CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   RhoExplicitPorousSimpleFoam (http://www.cfd-online.com/Forums/openfoam-solving/59535-rhoexplicitporoussimplefoam.html)

r2d2 July 30, 2007 04:36

Hello, I have a question (or
 
Hello,
I have a question (or more) about rhoExplicit(Implicit)porousFoam:
1. In specifying e1 and e2 in the porousZones, that gives me the orientation of the resistance "vector", right?
2. How does a given value of K (permeability m**2) and porosity phi translate into the "d" and "f" terms of Darcy-Forchheimer or the C0/C1 parameters of powerLaw ? Does anyone have some references?
Cheers,
Radu

olesen July 30, 2007 05:18

From the porousZone.H:
 
From the porousZone.H:

Porous zone definition based on cell zones and parameters obtained
from a control dictionary constructed from the given stream.
The orientation of the porous region is defined with the same
notation as a coordinateSystem, but only a Cartesian coordinate
system is valid.

Implemented porosity models:

powerLaw (C0/C1 parameters)
S = - rho * C0 * |U|^((C1 - 1) / 2) * U

Darcy-Forchheimer (d/f parameters)
S = - (mu * U * d + rho/2 * |U| * f) * U

The model does not include correction of the temporal terms.


This seems to cover all of your questions about orientation, porosity (no temporal terms yets) and the Darcy resistances.

r2d2 July 30, 2007 06:10

Yes, I saw porousZones...so d
 
Yes, I saw porousZones...so d is the inverse of K and f dunno...(?) Does the porosity (phi) of a material enters the fray in anyway? (or just via K,
and possibly f)

otsuki July 31, 2007 01:36

Hi, The porosity is not consi
 
Hi,
The porosity is not considered explicitly
for both powerLaw and Darcy-Forchheimer models.
i.e. velocity U in these models is
not a "physical velocity" but a "superficial
velocity".
Masato

markusrehm November 6, 2009 07:27

Multiple cell zones
 
Hello,

I want to use different cell zones but only the first one is recognized. My porousZones-Dict looks as follows:

Code:

1
(
    cat1
    {
        porosity    0.5;
        Darcy
        {
            d  d [0 -2 0 0 0 0 0] (11111 11111 11111);
            f  f [0 -1 0 0 0 0 0] (111 111 111);
        }
    }
)

2
(
    cat2
    {
        porosity    0.6;
        Darcy
        {
            d  d [0 -2 0 0 0 0 0] (22222 22222 22222);
            f  f [0 -1 0 0 0 0 0] (222 222 222);
        }
    }
)

3
(
    cat3
    {
        porosity    0.7;
        Darcy
        {
            d  d [0 -2 0 0 0 0 0] (33333 33333 33333);
            f  f [0 -1 0 0 0 0 0] (333 333 333);
        }
    }
)

Should it be defined that way? The cell zones are available.

Regards, Markus.

navier-stokes November 6, 2009 07:47

Hi Markus!
There may be a problem with your list definitions. Have a look at the UserGuide (Section 4.2.4).

markusrehm November 9, 2009 03:27

Hello,

you are right it should read:

3
(
cat1
{
porosity 0.5;
Darcy
{
d d [0 -2 0 0 0 0 0] (11111 11111 11111);
f f [0 -1 0 0 0 0 0] (111 111 111);
}
}

cat2
{
porosity 0.6;
Darcy
{
d d [0 -2 0 0 0 0 0] (22222 22222 22222);
f f [0 -1 0 0 0 0 0] (222 222 222);
}
}

cat3
{
porosity 0.7;
Darcy
{
d d [0 -2 0 0 0 0 0] (33333 33333 33333);
f f [0 -1 0 0 0 0 0] (333 333 333);
}
}
)

Thank you, Markus.

olesen November 10, 2009 03:28

It might be more convenient, and only very marginally less efficient, if you simply drop the size from the PtrList.
For example
Code:

(
    cat1
    {
    ...
    }

    cat2
        {
    ...
    }

    cat3
    {
    ...
    }
)

Internally it will simply use a linked-list during the reading and then move everything over to the PtrList.


All times are GMT -4. The time now is 19:08.