CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Pointwise & Gridgen (http://www.cfd-online.com/Forums/pointwise/)
-   -   zero-thickness wall (http://www.cfd-online.com/Forums/pointwise/128940-zero-thickness-wall.html)

lakeat January 24, 2014 11:20

zero-thickness wall
 
Hi,

Is pointwise able to generate a zero-thickness wall and then mesh around it? How? Thanks

cnsidero January 25, 2014 12:29

4 Attachment(s)
Daniel.

Yes. For domains, once the first edge is defined (which has to be closed) for addtional (internal) edges you simply need to choose the connectors twice. For blocks, once the first face is defined (which has to be closed), for additional (internal) faces there is an option to add the face as a baffle.

See the attached sequence of images for an example on domains. You'll notice in the first one I chose two connectors for the internal edge and in the second image I've chosen the same two connectors again (see how the arrows double back).

Quote:

Originally Posted by lakeat (Post 471625)
Hi,

Is pointwise able to generate a zero-thickness wall and then mesh around it? How? Thanks


lakeat January 28, 2014 14:43

Thank you Chris, I will try it out.

lakeat January 30, 2014 12:53

1 Attachment(s)
I made it.
Attachment 28359

Hmm, I am confused now how to convert the t-rex mesh to prisms, why it is always in grey. Did I miss something here?

PS: Are there any macros available that can build quickly a rectangular topology or a circular topology?

lakeat January 30, 2014 16:40

Hi Chris,

In order to generate a mesh for OpenFOAM with baffles, I have to extrude the 2D mesh in the 3rd direction. And then export the CAE. But now, it seems to me that the extrusion does not work for the baffles. What I'm saying is this, normally, you extrude a mesh, then connector becomes a surface, a surface becomes a domain, right? But now a baffle is not extruded to be a surface. The problem with that is that I can't in CAE boundary condition set tab to assign the b.c. to the baffles. Of cause I can manually extrude the connector here to create a surface and then set the boundary condition, but still in exporting to the openfoam mesh, there is no such boundary patch. Any ideas? Thanks!

dgarlisch February 2, 2014 12:22

Pointwise has a great collection of scripts available on GitHub. I think this is the script you want.

I also have some good/bad news...

GOOD:
There is a script in my personal GitHub account that thickens a 2D grid into a 1 cell deep (or more) 3D grid. All boundary conditions in the 2D grid are automatically transferred to the corresponding extruded domains in the resulting 3D grid.

BAD:
This script will only work directly with solvers that support both 3D and 2D grid mode. OpenFOAM does not support 2D mode. :(

WORKAROUND:
If you want to avoid thickening the grid manually, you will need to:
  • Load your 2D OpenFOAM grid into Pointwise.
  • Change the solver to one that supports 2D mode (e.g. CGNS).
  • Switch the mode to 2D (menu CAE/Set Dimension/2D).
  • Thicken the 2D grid with the script.
  • Switch solver back to OpenFOAM.
  • Reset the BC and VC types.
Good luck!

dgarlisch February 2, 2014 12:59

Converting trex tets to prisms is done during export. To enable, select the Combine Aniso checkbox on the export options dialog.

lakeat February 3, 2014 12:44

Thank you David. But I still don't know how to set the boundary condition for a baffle? (As I have mentioned in post #5) This seems to have nothing to do with OpenFOAM. Let's me give an simple example:

In a 2D CAE case, say it is a CGNS mesh. And there is a baffle inside, and I can set one connector as inlet, another as outlet, and so on, but I can't select the baffle to set it as a boundary condition. Why?

tcarrigan February 3, 2014 13:36

Daniel,

You need to check the box "Select Connections" when assigning boundary conditions.

dgarlisch February 3, 2014 14:01

1 Attachment(s)
Quote:

Originally Posted by lakeat (Post 473158)
Thank you David. But I still don't know how to set the boundary condition for a baffle? (As I have mentioned in post #5) This seems to have nothing to do with OpenFOAM. Let's me give an simple example:

In a 2D CAE case, say it is a CGNS mesh. And there is a baffle inside, and I can set one connector as inlet, another as outlet, and so on, but I can't select the baffle to set it as a boundary condition. Why?

In Pointwise, a baffle is considered to be a connection between two blocks. In the case of a baffle, it is the same block on both sides.

In CAE/Set Boundary Conditions..., you should see a listing of two-sided "connections" at the bottom of the BC dialog box. You must select the Select Connections check box to set BCs on these connectors.

I have attached an image.


All times are GMT -4. The time now is 07:03.