CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Boundary layer problem (http://www.cfd-online.com/Forums/ansys-meshing/89160-icem-boundary-layer-problem.html)

papis June 6, 2011 13:14

[ICEM] Boundary layer problem
 
Hi,

I did an unstuctred mesh of a NACA 0012 with 20 layers.The thing is that it is very bad at the trailing edge and i don't know why.

The procedure i followed to create the mesh was :
  1. Imported airfoil geometry(2 curves)
  2. Create farfield points and surface
  3. Segmented farfield surface with the airfoil curves
  4. Deleted airfoil surface
  5. Defined curve mesh setup(layers/nodes)
  6. Adjusted model tolerance from 0.007 to 1e-07 (0.007 spoiled trailing edge geometry)
  7. Computed mesh
Any ideas what is the problem? I can't really get it

Screenshots
http://147.102.42.169/icem/unstr1.png
http://147.102.42.169/icem/unstr2.png

papis June 7, 2011 06:38

Fixed. I actually did it with multizone Hexa/Mixed blocking. the boundary layer is good.

Don't know why surface mesh fails.

PSYMN June 7, 2011 10:15

Trailing edge curve...
 
2 Attachment(s)
A popular "trick" for unstructured mesh is to create a trailing edge curve behind the airfoil... This gives the prisms something to continue back with...

I have posted other images on CFD Online, but are a couple examples...

papis June 7, 2011 12:22

Thank you very much for you help.

There is another issue I have questions

At the picture below is a multizone mesh. with free blocks.The edge mesh setup in the red circle is like 10e-04(spacing1) where as in the green circle is 10e-05.As you can see free blocks when 10e-05 spacing is used are not meshed.

I guess it's a tolerance issue,because when i make the edge spacing coarser everything is meshed.I know the grid isn't very good,but it's critical to understand the reason behind this issue.Not mater how small the model geometry tolerance is nothing changes. Is there an internal limit for how small unstructured mesh shells can be?

Thanks again for your time.

http://147.102.42.169/icem/multizone.png

PSYMN June 7, 2011 12:45

Meshing a free block uses a recursive loop paving algorithm...

It starts from the line elements around the perimeter and paves inward... Along the way, it checks quality and can make adjustments to the paving in order to keep quality up...

In your case, with the size difference so huge between the horizontal and vertical edges, the elements created are such poor quality that the adjustments can't help and the loop fails to mesh.

When you adjust the sizes on that vertical edge so that the corner mesh is a little closer to matching (you can then have it grow away from that corner), the initial loop has a much better chance and you get a mesh in the loop...

papis June 7, 2011 15:34

You are SO right. Thank you very much for your help.

jasonbot October 23, 2013 17:29

1 Attachment(s)
Quote:

Originally Posted by PSYMN (Post 310867)
A popular "trick" for unstructured mesh is to create a trailing edge curve behind the airfoil... This gives the prisms something to continue back with...

I have posted other images on CFD Online, but are a couple examples...

Can this trick be used for blunt trailing edges too?

I'm having a problem with mine when using patch conforming unstructured mesh setups.

PSYMN October 23, 2013 22:02

Quote:

Originally Posted by jasonbot (Post 458632)
Can this trick be used for blunt trailing edges too?

I'm having a problem with mine when using patch conforming unstructured mesh setups.

In your case, I would suggest setting a smaller size on the trailing edge and setting ortho weight to 0.5 so the prisms will lean into the corner (it looks like you have it set to 1.0)

jasonbot October 24, 2013 02:09

Quote:

Originally Posted by PSYMN (Post 458647)
In your case, I would suggest setting a smaller size on the trailing edge and setting ortho weight to 0.5 so the prisms will lean into the corner (it looks like you have it set to 1.0)

I suspect this is for a 2D prism mesh and not a shell mesh?

PSYMN October 24, 2013 15:50

Quote:

Originally Posted by jasonbot (Post 458664)
I suspect this is for a 2D prism mesh and not a shell mesh?

Oh yea, the shell mesh offset is really just designed for bolt holes (FEA), not 2D N-S flow...

Instead, try using "blayer2D" to generate higher quality boundary layers. There are a number of threads about that if you want more info.

jasonbot October 25, 2013 06:53

1 Attachment(s)
Quote:

Originally Posted by PSYMN
Oh yea, the shell mesh offset is really just designed for bolt holes (FEA), not 2D N-S flow...

Instead, try using "blayer2D" to generate higher quality boundary layers. There are a number of threads about that if you want more info.


***just a note: I am used to using ICEM for clean airfoils, by means of blocking. I am currently working on a high lift airfoil in which blocking has not been successful. Hence my need to learn the unstructured prism mesh tools***

I've tried following steps in the other threads
I have reverted back to the most basic of geometries, a domain with a circle in it. Just to try and get the hang of Prism meshing.

Here are my steps:

1. I created a square in ICEM and drew a circle inside.
2. Create surface from square edges.
3. Create 2D Planar block.
3. Associate square edges with surface edges.
4. Associate block with surface.
5. Use segment tool to cut out the circle where we need no flow.

6. Global mesh setup.
6.1 Volume mesh set up as tet/mixed, robust (octree) method.
6.2 Prism mesh set up as linear with three layers, advanced setting: blayer2d on.

7. Fluid region has prism setting ticked with height, ratio and num layers set.
7.1 apply inflation to curves ticked.

8. Compute mesh, volume mesh, create prism layers checked.

Compute gives me this...

I think I'm doing something wrong with the way I am handling my geometry?


All times are GMT -4. The time now is 05:07.