Lift Analysis on a Wing Sail

I want to analyse the lift and drag for a wing sail. Therefore I have created this project:

Somehow I do not get valid results. There seems to be a mistake in the simulation setup, but I can not find it.

HI this is Fillia from SimScale Support.

Your boundary conditions and general set up look alright, so personally I would focus on the mesh and domain.

Try using this tutorial as reference: Tutorial: Compressible CFD Simulation of a Golf Ball | SimScale

Of course this is compressible analysis, but you can get good information about the Enclosure’s size ( Figure 4 ), how to apply Symmetry, and how use the Standard algorithm for mesh generation.

Try to recreate the mesh refinements of the tutorial as well, and make sure you monitor the y+ values:

After each mesh is generated, you can check the quality using this guide: How to Check and Improve Mesh Quality | SimScale

Best regards,
Fillia

To me it looks like something is wrong with the air flow. Because I started with an inlet velocity of 8 m/s and it seems to be some areas in the simulation where the flow reaches 300 or more m/s. I also do not understand why the flow is going upwards slightly.

Exactly, these high values can be created by bad elements inside the mesh, as the boundary conditions do not seem to be unrealistic. There is a method described here with which you can isolate the cells with high values (through isovolumes), so you can find out what areas are problematic: How to Check and Improve Mesh Quality | SimScale
Check section 2.2

Best regards,
Fillia

I will check on that. By the way, is it normal that the flow is going upwards and not in a straight line ?

You should expect a behavior close to this: Compressible Flow Around a Wing | Tutorial | SimScale

But this is a compressible Simulation, because it is an aircraft wing. Mine is a wing so a sailing vessel, so the maximum speed will be the wind speed + boat speed. Making it not more than 30m/s. That’s why I chose incompressible.

Then you can also check the vehicle tutorial: Aerodynamic Flow Behavior Around a Vehicle Tutorial | SimScale
What I mean is that the streamlines should remain close to the body for this type of application, especially for a single wing, does this make sense?

Yes it does, but all these tutorials are not helping. I checked all of them and tried several runs. There has to be something fundamentally wrong with my simulation. The last run looked like this:

This is because of the bad cells of your mesh, please check this documentation I sent you before (How to Check and Improve Mesh Quality | SimScale) to refine it further :slight_smile: Cheers

Is that project private? I’d like to take a look to help you

That’s a steady-state solution, right?

I see the velocity values are very high near the upper and lower boundaries. Are you using something like freeStream boundaries?

I disabled the private function. You should have access to the project now.

Yes, it is a steady-state-solution.

Ok thanks, many things:

1 - Do listen to @tsite advise and improve your mesh quality. Use a structured mesh (hex-based). A good mesh is arguably the most important part of the simulation process. No matter how powerful is your computer or accurate is the CFD method used, you need a good mesh to achieve good results.
2 - Poor quality grids need a very robust interpolation scheme. Use a bounded Gauss upwind first (always) for div(phi,U). If it works well, you can jump to a second order-accurate scheme (gauss-linear upwind).
3 - The solver needs to solve a complete fluid dynamics case but we aren’t giving it much help. Do set an initial velocity in the Ux direction to give the solver much-needed help to come out with the solution. The initial velocity of the internal field should be the same as used in the inlet boundary.
4 - While using slip-walls as boundaries is not a bad approach, it is much better to use a freestream boundary, unless you are simulating a wind tunnel. SimScale has already prepared some documentation for it: Velocity Inlet & Velocity Outlet Boundary Conditions | SimScale .
4- If the object (wing) starts at the wall, it is much better to use a symmetryPlane.

(1), (2) and (3) are or may be error-generators. (4) and (5) are improvements.

I hope this helps,

Regards,

J.A. Gutiérrez

1 Like