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] Conjugate CFD - Heat Transfer mesh (http://www.cfd-online.com/Forums/ansys-meshing/67613-conjugate-cfd-heat-transfer-mesh.html)

Subhadeep August 20, 2009 10:41

Conjugate CFD - Heat Transfer mesh
 
Hi

Trying to achieve this task of meshing a 3D steady state problem in ICEM. Goal is to achieve a mesh capable of conjugate flow - heat transfer simulation. Have two solid walls with thickness and rest of the walls will be thin with thermal BC.

There is fluid flow passing from one channel into the main flow domain through a wall.

In ICEM I have tagged all the surfaces and have 3 material point: Fluid, Solid1, and Solid 2.

Solid1 and Solid 2 will be done using unstructured tet mesh (not too fine)

Fluid will be simulated with prism layers at the surface for resolving boundary layer and rest in unstructured tets.

Have created successfully and modeled just the fluid before in ICEM. Having a hard time understanding how to put the solids in the meshing too. For example an interface between solid and fluid : one side is facing the fluid so I want prism on that side of the interface 1st and then the tets. On the solid side of the interface I just want tets. How do I make ICEM understand that?

Any help will be deeply appreciated.

PSYMN August 21, 2009 08:59

Prism Volume Parts
 
On the Params by Parts menu where you selected the surface parts for Prism, you can also select the volume parts…

The default (no volume parts selected) means to grow prism from any selected surfaces into any adjacent volume regions.

But if you select a volume region(s) (in your case, Fluid), then the prisms will only grow from selected surface parts into selected adjacent volume parts.

One other thing to think about with Conjugate heat transfer… Some users love how ICEM CFD effortlessly makes these node for node connected meshes, but others would prefer a coarser mesh, or even a quadratic mesh, on the Solid Side. If you want non-conformal mesh, you will just need to mesh the fluid region and solid regions separately… If you just want the solid mesh to be quadratic, you can make the conversion on just the Solid part thru the Edit Mesh Tab.

rskrishna87 May 30, 2011 04:17

Hi,

How did you transfer both the solid and fluid into cfx 13.0? can you please tell me.

thanks,

Krishna

PSYMN May 31, 2011 12:14

Just make sure to have the volumes in separate PARTS. You can do that with different material points for Tetra or by assigning blocks to different parts (right click on the PARTS branch of the tree and "add to part").

When you get to CFX, you tag each of these regions as what ever type of solid or fluid you want...


All times are GMT -4. The time now is 01:35.