CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Pointwise & Gridgen (http://www.cfd-online.com/Forums/pointwise/)
-   -   [Pointwise] Boundary layer mesh (http://www.cfd-online.com/Forums/pointwise/113895-pointwise-boundary-layer-mesh.html)

James_ February 28, 2013 13:09

[Pointwise] Boundary layer mesh
 
Hi,


I’m trying to generate boundary layer mesh on airfoil profile selig 1223. I’ve 3d model geometry and I use option extrude normal to boundary (hyperbolic extrusion) but after 1 step generation of mesh is stopped due to error:”positive skew jacobian”


When I change type extrusion on algebraic extrusion it works but quality of generated mesh is poor.


I wonder if it is possible to generate BL mesh with hyperbolic method for any geometry shape or only for special cases

cnsidero February 28, 2013 20:37

James_,

I posted a reply in the previous thread to Ali about the same issue:

http://www.cfd-online.com/Forums/poi...tml#post410315

Those are just general guidelines. While the hyperbolic extrusion can generate beautiful, high quality grids it takes a bit of experience to get to perform. A goofy analogy is it's kind of like a Ferrari - tough to drive the first time but once you learn you can make it do amazing things.

I can [most likely] give better guidance if you post some pictures of your mesh.

-Chris

James_ March 2, 2013 15:15

4 Attachment(s)
Thank you very much Chris for your hints. Now I can generate 10 layers but I need at least 26, Iíve tried reducing volume smoothing parameter below 0.005 but extrusion is still stopped after 10 steps.


Wing dimensions:
Wing length 2000mm, connector is divided into 500 points
Chord length 500 and 300mm, two connectors upper and lower are divided into 300 points
Spacing (Fig. spacing) equals 0.1 mm


I have also tried generating BL without wake region but in this case extrusion was stopped after 1 step.


Could you suggest me some changes in extrusion parameters?
Do you know where I can find more information about hyperbolic extrusion in Pointwise? I have only tutorial workbook.




PS
I hope one day cfd buy me Ferrari :)

Attachment 19480

Attachment 19481

Attachment 19482

Attachment 19483

taxalian March 3, 2013 16:59

1 Attachment(s)
Hi James,
Well i think you made a mistake, may be you need to define proper boundary condition to constrain your span-wise (y/z) and x-coordinate. This can be done in choosing the appropriate boundary condition within the Create - Extrude - Normal command and then choose the last tab - boundary condition.

Another tip is try to decrease the growth rate to about 1.025 or 1.05 and then slowly increase this after 15 to 20 layers.

See the attached picture, i am able to get 50 extruded layers without any trouble.

I hope this helps, good luck.

cnsidero March 4, 2013 12:49

James_,

I think I have an idea but it's still tough to tell what's going. Are you able to email me the mesh?

If not, I think the problem area is the trailing edge. First, if you try to extrude without a wake sheet, because the trailing edge is sharp, it's likely going to have difficulties. This is caused by the large turning angle around the trailing edge (probably 340-350 deg). In these situations, if the spacings on the opposite surfaces of the external corner, the upper and lower surfaces at the trailing edge in this case, aren't exactly the same (or very close to it) negative volumes will occur. This is because the algorithm computes the surface normal at each point from an area-weighted averaging of the neighboring points. For sharp external corners, for the extrusion to be successful, the normal needs to bisect the angle almost perfectly. That means the adjacent spacings have to be same or the normal will get pulled to one direction and invert the cell.

If you attempt the wake sheet, since your airfoil has a lot of camber and the turning angle at the trailing edge is quite high I would suggest creating a much more organically shaped wake sheet (i.e. follows the direction of the trailing edge and then curves back to horizontal) much like the actual flow would do. Then ensure the streamwise spacing of the wake sheet at the trailing edge matches the airfoil trailing edge spacings.

If you're careful about either approach you should be able to get it work. Again if you can, send me the mesh and I'll give you specific instructions.

-Chris

Quote:

Originally Posted by James_ (Post 411085)
Thank you very much Chris for your hints. Now I can generate 10 layers but I need at least 26, Iíve tried reducing volume smoothing parameter below 0.005 but extrusion is still stopped after 10 steps.


Wing dimensions:
Wing length 2000mm, connector is divided into 500 points
Chord length 500 and 300mm, two connectors upper and lower are divided into 300 points
Spacing (Fig. spacing) equals 0.1 mm


I have also tried generating BL without wake region but in this case extrusion was stopped after 1 step.


Could you suggest me some changes in extrusion parameters?
Do you know where I can find more information about hyperbolic extrusion in Pointwise? I have only tutorial workbook.




PS
I hope one day cfd buy me Ferrari :)

Attachment 19480

Attachment 19481

Attachment 19482

Attachment 19483


James_ March 4, 2013 16:47

Thank you taxalian and cnsidero for yours advices
I'll try to introdce them to my project

robboflea July 31, 2013 15:18

2 Attachment(s)
I am having a similar problem and I don't know how to solve it.
I am working on meshing a turbine blade following the steps of the video on the website.

The problems is that I need a really small first cell distance because I need y+ to be around one. When using a first wall distance this small the building of the BL block by means of extrusion fails while creating the first layer due to negative skew Jacobian.

By increasing the first node distance the number of faulty cells decreases until it finally creates the o-grid for the boundary layer but at this point the first cell distance is not small enough for obtaining a reasonebl y+.

I tried to play with all parameters in the "attributes" tag but without success. Any suggestions? Attached is a picture of the domain.

Also I noticed (but I don't know if it is meaningful or it just a visualization issue) that I seem to have in some points like for example at the trailing edge another edge, running close to the mesh edge. It might be that the cause of the problem?

Is there a way to clean up the geometry in pointwise? The only thing I did was to group the quilts in a model within tolerance so that it was waterproof.

Thanks a lot for the help.

Rob


Quote:

Originally Posted by cnsidero (Post 411434)
James_,

I think I have an idea but it's still tough to tell what's going. Are you able to email me the mesh?

If not, I think the problem area is the trailing edge. First, if you try to extrude without a wake sheet, because the trailing edge is sharp, it's likely going to have difficulties. This is caused by the large turning angle around the trailing edge (probably 340-350 deg). In these situations, if the spacings on the opposite surfaces of the external corner, the upper and lower surfaces at the trailing edge in this case, aren't exactly the same (or very close to it) negative volumes will occur. This is because the algorithm computes the surface normal at each point from an area-weighted averaging of the neighboring points. For sharp external corners, for the extrusion to be successful, the normal needs to bisect the angle almost perfectly. That means the adjacent spacings have to be same or the normal will get pulled to one direction and invert the cell.

If you attempt the wake sheet, since your airfoil has a lot of camber and the turning angle at the trailing edge is quite high I would suggest creating a much more organically shaped wake sheet (i.e. follows the direction of the trailing edge and then curves back to horizontal) much like the actual flow would do. Then ensure the streamwise spacing of the wake sheet at the trailing edge matches the airfoil trailing edge spacings.

If you're careful about either approach you should be able to get it work. Again if you can, send me the mesh and I'll give you specific instructions.

-Chris



All times are GMT -4. The time now is 17:10.