CFX: what is "A true volume-porous media model?"
 

Hi, all, I see "A true volume-porous media model" from the website: http://www.ansys.com/assets/brochures/cfx-11.pdf

Can anybody explain it for me? and I will be grateful if anybody can give me some materials about this model.

Regards, whiz

Re: CFX: what is "A true volume-porous media model
 

Hello whiz,

Before CFX 11, to model a porous media (like a screen plate or honeycomb), one would use a momentum-losses approach to account for pressure drop and deflection effects over a fluid sub-domain. This was achieved by defining a extra source term in the momentum equation, with help of loss coefficients (like the pressure loss coefficient, among others) within a given fluid sub-domain.

Now in CFX 11, there is a extra domain (other than fluid and solid) called "porous" which should be considered the preferred way to do the same thing as described above.

The details of this approach/model are described on "CFX-Solver theory manual". Basically, a generalized form of Navier-Stokes equation together with Darcy's law are solved over a given domain. Simple said, the Navier-Stokes equation are solved in a form which accounts for the volume porosity of the media and the pressure source is expressed in terms of the Darcy's law.

--Roberto

Re: CFX: what is "A true volume-porous media model
 

Dear Janny, Thank you very much for your reply. Do you mean the "A true volume-porous media model" is the porous-domain model which is parallel to fluid-domain and solid domain? I know the moment equation in porous media, and moment equation of clear fluid as well. But I modeled one simple case with both fluid-domain and porous-domain, I noticed the velocity is not continous at the interface of "fluid-porous"? I want to know why the velocity is not continous there and I also want to know the theory of "fluid-porous" interface. Thank you very much! Whiz

Re: CFX: what is "A true volume-porous media model
 

By "porous domain" I meant to say that CFX offers a formalism for fluid flow though porous media, including interface (zero thickness) boundary treatment.

This "discontinuity", or rather sharp variation, originates when considering interface treatment in the model. The previous models were not able to capture sharp gradients by sole using momentum sources.

The "true volume-porous" model uses a "double-node" approach at the porous interface, so to capture sharp pressure and velocity discontinuities that may occur. As far as I know, this "double-node" are really two nodes of the adjacent continuum elements that represent the potentials in the pore system on each side of the interface.

And as far as I understand, this "double-node" can account for both longitudinal and transversal pressure losses, if one need to model both (please, someone correct me if I'm wrong).

Additionally, the discretization of the pressure source in the "true volume-porous" model, on the interface, is spatially third-order accurate based on a "pressure redistribution term". The pressure redistribution term can produce spurious velocity fields, when using default Rhie Chow discretization. These wiggles may be greatly reduced by redistributing the body force with a discretization with reference on the porous drag source term.

Well, I really don't know about the specifics of CFX modeling for porous domain, more than what I've said.

--Roberto

Re: CFX: what is "A true volume-porous media model
 

Dear Roberto, I have one paper "Analysis of fluid flow and heat transfer interfacial conditions between a porous medium and a fluid layer", by B. Alazmi, K. Vafai. In this paper, the author sumed up there are 5 methods to treat the fluid-porous interface. And as I know, there is "channel effect" between porous media and a wall, many scientist attribute this to the variable porosity near the wall. And the velocity profile from the CFX simulation seems reasonable, but I can't get any theory behind the result. whiz

Re: CFX: what is "A true volume-porous media model
 

Dear friends,

can anybody explain me how to include the porous pressure drop, when the same porous domain treated as a heat source to?

Re: CFX: what is "A true volume-porous media model
 

would you please explain your problem in more detail? whiz

Re: CFX: what is "A true volume-porous media model
 

thanks for ur response whiz,

am doing simulation with tube bundles, where heat is removed and pressure drop occurs at the same bundles.so i model tube bundles as porous media and calculating quadratic resistance coefficient for a fixed pressure drop with out considering the heat transfer through bundles first.after obtaining the pressure drop through porous media,the heat source is supplied.now what is the problem is due to the heat transfer through porous,the pressure drop first i fixed is changed to a new value.but i don't want the drop to change.how can i get this by calculating the quadratic resistance with heat transfer effects. thanks in advance

Re: CFX: what is "A true volume-porous media model
 

"the pressure drop first i fixed is changed to a new value"

as I know, for porous media, you just add source term to moment equation to take account of the pressure drop. In CFX, you just input a few coefficient, from the coefficient you provide, CFX then calculate the pressure drop. Do you input pressure drop directly? and where?

By the way, I guess the pressure drop is caused by the change of material properties such as density and viscousity. Regards, Whiz

Re: CFX: what is "A true volume-porous media model
 

thanks whiz,

am not give the pressure drop as input directly.by giving the coefficient am obtaining the drop.when the source is not given as input the drop is matching however when source given as input drop is changed.

Re: CFX: what is "A true volume-porous media model
 

because of the fluid properties change with temperatrue.

