[madakaczka]

Hi,

I am currently in my final year at the university and what I am working on are wind turbines. What I am trying to do at the moment is make a simple model of the wing and study effects of flow on it.

I would like to examine the wake behind the airfoil in more detail however, I am not entirely sure how to go about meshing the region behind the airfoil in the wake to a finer mesh. Would anyone have some sort of good tutorial on how to do it perhaps?

Best Regards,
Kacper

[fluid23]

There are a few different approaches you can take. However, you need to clarify your statement a little to know which is going to be your best bet. Is this 2D analysis of the airfoil or 3D analysis of the rotor blade? Is the blade rotating or not? You use the terms wing and airfoil interchangeably, each meaning something specific, and I am guessing you meant something else entirely (i.e. a rotor).

That being said…
1) Volumetric Controls – These can be used to prescribe a specific cell size in an area of your domain. You define the shape using a CAD body and prescribe the cell size, the mesher will try to incorporate what you specify. You need to be careful because you can easily define a mesh that will be too dense for you to actually generate. This will require you to have some idea of the size and shape of your wake a priori.

User Guide > Pre-Processing > Meshing > Volumetric Controls

2) Wake Refinement – Star-CCM has an option to include wake refinement. You select the surface that will generate your wake and specify some direction and size options. The mesher will generate a refinement based on your inputs. This is going to yield a smoother transition than the volumetric controls, but seems to take longer to complete. Sort of a trade-off there I guess. It can also be a little funny figuring out the correct inputs the first time you do it. You may have to play around, so start with a coarse mesh, work out your refinement, then bring the mesh fidelity down to where you need it. If you aren’t using parts based meshing then this will be limited to trimmed cell mesher only.

User Guide > Pre-Processing > Meshing > Mesh Refinement > Wake Refinement

3) Field Function Refinement – This allows you to refine cells based on the value of some parameter of interest (turbulent energy, energy deficit, velocity gradient, etc…). This requires you to already have an unrefined solution, you apply the field function refinement, then remesh and continue running.

User Guide > Pre-Processing > Meshing > Mesh Refinement > Field Function Mesh Refinement

That being said, I am not sure how well these work with a rotating flow field or bodies depending on how you choose to approach this. Maybe someone with more experience refining a rotating flow field can chime in here…

[Andi_Didi]

Maybe you can meshing with Direct Mesh.

In Operations > New > Mesh > Direct Mesh

You can learn direct mesh from this tutorial.

https://drive.google.com/open?id=1ey...NVxwS3pPK6EFcU

I hope it help.

[ping]

please dont use the direct mesher for a wind turbine - it is not designed for anything like that - it is for electric motors maybe pipes and extruding existing mesh along good 3d-cad it is more like a 2.5d mesher