CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   O-grid generation on segmented confuser (http://www.cfd-online.com/Forums/ansys-meshing/78461-o-grid-generation-segmented-confuser.html)

 LD696 July 22, 2010 06:35

O-grid generation on segmented confuser

2 Attachment(s)
Hi!

I have to simulate a confuser with 19 "subchannels". Since this is my first 3D simulation on such a (at least for me) complex geometry, I got stuck with the blocking. I got a suggestion, that I should create an O-grid in the central channel and then "expand" it to the outer segments. Is that possible somehow? Any goood idea about the blocking strategy is appreciated. I'm using ICEM CFD.

Thanks for the replies.

Daniel

 PSYMN July 23, 2010 09:47

Yup, it is a simple topology, perfect for Ogrids... Is it just structural or is there a fluid flowing thru? I will assume the later and assume that there are surfaces across both ends (inlet and outlet) to close them off.

Start with a single box around this model. Put an Ogrid in that box with faces at the ends. This will give you your initial Ogrid of 5 blocks.

Reduce the index control so you have a single plane (5 faces) on the small end of the pipe. Associate the outer 4 edges with he circle and move them into place... Move the center 4 verts inside the middle circle.

Reset the index control and then use the Align verts command to align the other side.

Then associate the outer edges on the other side to the larger end of the pipe...

After that it is mostly about splitting. Split the Ogrid to get each of the radial steps... Split a vertical and horizontal edge to get the radial structures. Split along the cone if there are any internal walls I can't see in this pic. Between splits, Associate edges that align with curves. You may also want to associate verts with points since this model will have a lot of baffle corners (it just keeps it tidier).

The only tricky thing for this model is that you are dealing with zero thickness baffles. Since the blocking material on both sides is the same, the default is not to create shells on these faces. To force shells, you will need to use the Associate faces option. Either choose closest surface or select the specific parts.

When you are done, please post a final pic... ;^)

 LD696 July 23, 2010 15:25

Thanks for the help I'll post a pic as soon as I can.

 LD696 August 16, 2010 07:42

2 Attachment(s)
Thanks to your help I managed to finish the blocking...I think.

Unfortunately due to the high number of cells (~ 4 million), the lack of time and computational capacity available, I'll have to abandon the project for a while now, so I can't really test the resulting mesh:mad:.

Anyway, thank you for the help; I included pictures of the complete block structure and five cross sections.

 All times are GMT -4. The time now is 22:19.