Re: CFX: what is "A true volume-porous media model
 

The velocity is not continuous because the volume change also implies an area change at the interface. So, for equal mass flow rates in the open domain and the porous domain, the velocity has to go up in the porous media.

As explained by another poster, the interface is treated specially in CFX to allow this to happen discontinuously. Total pressure on side 1 and side 2 are assumed to be equivalent, accounting for the velocity change due to the flow area change.

Re: CFX: what is "A true volume-porous media model
 

Dear HekLeR: in the CFX-pre, I see "conservative interface flux" about mass and momentum and turbulence option for the "fluid-porous" interface boundary. Do you have any insight theory about this technique? Kindly regards, whiz

Porous
 

Does anyone has idea regarding the Natural convection in Porous media in ansy14? If you have links and pdf than please share it.
:).

What specifically are you looking for? There are lots of examples of porous flow and lots of natural convection, but not many of both I suspect.

Hi
 

Thank you for the reply Ghorrocks. Actually, I am looking for the Natural convection process that takes place in a porous media. If u have link or pdf just in porous flow beside natural convection than here is my ad- amarcheetri@gmail.com
Thanks

Why don't you just try running the case you are interested in? There should be enough info in the manuals to get you going.

thank you chris...I am going through the manual I have but it is straight forward...if you have proper pdf file regarding porous (in ansys) would you please send for me...thank you

Hello, can someone suggest options for introducing artifical compressibility to deal with this velocity change at the fluid-porous interface (in CFX)? My transient simulation begins to diverge at this point. Thanks!

Why would you want to do add artificial compressibility?

I thought it would stabilize the solution at the fluid-porous interface, because that's where it begins to oscillate and diverge.
But that was just a thought, I would be grateful for suggestions!

So far I thought of changing the under-relaxation parameters (which one?!), smaller time steps, better mesh quality at the interface.

Thank you in advance for your suggestions!

How is the flow around the interface?

Normal to the interface, or parallel to the interface?

In CFX, timestep is the "under-relaxation" mechanism. More information is needed to determine if you need under-relaxation or not.

Under-relaxing can solve any divergence problem to the point of not making progress during the iterations--> never converges but it does not diverges.

The motto in a CFD algorithm is to force/enable/enhance/drive towards convergence, not to prevent divergence.

Flow is normal to the porous domain and flowing into it. It is also a multiphase set up : Fluid A is present in all domains at initialisation, and Fluid B enters through the inlet at a constant mass flow rate. Both fluids are continuous, using VOF, mixture model. I'm using adaptive time steps (min time step is 10^-6 s). Mesh has a max skewness of 0.95.

The discontinuity seems to occur when Fluid B reaches the fluid-porous interface.

Is there an ideal mesh quality requirement for multiphase simulations? This setup for single phase, steady state converges fine.

Thank you!

Regarding mesh quality - The quality requirement is different for different simulations so it is not possible to give general answers. But every simulation will run better with better mesh quality. So time spent improving mesh quality is never wasted, even if the quality was pretty good to start with.

Pressure diffusion scheme - expert parameter
 

Can someone explain the effect of this setting? (more than what is mentioned in the documentation)

Not sure you want to apply a global parameter to solve a localized issue at a domain interface.

However, if you are willing to try another expert parameter, you could also try the following

porous cs linearization option = 1 or 2

Its default value is no-linearization as far as I know, and 1 and 2 are different strategies to improve convergence at porous domain interfaces.

Hope the above helps,

Not sure you want to apply a global parameter to solve a localized issue at a domain interface.

However, if you are willing to try another expert parameter, you could also try the following

porous cs linearization option = 1 or 2

Its default value is no-linearization as far as I know, and 1 and 2 are different strategies to improve convergence at porous domain interfaces.

Hope the above helps,

maarsalan_1@yahoo.com

The attached file has Foam type, Its porosity phi, df fibre diameter, dp pore diameter, Cf inertial coefficient, Kp permeability and more.

My question is that for a CFX input we need
Volume porosity which is phi,
Permeability is given Kp,
Resistance loss coefficient (need to be calculated as inertial loss coefficient is unit-less)
and interracial area density by formula = 6(1-phi)/particle diameter

My questions is:
1. how to calculate resistance loss coefficient (1/m) form inertial loss coefficient (unit-less).
2. The data is enough to calculate interfacial area density? as diameter of pore is given but not of solid converted into sphere..

When I was using ANSYS Fluent, there were problems so I switched to CFX also bcz my advisor knows CFX.

Anyway
1 Try using refine mesh near interface.
2 If there is no turbulence e.g Re is low then don't use any Turbulence model (Shear Stress Transport is good though) in solving scheme as it causes velocity-pressure coupling (idk what that is but my advisor told me).
3. Try structure mesh instead of unstructured. There can be comformality issue.