CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   velocity at porous region (http://www.cfd-online.com/Forums/fluent/28525-velocity-porous-region.html)

CHUBBY May 13, 2001 08:38

velocity at porous region
 
Hi everyone, I am interested in knowing about the velocities of a particle before and after entering the porous media, When I see velocity vectors of a porous media, It shoes some vectors, I am not able to understand whether the velocity vectors of the particle are of the region before the entry into porous region or after the entry of the porous media. If suppose, they are velocity vectors of entry , Is there any way to find the velocity vectors of particle after they leave porous media.And vice-versa as well.. thank U any suggestions are welcome, Chubby

Evan Rosenbaum May 14, 2001 12:17

Re: velocity at porous region
 
Be careful what your're looking at. The FLUENT porous medium model uses a momentum sink term based on the superficial velocity of the flowing fluid, not the actual velocity through the reduced-area porous section. Flow acceleration through the reduced area of the porous medium is not calculated or displayed. I'm not sure how it would work with a particle, so be careful.

CHUBBY May 15, 2001 07:57

Re: velocity at porous region
 
hi, U mean to say that the velocity displayed for the porous media is the inner velocity. then is there any way to find the outer velocity , ie.. velocity of fluid after leaving teh porous media. Any suggestions are welcome, Chubby

Lanre May 15, 2001 23:37

Re: velocity at porous region
 
The velocity of the fluid on either side of the porous media will be 'correct'. The velocity inside the porous region will not be the true velocity of the fluid. To get the approximate true velocity of the fluid for the transport of your particles, you need to divide the computed velocity by the void fraction or porosity of your porous media. After obtaining your converged solution for the 3D fluid flow field:

1. define three UDS's (Define->Models->User Defined Scalars...

2. create a custom field function (CFF) for each component of velocity, ie. u, v and w are x-velocity, y-velocity and z-velocity

3. Patch your three CFF's into the UDS's by checking the "field function" box into the fluid zone corresponding to the porous region. This will fill the UDS with values of the current velocity.

4. create a custom field function (CFF) for each component of velocity based on the UDS's filled with the current veolcities, ie. porous-u, porous-v, porous-w, to be UDS-0/porosity, etc.

5. Patch the new CFF's (velocity/porosity) into x-, y- and z-velocity for the porous region.

The last step fills your x, y and z-velocity fields in the porous zone with corrected values. When you perform your DPM calculation, these values will be used. It also works with transient transport of constant density scalars, e.g. tracers although FLUENT now has a porosity term in front of the time-derivative term so the above procedure is moot for those cases.


All times are GMT -4. The time now is 22:36.