[sdfij6354]

Hello,

I want to implement the pressure drop along a netting into my OpenFOAM case though the Porous Media and Darcy-Forchheimer-Equation.

OpenFOAM requires the coefficients D and F which I calculated according to
Darcy-Forchheimer law for specifying Porous Zones

F = 2 * a / (deltaP * dx)
D = b / (viscosity * dx)

With deltaP being the pressure drop and dx the length if the Porous Medium in x-Direction (0.5m). "viscosity" is the dynamic viscosity of air (1.789*10^-5 in my case, 20°C and sea level).


First, I measured the pressure drop along the real screen in a wind-tunnel experiment.
I obtained the variables a and b by fitting a second degree polynomial using R-Studio and the curve dp=f(v):

x <- c(7.4,4.3,3.1,0.0)  // inlet velocity
y <- c(67.4,33.2,21.4,0.0) // measured pressure drop
lm(formula = y ~ x + I(x^2))

Results were:
Coefficients:
(Intercept)            x       I(x^2)  
   -0.06875      5.57380      0.48012

Hence,
a = 0.48012
b = 5.57380


Then I calculated F and D

> velocity <- 4.2
> deltaP <- a*velocity^2+b*velocity
> print(deltaP)
[1] 31.87928

> dx <- 0.5
> viscosity <- 0.00001789
> F <- 2 * a / (deltaP * dx)
> D <- b / (viscosity * dx)
> print(F)
[1] 0.06024227
> print(D)
[1] 623119.1

and inserted it into fvOptions in /case/constant.

    explicitPorositySourceCoeffs
    {
        selectionMode   cellZone;
        cellZone        porousBlockage;

        type            DarcyForchheimer;

        DarcyForchheimerCoeffs
        {
            d   (623119.1 -1000 -1000);
            f   (0.06024227 650 650);

            coordinateSystem
            {
                type    cartesian;
                origin  (0 0 0);
                coordinateRotation
                {
                    type    axesRotation;
                    e1  (1 0 0);
                    e2  (0 1 0);
                }
            }
        }
    }
}

I've defined the cells for the Porous Medium using the command "topoSet" and defining the cellZone boundaries in the file "topoSetDict" in /case/system.



However, when running a test run with a simpleFoam case and measuring the pressure drop along the x-Axis in ParaView, I obtain just a deltaP of ~16, compared to the ~32 I should have according to the polynomial equation:

> a <- 0.48012
> b <- 5.57380
> v <- 4.2
> deltaP=a*v^2+b*v
> print(deltaP)
[1] 31.87928

I've also attached my complete case. Did I do anything wrong in calculating the D/F coefficients? Or is my case set up in the wrong way to verify the measured/simulated pressure drop across the screen? I appreciate any help

I've also read papers where the Porous-Medium / Darcy-Forchheimer-Equation was implemented using K (permeability) and Y (nonlinear momentum loss coefficient), but I don't know how to convert these values into D/F required by openFoam. Is there a way do to it and where could I find further information on how to do it?

[dewey]

Take a look to this file.

https://es.scribd.com/document/23868...orousInter-v11


The coefficient D specifies the viscous resistance , it is calculated as 1/K where k is the permeability, and Fij specifies inertial resistance, i dont know if you need the coeeficient F.

[sdfij6354]

Thank you for you answer, I will take a look at the document (need to sign up first though).
However, I'm wondering about D = 1/K. Doesn't depend D in some way also on the thickness of the porous media? Or is this irrelevant for OpenFOAM?

Since my K = (3.44*(10^-9)*(epsilon^1.6) with epsilon = screen porosity = 0.4 and hence K = 7.94062E-10, my D would be = 1259347462.
So I set
D = (1259347462 -1000 -1000) since the resistance is only in X-Direction and
F = (0 0 0).
This leads to a pressure drop of ~55 along the screen, which is still a bit off.

[dewey]

Take a look to this files, I hope this could help you.

It is irrelevant for OF. K is a resistance for the fluid.

I dont know if that is the way to do the resistance only in the X-direction, You could put the same value in the three directions, setting that it is a isotropic medium. Are you trying to do a 2D simulation? because if you want to do that, you only have to set the faces as empty.

I am working with porous media too, but I am not an expert, if I can help you in something, let me know.


https://www.dropbox.com/s/djktzs0umq...efano.pdf?dl=0

https://www.dropbox.com/s/ivb3igaj7o...r_v11.pdf?dl=0

https://www.dropbox.com/s/n127zo90so...eport.pdf?dl=0

https://www.dropbox.com/s/sxjj5hvu66j9gmd/leer.pdf?dl=0

[sdfij6354]

I have a question regarding to this paper:

https://www.dropbox.com/s/ivb3igaj7o...r_v11.pdf?dl=0

μ(kg·m−1·s−1) is defined as the "dynamic viscosity" - of air?
In my case, air is flowing through a tube with a netting in the middle. I want to implement this netting as my porous media.

