[erayerisik]

hi everbody, I am new here also ansys workbench and firstly I want to apology for my poor english
I working on an airfoil naca2412, trying to mesh with tetrahedrons method in Ansys ICEM CFD. Its max. skewness value is 0.92. I want to make it under 0.8 Can anybody help me to do it? I have also attached pics.
b1.jpg

b2.PNG

b3.jpg

sharp edge of an airfoil has the worst skewness value(0.92) ,
d1.jpg
d2.jpg

thank you all.

[erayerisik]

Is there anyone to help me??

[siw]

Looking at your images I would say the mesh size is far to coarse at the trailing edge (TE) and that you need many more prism layers to get a smooth transition from the last prism to the first tetrahedral elements. As a quick test you could try the default inflation settings with Smooth Transition just to see what happens to the quality metrics. If you find that the inflation layers are not wrapping around the sharp TE (I assume it's sharp) then increase the Maximum Angle to 180 (in the Outline go to Mesh > Inflation > View Advanced Options = Yes to see that).

In you third image why are there three coloured regions (grey, blue and green)? If your just simulating the flow around a single wing then just use a single fluid domain body.

You should also consider using a body of influence or edge sizing along the TE to refine the mesh and better capture the wing wake.

Post you model for others to try.

[erayerisik]

hi siw,
it is 3D model and it has 7.25degree angle of attack. I slide it 3 part and formed it as a new one part thats why it has 3 part(3 different colour, grey-blue-green). I had slided it 3 part to get better mesh quality through TE, also upside and downside of airfoil along fluid domain. If I dont slide it 3 part I cant give it face size along these line.
yes my te is sharp and I changed max angle to 180 degree. Even if I change first layer thickness to smooth transition max skewness is again 0.92.
I also tried using edge sizing along te with used face sizing on airfoil but this time it forces to my computer too much then stop meshing.
thank you for answer
eray.

[siw]

If you can please post your model.

[erayerisik]

I am using ansys 14.0 and upload my model to google drive here is the link thank you so much siw

https://drive.google.com/folderview?...U0&usp=sharing

[siw]

I've imported your model have have the following comments/observations:

1. As I indicated in the above post the use of three fluid bodies for this is rather unhelpful and it would be simpler and less constraining to have only one fluid body and use either the TE or body of influence for local element refinement. Also the joint of the three bodies is only very close the TE where the chord is the greatest.
2. This looks like a wind turbine blade. Why have you left only a very small gap between the blade tip and the side face of the fluid domain? This should be as large as, say, the upstream fluid domain extent for a 3D simulation otherwise the flow is artificially constrained.
3. Why have you made these two smallish surface patches at the farfield? They will make smaller elements in this region as opposed to the rest of the farfield surface (see image 1).
4. The wing root has elements on it. This should not be the case since there is no flow there (see image 2).
5. The seven layers in the inflation layer is really thin. I guess you are working with a target y+ of about 1. The prism to tetra transition is huge so this will inaccurately predict the boundary-layer.
6. Is this for mesh for a simulation requiring rotational periodicity to represent multiple blades on a wind turbine? If so the farfield shape is not right. I'm just making a guess as to the purpose of this and may be wrong.

Rather than uploading the *.meshdat file can you upload the Workbench project file (*.wbpj) or better the Workbench archive file (*.wbpz). That way some changes can be made to the geometry in DesignModeler, which would help the mesh rather than doing it all in Meshing which may not really get the best hybrid mesh.

[erayerisik]

thank you so much for answer siw,
I am trying to upload workbench file but its size 1.13gb can you suggest me any other option.

[siw]

Clear out the generated data (see image 1, sorry the pictures are really poor quality but you should get the idea). To make things even easier archive and upload the Workbench project (see image 2), that way you only have to send the *.wbpz file and not both the *.wbpj file and the directory containing the data files.

[erayerisik]

https://drive.google.com/file/d/0B0z...it?usp=sharing

I made that what you said, I hope it works.

[erayerisik]

hi siw,
I want to analysis drag and lift coefficient also pressure and velocity vector of this wind turbine blade as you guess, I have researched about fluid domain and saw that generaly c grid fluid domain is using to analyse airfoil. Is that also wrong? yes it is 3blade wind turbine but I want to simulate just one blade of it. Is that wrong aproach?

[siw]

I would say a streamwise C-grid is better if you were to make a multi-block structured mesh. But for a hybrid mesh just using a box or cylinder domain would not make any difference - apart from some additional elements. But there are many benefits to the multi-block mesh if you have the software (e.g. ICEM Hexa).

If this is part of, say, a three-bladed turbine then you may want to include the hub and use rotational periodicity and model just one third (e.g. see the Pointwise video at http://www.youtube.com/watch?v=_o0KOJ7RJXc, same principle just different mesh genertor). It all depends on what you want to do - e.g. is the blade stationary or rotating.