CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Query on POROUS MEDIA (http://www.cfd-online.com/Forums/cfx/92764-query-porous-media.html)

MPrabanchan September 24, 2011 13:05

Query on POROUS MEDIA
 
I'm doing a project in Pressure Drop analysis on a Catalytic Converter.In my model I need to split the porous media in to 3 regions to have different porosity in each region.Can any one say how to split?

ghorrocks September 25, 2011 06:16

If the media is a volume then define 3 mesh volumes. If the media is thin then define 3 cross sections, you can call them interfaces if you like.

MPrabanchan September 25, 2011 11:07

I Split the regions while modeling.There comes a error report as below
"Default Domain
Substrate3
Substrate1
Substrate2
If the isolated regions do not have the pressure level set either
by the boundary conditions or using a reference pressure equation,
you may encounter severe robustness problems.
This situation may have arisen because a domain interface was not
properly defined during problem setup. Please carefully check
the setup.
The solver will stop now and write a results file. The isolated
regions can be visualised in CFX Post by making plots of the
variable "Isolated Volumes".
If you are sure that the pressure level is set in each isolated
fluid region then you can force the solver to turn off this check
by setting the expert parameter "check isolated regions = f".
+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. |
+--------------------------------------------------------------------+
End of solution stage."

ghorrocks September 25, 2011 18:12

Yo have not set it up correctly. The domain should include all these regions. Then you define the volumes as sub-domains.

Chander September 25, 2011 18:47

As Glen already said above, you have not setup your case properly.

i recently did something very similar. I had a layer of porous medium and I wanted to define different porosity and permeability in three different parts the porous volume. this is how I did it.

1. I use structured mesh. So I simply assigned different blocks to the three regions thus defining separate volumes for the three regions of the porous medium.

2. then in CFx, I created three separate domains each containing one region of the porous medium. For each domain, I defined porous medium parameters as per my need.

3. I created porous-porous interfaces between the three porous domains.

And it worked without any problem. hope this helps.

ghorrocks September 25, 2011 19:31

You do not need to make the porous regions different domains. They can all be one domain, just the porous region defined as a sub-domain.

The only reason why you would put them as different domains is to generate interfaces so you can put interface conditions (eg resistance) on them.

evcelica September 26, 2011 18:38

Instead of remodeling you could also define the porosity with a user defined function with respect to a global coordinate. I'd do this instead of re-modeling/remeshing and redefining a bunch of boundary conditions.


All times are GMT -4. The time now is 16:12.