I'm wondering, because I don't get feasible results using the equation for deltaPressure in the reference:

deltaPressure = (μ/k)*velocity

I have my permeability k calculated as 7.94062E-10. When assuming a dynamic viscosity of air at (μ) 20°C of 15.11*10^-6 m-2/s, I get unrealistic results for my pressure drop value. E.g. deltaPressure = 16897 with a velocity of 0.75 m/s, even though it should be around 4.5 according to my measurements.

[dewey]

Yes, it is the dynamic viscosity

You are trying to run your simulation with porousSimpleFoam right?

Do you know that this incompresible solver works with kinematic pressure ?

When I started, first of all I did the example of the page 73

https://www.dropbox.com/s/2ztsdtebjv...oleum.pdf?dl=0

and after i did an experiment for validate.

You should do that excercise and simulate to compare.

[sepp.zell]

Maybe you can also have a look at my comparison between Darcy's law and the OpenFOAM simulation.
porousSimpleFoam - comparison to Darcy's law

There it is shown that OpenFOAM might not work for flow through porous media. Maybe this is the same in your test case. I discussed this issue with the developers. In the moment there is no fix for it. One suggestion was to try different schemes.

You should also have a look at a plot for the velocity over the x-axis. There are some spurious oscillations over your porous netting. This seems to be the reason that the pressure drop is not computed correctly (see also here: https://bugs.openfoam.org/view.php?id=134).

[SebT]

Dear Alwin,

i looked a little bit into your problem and think i can solve some Problems. First of all you are calculating a regression curve with y-intercept. Since there is no pressure drop at 0 speed there should be none. Hence:

dp = a * v² + b * v

The Darcy-Forchheimer equation can be written as:

dp/dx = mu * d * v + 1/2 * f * rho * v²

with dx being the thickness of the porous medium.

Coefficient comparisson leads to following expressions for d and f:

f = (2 * a) / (rho * dx)
d = b / (mu * dx)

I attached a libre file to automatically calculate the coefficients from meassurments.I also set up a test case to check the values. When calculating the pressure drop with your settings I get a relative diviation regarding your measurments of 5.04 % for 7.4 m/s and 3.01 % for 4.3 m/s, which i consider completely ok. Maybe you forgot to multiply the pressure by the fluid density? Incompressible solvers in OpenFOAM use kinematic pressure pk which is defined as pk=p/rho. So to obtain static pressure you need to multiply with the fluid reference density.

I hope this helps with your Problem. If you need the test case let me know and I'll send it to you.

[svramana]

Originally Posted by dewey

Take a look to this files, I hope this could help you.

It is irrelevant for OF. K is a resistance for the fluid.

I dont know if that is the way to do the resistance only in the X-direction, You could put the same value in the three directions, setting that it is a isotropic medium. Are you trying to do a 2D simulation? because if you want to do that, you only have to set the faces as empty.

I am working with porous media too, but I am not an expert, if I can help you in something, let me know.


https://www.dropbox.com/s/djktzs0umq...efano.pdf?dl=0

https://www.dropbox.com/s/ivb3igaj7o...r_v11.pdf?dl=0

https://www.dropbox.com/s/n127zo90so...eport.pdf?dl=0

https://www.dropbox.com/s/sxjj5hvu66j9gmd/leer.pdf?dl=0

I am working on porous media on OpenFoam, i have a question about porosity and calculation of D and F coefficients. Can i have access to the above files ?

Reagrds,
S.V.Ramana

[deeptiof]

there are two coefficient D and F used in darcy forchhiemer equation for porous media modelling.
I have one doubt that why F value is set to zero for most of the cases??

[ombretta]

How did you find this relationship between porosity and permeability?
Thank you.

[west barkley]

Originally Posted by SebT

Dear Alwin,

i looked a little bit into your problem and think i can solve some Problems. First of all you are calculating a regression curve with y-intercept. Since there is no pressure drop at 0 speed there should be none. Hence:

dp = a * v² + b * v

The Darcy-Forchheimer equation can be written as:

dp/dx = mu * d * v + 1/2 * f * rho * v²

with dx being the thickness of the porous medium.

Coefficient comparisson leads to following expressions for d and f:

f = (2 * a) / (rho * dx)
d = b / (mu * dx)

I attached a libre file to automatically calculate the coefficients from meassurments.I also set up a test case to check the values. When calculating the pressure drop with your settings I get a relative diviation regarding your measurments of 5.04 % for 7.4 m/s and 3.01 % for 4.3 m/s, which i consider completely ok. Maybe you forgot to multiply the pressure by the fluid density? Incompressible solvers in OpenFOAM use kinematic pressure pk which is defined as pk=p/rho. So to obtain static pressure you need to multiply with the fluid reference density.

I hope this helps with your Problem. If you need the test case let me know and I'll send it to you.

Hi, could you please help me with this question. where are the dp values? where can i find them to feed into the table?