porous media convergence help
 

I'm simulating unidirectional flow through a porous media (a tube bank). I've estimated the intertial resistance coefficient in the direction of flow through the porous region to be on the order of 3.5e+06, and to constrain the flow to the direction of the tubes, i've set the inertial resistance in the other two directions to be 3.5e+08.

The flow seems to be acting the way i would expect it to, but I am having trouble getting my solution to converge. Does anyone have any suggestions on what i can do to help my solution converge?

Re: porous media convergence help
 

Start with laminar flow and then turn on turbulence if any...

Re: porous media convergence help
 

Hi Brian,

the coefficients seem to be viscous resistances not inertial. Could you please explain me how you calculate it?

Re: porous media convergence help
 

Gelisli, Thanks for the response. I thought the same thing about the resistance being more viscous rather than inertial. However, when using the viscous resistance, i was unable to restrict the flow to a single direction to simulate flow through a tube bank. These simulations yielded large swirling flows within the 'porous' tube bank... a kind soul on this forum pointed out a brief mention in the fluent help file on simulating tube banks and it suggests to neglect the viscous resistance factors and use only inertial. Seems strange, but it works to constrain unidirectional flow. As for estimating the coefficients: the fluent help file porous media section has some equations for estimating the viscous and inertial resistance coefficients for beds of packed particles. these equations are funcions of the particled diameter, and the void fraction of pourous region. I equated the surface area of the opening of one of my 'tube bank' tubes to the surface area of the gap between three theoretical particles. I used the diameter of these theoretical particles in the coefficient equations along with the actual calculated void fraction of my tube bank {oops, i just realized that i grossly underestimated the void fraction previously which now lower my inertial coefficient by several orders of magnitude, perhaps my convergence problem will go away now}

well i guess trying to explain your problem to someone else is the best medicine sometimes...

while i'm posing: does anyone know of a good way to estimate the inertial viscous resistance coefficients for a tube bank (other than experimentally)?

Re: porous media convergence help
 

Hi Brian,

The resistance coeficients for various geometries of grid banks, tube banks, and structures (of which a packed bed which you had used is one of the simplest) have been measured and correlated in several places. Probably the most extensive that I have seen is:

Flow Resistance: A Design Guide for Engineers I.E. Idelchik, July 1989

There also are some tabulations in various heat exchanger design handbooks and textbooks. One that I remember being particularly useful is in:

Adrian Bejan's "Convection Heat Transfer". There you will see an nice little explanation of the viscous and inertial resistance coeficients and how the relative importance changes with Reynolds number. This goes toward answering your question regarding the importance of the 2.

In my experience for most devices with tube banks and "normal fluids" ie air, water, steam, light hydrocarbons, etc the dominant effect is the inertial term. This would of course change for nano-scale devices or heavy oils, etc.

Best Regards,

Bak_Flow

Re: porous media convergence help
 

Hi Brian,

I have done several porous media calculations (not tube banks) using viscous resistance coefficients and it really works well. Actually I always use 1000 times larger coefficients for non flow directions and convergence never be a problem.

Regards,

Divergence
 

Hi,

I'm trying to set up a fairly basic 2D model of flow through a tube bank which I have modelled as a porous media. However as soon as fluent carries out 1 iteration the solution diverges rapidly. Could this be a problem with boundary conditions.

I am using ANSYS 14.0 with fluent as my solver. I have set the porous zone as a "porous jump" is this the correct way to approach the problem?