CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   What is the significance of the input vectors (e1, e2, d, f) in porousSimpleFoam (https://www.cfd-online.com/Forums/openfoam-solving/90832-what-significance-input-vectors-e1-e2-d-f-poroussimplefoam.html)

 bigbang July 21, 2011 13:28

What is the significance of the input vectors (e1, e2, d, f) in porousSimpleFoam

I'm solving a flow through a radiator using porousSimpleFoam. I understand Darcy's law to the extent of what I read in wikipedia, but what is the coordinate system for and why does d and f have vectors associated with them?

 dima July 22, 2011 04:28

The d f coefficients are relative to the porousZone and the resistance is described in each direction

so it is better to set the porousZone parallel to the e1 e2 plane to ease the entry for d and f

that is what i have understood

 olesen July 22, 2011 06:54

Quote:
 Originally Posted by bigbang (Post 316961) I'm solving a flow through a radiator using porousSimpleFoam. I understand Darcy's law to the extent of what I read in wikipedia, but what is the coordinate system for and why does d and f have vectors associated with them?
Any two of e1, e2, e3 can be used to define a local coordinate system (1,2,3 are the local x,y,z directions).
The d is darcy law and f is the Forchheimer coeff.

If you have an isotropic porosity you can take any arbitrary local coordinate system (eg, take the global system) and use the same d/f coefficients for each direction. For convenience, you can set one coffecient direction and use a negative coefficient (eg, -1) as a multiplier for the other two directions.

We often have porosities that only allow flow in one-direction. Our convention is to specify the coordinate system so that this is the local 'z' flow direction.

 bigbang July 22, 2011 11:18

Quote:
 Originally Posted by olesen (Post 317065) Any two of e1, e2, e3 can be used to define a local coordinate system (1,2,3 are the local x,y,z directions). The d is darcy law and f is the Forchheimer coeff.
I'm not clear on how to specify the value of e1 and e2. Shouldn't there just be a single vector to define the flow direction? My goal is to model the flow through a vehicle's radiator. So the flow is going along the x direction. How would I define that with e1 and e2 in porousZones file

Here is the code taken from angleDuct tutorials in \$FOAM_RUN/tutorials/incompressible/porousSimpleFoam

Code:

```1 (         radiator         {                 coordinateSystem                 {                         e1  (0.70710678 0.70710678 0);                         e2  (1 0 0);                 }                 Darcy                 {                         d  d [0 -2 0 0 0 0 0] (5e7 -1000 -1000);                         f  f [0 -1 0 0 0 0 0] (0 0 0);                 }         } )```

 olesen July 22, 2011 11:31

Quote:
 Originally Posted by bigbang (Post 317122) I'm not clear on how to specify the value of e1 and e2. Shouldn't there just be a single vector to define the flow direction?
But in the general case a porosity is not rotationally symmetrical, thus you need to define an extra vector to specify the orientation of the coordinate system. If you dig into the coordinateRotation documentation, you'll see that any moderate non-orthogonality is absorbed into the second vector.

You might then want to have 'e3' (ie, local z-direction) being the defined flow direction and add 'e1' (ie, local x-direction) to orient about this axis.

 All times are GMT -4. The time now is 18:46.