Dear Ms. Maria

I am confusing and miss understanding with your problem. If the flow is in radial direction, it is not called an annular flow. Because in an annular cylinder , the flow should be in axial direction and flows between two concentric cylinder.   Please let me  understand properly your physical problem first.

Maria,

From your description, it sounds like your problem is not only anisotropic but also heterogeneous, i.e. varying with position as well as direction.  If this is the case, I believe that your only option is to write a UDF to assign the permeabilities as a function of R, Theta, and Z.

Dear Nouri-Borujedi, 

the device i want to simulalate the flow through, is composed by different parts. it is composed by an external cylinder with an inlet on the top, an internal fiber bundle(annular cylinder), and an outlet on the bottom side of the external cilinder. the fluid entering through the inlet is deviated and passes through the fiber bundle. So the flow has more than one direction. In fluent I'm considering only the fiber bundle as a porous medium.

Thanks!

Dear Jeremy,

the fiber bundle is made by different layers of fibers; every concentric layer is made by parallel fibers, with a certain angle of inclination. Passing from one layer to the next one the angle inclination is reversed. so varying the position, the "texture/structure" of the fiber is the same, but depending on how the fluid enter the bundle (so depending on the direction of the fluid) the permeability is different. I'm considering the fiber bundle making the assumption of porous medium because to simulate and reproduce the real geometry of the bundle requires too much computational effort. 

I have also thought to assign the permeability as a function of R, theta, and Z, but this means that I have to work with a spherical coordinate system. in this case I think that I should consider the entire problem with spherical coordinates, also solving the navier stokes equation in spherical coordinates. Should I write an Udf to solve the navier stokes equation (including the source term to consider the perous medium) in spherical coordinates?

Thanks a lot!

Hi Maria,

I have worked on a similar kind of problem, only difference is that I didn't use cylindrical/conical coordinates for defining permeability. I am not sure whether this will work with cylindrical coordinate system, but the way you want to define permeability, you need to define it as a tensor. Now, the thing is Fluent doesn't allow you to do it directly through its interface, so you need to define three UDFs using macro DEFINE_SOURCE, each UDF for each direction. As an example, something like this for radial direction:

DEFINE_SOURCE(radial_source, c, t, dS, eqn)

{

radial_source = -(Dr*mu*Ur + Drtheta*mu*Utheta + Drz*mu*Uz)

dS[eqn] = -(Dr*mu)

}

similarly for theta and z direction. And then insert this UDF in the source of momentum equations. 

Hopefully this helps, and let me know if it helps.

Maria,

Can you provide a diagram of your flow domain?  From your description, it sounds like you are using a 3D domain and the permeability is assumed to be circumferentially homogenous but unknown.  Do you expect flow in the circumferential direction or is it purely radial-axial flow?

My previous comment concerning the UDF was simply to assign the permeability:

K1=function1(x,y,z)

K2=function2(x,y,z)

which would then be linked to the viscous resistances via the drop-down boxes to the right.

Possibly what you need to do is to consider a coordinate transformation:

http://petrowiki.org/Diagonalizing_the_permeability_tensor

But since your geometry is 3D and circumferentially homogeneous, you would need to assign the principal directions (Direction Vectors) and permeability components (Viscous Resistance) using a UDF as above.  This would allow you to have just the radial-to-axial angle dependence.

Disclaimer: I have never tried this specific approach.

If the flow is essentially 2D (radial-axial), then you can directly model the coordinate transformation in FLUENT without a UDF.  This is accomplished by choosing the Direction-1 Vector to align with your principal permeability direction.

hi Bachchan,

thanks for your answer!  is it correct to add these UDFs in the x,y,z momentum source writing them in terms of R, theta, and z? Should I set something on fluent to work in spherical coordinates?

In the case that I can do this, is it possible to pass in the UDF just for theta a variable for the permeability that is a function of theta?for R and z the permeability is constant.

Thanks!

Hi Jeremy, 

thanks for your interest. I've attached a drawing of the device, hope it is helpfull. the flluid flows in the inlet and thanks to the flow diverter (it is just a cylinder with a conical shape on the top) it is deviated to pass through the bundle and exits at the bottom through the windows that are opened. when you talk about assigning the direction vectors, do you mean that I should assign direction vector for R, theta and z ? in this case the value for the permeability would be constant for R and Z, and a function of theta for the theta component. Can I work in fluent with x y z coordinate system and write a UDF considering r theta and z? 

Maybe I have misunderstood what you wrote me, How should i write a UDF to consider the radial -axial dependence?

Thanks a lot!

Hey Maria,

We can transform those UDFs to Cartesian coordinates and then we can hook them with X, Y and Z momentum. But, wait !! Here is the thing :According  to your diagram and fluid flow pattern, I am under the impression that your fiber bundle is cylindrical, in which case you don't need a conical coordinate system, you can just work with cone half angle as zero which makes it a cylinder, and when you go with cylindrical coordinate system there is no need of theta and r, and therefore there is no need of UDF. So just enable conical in fluent, define your axis direction vector and define permeability values for direction 1,2 and 3, where direction-1 permeability will be axial permeability, direction-2 permeability will be radial direction permeability and direction-3 permeability will be circumferential permeability.

Also. correct me if I am wrong, and send a better picture defining how you are considering your theta to define your permeabilities and why.

Hi Bachachan,

yes you are correct, and I was already working with 0° using the conical coordinate system, so the system is cilindrical. the problem is that I don't have the permeability along the circumferential direction. what I have is the value for the permeability in axial direction (thinking about this axis as at 0°), the premeability for the radial direction (so it is the permeability at 90° with respect to the axial one), and two other values respectively for a direction of 30° and 60° with respect to the axial direction. So my values are just in the plane given by the axial and radial direction. I was wondering If I can use these values (without the circumferential one) to characterize the porouse zone. If I don't specify the value in the circumferential direction how does fluent consider the flow in that direction?

Thanks!

Hey Maria,

I have two points here :

1. For the solution point of view 30 deg and 60 deg permeability values are not required for a cylindrical fiber bundle (as far as i understand the problem), you need to provide axial, radial and circumferential permeability only. But, in your case the flow is axisymmetric, so even if you don't have a value for circumferential permeability, just use some default value closer to radial or axial permeability, because due to axisymmetry there won't be much circumferential movement of fluid in fiber bundle, and therefore it won't affect your solution.

2. If you want to define it more accurately, you can define all 9 components of permeability tensor through UDF, which will take into account of the permeability in all possible directions. But, in your case you have only radial and axial permeability, so you can just proceed with the first point.

Hi Bachchan,

I agree with you. I was also thinking about neglecting the circumferential movement of fluid. I will try to set both permeability close to 0 and close to an other direction(radial or axial as you told me) and see what change.

Thanks a lot!