CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Define another cell zone (http://www.cfd-online.com/Forums/fluent/116460-define-another-cell-zone.html)

billue123 April 19, 2013 12:12

Define another cell zone
 
I am modelling a gas water heater for my FYP so i have do analysis on ansys 14.0. I have constructed the body and even the mesh, but unfortunately when i go into fluent it only give me a single option of cell zone conditions where as my geometry is of 2 concentric pipes, one with flue gases and other of water. Please help me in this regard. how can i separate the cell zone and define 2 different zones, one for each tubes?

billwangard April 19, 2013 15:56

Separate cell zones
 
Easy way to separate one cell zone into two:

1. Adapt->Region
2. Define a rectangular block that marks the inner cells of your zone
3. Mark the cells, but do NOT adapt.
4. Mesh-> Separate-> Cells...
5. Separate based on adaption register. Pick the cell zone and register that you just created.
6. Click separate.

Now you will have two separate cell zones. Note that additional face zones will be created. Interiors that mark the new boundary, and other zones that span the two zones will be separated.

To identify the zones,

1. Surface-> Zones...
2. In the left panel, seleect the newly created cell zone (and perhaps the other one, too). For each one, click create surface.

then in the Display mesh panel, you should be able to see the cell zones in the list of surfaces.

Hope this helps,
Regards,
Bill Wangard
Engrana LLC

diamondx April 19, 2013 15:58

separation can be done in fluent , but it will never be as precise as in the meshing software. how you used icem cfd for that ? if so you need to define too bodies. have a look at the link a attached in my signature. it's a small book where i explain the principle of having multiple bodies while meshing...

billue123 April 20, 2013 07:40

thanks alot. i have tried your method and it seems to work a bit. can you please tell me more detail about defining two zones in meshing? i have not really used icem cfd as such..
thank you

jdrch April 20, 2013 18:32

I've never used ICEM, but I do surface tria meshing in HyperMesh before doing volume meshing in ANSYS Fluent Meshing Mode. Generally speaking you should place the mesh sections you want as separate zones in separate components (the actual term may vary) during the meshing process itself.

billue123 April 21, 2013 09:24

i have added two extrudes as frozen representing two bodies but when i open fluent they have single cell zone meaning they have 1 fluid flowing through them.. how can i separate components or zones at meshing stage?

mayurb February 16, 2015 08:20

I cannot select the region by clicking mouse.
"Click on diagonal points defining the
hex in the graphics window with
the MOUSE-PROBE mouse button" This window is appeared?

ankit1512 November 23, 2015 11:57

Quote:

Originally Posted by billue123 (Post 421778)
I am modelling a gas water heater for my FYP so i have do analysis on ansys 14.0. I have constructed the body and even the mesh, but unfortunately when i go into fluent it only give me a single option of cell zone conditions where as my geometry is of 2 concentric pipes, one with flue gases and other of water. Please help me in this regard. how can i separate the cell zone and define 2 different zones, one for each tubes?

Hi there,

If you are using ANSYS Meshing and want to export different mesh regions as different cell zones, I suggest you do the following, group similar cell zones , say fluid zones under a new part in ANSYS DM by selecting the desired objects, right clicking in the object tree and clicking on "form a new part" option. Repeat the above steps for all the cell zones


All times are GMT -4. The time now is 13:30.