[fadoobaba]

I am simulating a 2 blade helical vertical axis tidal turbine in SolidWorks Flow Simulation 2018, I have a mesh with ~1,000,000 cells. With this mesh I am getting an answer within 5.5% of the experimental results.

For the said mesh, global mesh is set to 5. I have added 2 mesh controls, one on the blades with advanced refinement option selected with the following settings: 7, 8, 0.25 rad, 6, 0.0025 m. The second mesh control is applied to the rotating region. It has channels option only, settings are: 12, 3, disabled, disabled.

The problem is that when I increase the mesh density, using both mesh controls same and changing global mesh from level 5 to level 6 to level 7. The desired value diverges from the experimental results, from within 5.5% for level 5 to within 10% for level 6 to within 20% for level 7.

What should I do? If I want to publish the results in a conference, I think I will need mesh independence and grid independence along with matching the results with experiments.

Thank you for reading and replying.

About the project (https://3dimensionaldesigningandmanu...axis-wind.html)

[Boris_M]

Hello fadoobaba,

It seems you are using the automatic mesh settings if you change the levels. This is not advised when trying to make mesh convergence studies as there are sub settings behind the automatic settings that change depending on the level you set.
If you chose Lvl 5 you will get different settings for the advanced refinement levels and criteria than with level 6 or 7 and starting with a specific level the adaptive refinement is activated etc.

It is best to specify a manual mesh with either number of cells in X, Y and Z or their cell size and then only increase the level for fluid, solid or interfacing cells. This will also not influence the settings of the local meshes you defined.
If you use automatic settings the basic mesh changes and with that, the specified levels in the other mesh regions will be based on that basic mesh.

In addition, hydrofoils should be meshed very good just like airfoils.

Hope this helps,
Boris

[fadoobaba]

Hello,

Thank you very much for your reply. I came to same conclusion from reading the technical reference file.

I have also found many papers in which authors do not conduct mesh/domain independent studies (example: https://onlinelibrary.wiley.com/doi/abs/10.1002/we.479 and https://arc.aiaa.org/doi/abs/10.2514/6.2017-4626 and https://www.sciencedirect.com/scienc...664?via%3Dihub) etc.. To verify there mesh and computational domains, they compare the CFD results with experimental results. I think I will take this approach, as I already have my results within 5.5% of the experimental results using the settings I mentioned in the original post.

I have also noticed that computational domain and cell count is much smaller for Flow Simulation studies as compared with Fluent or StarCCM+ etc. Can you explain a little why is that? I read the manual and it mentioned immersed boundary method and Cartesian mesh as a the reason for this.

Thank you very much

[Boris_M]

Yes, often mesh convergence studies are still conducted but if experimental results are matched several times for different models you can also assume to some degree that the results won't change anymore with a finer mesh, or at least not significantly which would make the extra solver time worth it.

Purely CFD technically speaking, you should still do it just to confirm but in reality you do that a few times to get confidence and then you trust in your skills as you would not have the time to run 3-5 simulation on every model just to prove the mesh has converged as well.

Yes, that is mostly correct. There is a special approach to the boundary layer treatment which is why there is no need for a specific boundary layer mesh. And in addition the cell count is not the only thing that is playing a role as there are cells that can have multiple control volumes not being counted individually as cells as other tools do since they need to mesh it separately. Those are usually solid-fluid or multiple of such volumes in one cell. The video below explains it nicely I think:
http://go.mentor.com/4QLXV

Regards,
Boris

[fadoobaba]

Thank you very much for your reply. In Flow Simulation, Total cells = Fluid cells + Cells Contacting Solid?

If the person reviewing my paper or a fellow engineer says cell count is low, I will tell him/her about the cells that can have multiple control volumes not being counted individually as cells as other tools do since they need to mesh it separately. Thank you for clarifying this.

Also, I have used similar mesh settings as in original post to validate another wind turbine (NREL Phase VI Wind Turbine here: https://3dimensionaldesigningandmanu...imulation.html). Results are compared with CFX, StarCCM+, OVERTURNS, Fluent, Ellipsys3D In Fig. 1 in the link. Please do check it out.

In the vertical axis wind turbine, I used same mesh settings, and the results are within 5.5% of the experiments by conducted by (https://www.sciencedirect.com/scienc...29801812000194). This is why I am confident and don't want to do mesh/domain independence studies. (Two different times I have validated the mesh for two different devices)

Thank you

[Boris_M]

Almost

Total Cells = Fluid Cells + Cells Contacting Solid + Solid Cells

But since you are not using heat conduction, the solid cells do not count. Just wanted to complete it for anyone else reading the post :-)

The Fluid and Solid Cells are one control volume as they are fully inside the single fluid and solid. The Cells Contacting Solid are the one with multiple control volumes. For example if you have a thin sheet metal separating two fluids such as a water pipe in an air environment and one cell is cutting across both regions with the solid separating them, then you have 3 control volumes. One for each fluid (air and liquid) and the third for the solid in between the two fluids.

Regards,
Boris