulation with a steady first order k-w-SST turbulence model, and then change it to transient second order after about 500 iterations. The time step size is 1e-3, with 30 iterations per time step.



However, I noticed that the value of k is increasing slowly at the first iteration of every time step and eventually causing a floating point error after tens of time steps. This slowly-increasing problem is not happening to other residual components.



boundary conditon are as follows:
front: velocity inlet 44m/s, 1% turb intensity, 0.05 length scale
left: velocity inlet 20m/s, 1% turb intensity, 0.02 length scale
right: pressure outlet, 0 Pa, 1% backflow, 0.02 length scale
back: pressure outlet, 0 Pa, 1% backflow, 0.02 length scale
top: symmetry
bottom: moving wall 44m/s, specified shear=0


Can anybody enlighten me on what I have missed on the settings that caused the divergence of K? or is it something that has to do with the mesh?


I have tried changing the simulation to other turbulence models and even a DDES based on k-w-SST would still show the same problem for a 5.5M mesh and 8.1M mesh.



Thanks,
Tim

[vinerm]

You have good mesh in the region of less importance and bad mesh in the region of high importance. Everything else is good. You don't need to use transient simulation or DDES. You can use steady-state simulation with either or . But first, you have to improve the mesh. The region around train should have high quality mesh. If you cannot put hex mesh around the train, try to generate a very fine tet mesh and then convert it to polyhedral in Fluent.

[tim13]

Hi, thanks for your reply!



Now I know that the mesh around the train have to be improved. But how do you decids that the problem should be okay with steady instead of transient? I have read some paper saying that flows around train are unsteady and vortex shedding may occur.



What are the advantages of converting my mesh to polyhedra in fluent? And in case of polyhedra conversion, would it be okay to just convert the skewed cells or should I go with the whole domain being converted?



Thanks,

Tim.

[vinerm]

Each and every flow is transient, there is nothing called steady-flow. However, a flow may be statistically steady. But whether you run a steady simulation or transient depends primarily on the objective and not on the flow itself. If your objective is to study oscillations due to the vortex shedding or if you have boundary conditions or other parameters varying with time, you need to run a transient case, otherwise, you just need to run a steady-state one. Sometimes, case are run as transient because transient cases are more stable in running but there is no other objective.

Convert whole domain to polyhedral; do note that only the tet and triangular prisms are converted to polyhedral and not the hex cells. It will reduce the number of cells, make the convergence faster, but may make the simulation a little more unstable. However, I don't expect any unstable situations in your case. So, you can easily go ahead with full polyhedral.

[tim13]

Thanks for your suggestion Vinerm.
I have already improved the mesh quality of the important part near the train, and the smaller box. ICEM CFD has shown minimum quality criterion of 0.1 and minimum orthogonal quality of 0.05. Fluent case check has no recommendation as well in terms of mesh quality


I have converted the tetra near the train to polyhedral. Now my cell count is decreased from 8M to around 7M, and it's good considering my hardware limitation during this work-from-home period. However, I am receving problem when running the case now in steady second order k-w-SST. After about 50 iterations I started to see a turbulent viscosity ratio limited. The value is increasing till it reached around 60K cells and never reach higher than 65K cells. Could my mesh still be the issue or should I check my settings again in terms of cross-flow of the train? The boundary conditions are like in my first post above. I have tried changing the outlet gauge pressure up to -100Pa but nothing works so far.



I attached some picture below related to the problem, mesh quality in ICEM CFD, and pressure contours as well. Thanks.


Best,
Tim

[vinerm]

From the residual perspective, convergence is alright. Over prediction of turbulent kinetic energy leading to over prediction of eddy viscosity is normal with EVMs. You can enable Production Limiter under Viscous panel to reduce it. However, if the number of cells with high eddy viscosity reduce to almost nil, then you don't need to worry about those. As far as mesh is concerned, should be used if mesh has of the order of 1. If that is not the case, refine the mesh further closer to the vehicle. Reduction of outlet pressure will not have any effect. It's equivalent to shifting total pressure field down; it does not affect the flow-field.

[tim13]

Thanks for the reply again.
The turbulent viscosity ratio limit problem is rather confusing for me. Especially with the fact that production limit option is already selected by default and still causing around 60.000 cells being limited.
Considering that many of cells from about 7M cells in total, can this problem be neglected? Would there be any significant problem if I increased the limit of turbulent viscosity ratio up to 1 order (or up to 10^6)?

[vinerm]

Setting higher value for turbulence viscosity does not help. Most likely the mesh at the transition from tet region to hex is not good. Or there are sudden changes. Since the flow is not aligned with any particular axis, I'd suggest you to generate a full tetrahedral mesh with smooth transition and then either convert it to polyhedral or run the case with full tet. Large mesh transitions could cause such issues. Furthermore, if you are using first-order scheme for turbulence, then change it to second-order before trying full tet or polyhedral mesh.

[tim13]

Since the flow is not aligned with any particular axis, I'd suggest you to generate a full tetrahedral mesh with smooth transition and then either convert it to polyhedral or run the case with full tet.

Hi vinerm, Why would you suggest to generate full tetra mesh in such case where no flow is aligned to any particular axis? Is there any correlation between hybrid tetra and hexa mesh with fluid flowing straight ahead in terms of solving the equation?
Thanks.

[vinerm]

While using higher order schemes, hex mesh loses its numerical advantage over tetrahedral mesh if flow is not aligned with the mesh. In other words, if flow is not flowing along the mesh lines, then tet and hex will give you almost same results, provided higher order schemes are used. The only advantages hex has over tet is that the number of cells as well as number of iterations required will be lower that those of tet. I suggested it because right now you have high quality mesh outside the core region while low quality mesh in the core region around the vehicle. Better to make it all tet with a slow transition so that quality around the vehicle could be maintained.