[Bigio]

Hi All,
I'm a student of Aerospace Engineering and I'm actually working about a thesis about two airfoils in tandem with the second one very close to the first. I have to solve the 2D fluid arond the airfoils and i'm trying to use ICEM CFD to prepare the mesh.
I have some problem because i'd want to do an unstructured mesh but i'm not able to guide the mesh in some regions of the environment, for example I don't know how to do a more dense mesh in the wake of the airofoils.
I attach an image of my problem.
I hope someone could help me.
Thanks a lot.

[PSYMN]

ICEM CFD is really a collection of meshing technologies, each with their own advantages and some disadvantages.

You are using the patch dependent surface meshing method (a recursive loop paving algorithm), so there isn't a really nice way to control the refinement between curves (no sizing function or back ground grid). You could control the refinement by creating a line or segmented region between the airfoils (gives you control over the sizes along the edge of a loop), then you could control the mesh refinement along this line or in this region.

Alternativly, you could switch to patch independent tetra (based on the octree algorithm and hooked up to a sizing function) and use something called a "density region". This is usually intended to control the refinement in a region of a 3D volume, but it can be used on a 2D surface if you use this method... It is one of the options on the mesh tab. Note, it will not work with the patch dependent surface meshing method.

Another alternative would be ANSYS Meshing. It can use a very nice sizing function and its patch conforming (a combination of the TGrid Delaunay paver and the next-gen Gambit sizing function) surface mesh method is probably better suited to CFD than the ICEM CFD Patch Dependent method.

[Bigio]

Hy Simon,
thanks a lot for your answer.
I also thought to divide the field in regions with lines and refine the mesh in these region, but the problem is that later, when i run fluent these lines are seen like wall and i can't change the boundary conditions on these.
Ansys assistance tell me to try to use Ansys Meshing, but i have a lot of difficulties to create the geometry in design modeler or to import it from Icem.
I'll try to use the indipendent method refining the mesh with the 'density region' tab.
I'll tell you if this work successfully, thans for the moment.
Andrea

[Bigio]

Hi Simon,
I'll try use the indipendent method and in effective I'm able to use the density region tab to refine the mesh in some zones, but i loose the possibility to create the layers for the strucutred mesh in prossimity of the airfoils, where I have to capture the boundary layer.
In fact, in the patch dependent method i'll use ' curve mesh setup--> ' Height, ratio, numbers of layers'.
For the inpendent method this tab doesn't work.

[PSYMN]

1) With the patch dependent method using sub regions, you can just delete the line elements so there are no internal walls... Just use a name for those curves like "construction" or something like that, and then after the mesh is generated, Edit Mesh => Delete Elements; Select by Part => CONSTRUCTION...

2) With Patch Independent meshing, you need to insert a prism layer after the fact... Do a google search for "blayer2D" for specifics of how to insert a 2D boundary layer with ICEM CFD...

[eirikurjon07]

Hi Simon
I am doing a very similar study as descibed in this thread and I would like you the patch independent method since is offers this excellent control of where to put density regions as well as it produces more "even" mesh in my case than the dependent method.

Your last reply suggests a google search for blayer2d on how to insert a prism boundary layer into the independent method. I have done some research but I am unable to find anything. I have been using line elements with the dependent method to obtain the density I require but that is somewhat not very elegant.

Could you please describe how to do this with the patch independent or what steps need to be taken in oder to achive a prism boundary layer with the independent method. It would be really helpful.
Eiki

[PSYMN]

I have done a number of posts on CFD online on the subject of blayer2D. I had hoped that a google search would find those for you.

I just tried and found many links...

Basically, it is an option you can turn on under Advanced prism options that will allow you to insert ICEM CFD prism in a 2D mesh... (ICEM CFD Prism was intended for 3D so you need to turn on this option to get it to work for 2D).

Best regards,

Simon

[hoyos98]

I suggest you visit https://aeroptimal.com/mesh (you must create an account to use this module), where you can create a full structured airfoil mesh - https://youtu.be/4Opu0zk7gFk . You can export .su2 .msh .foam .vtk

[Gert-Jan]

Are you trying to gain new customers with all these posts?
Keep in mind that it can be marked as SPAM.

[hoyos98]

The meshing at aeroptimal.com is free, we do not have customers. Moreover, I'm promoting the meshing in the posts where I consider the users can find a solution to the question.