I am modelling a packed bed with cyllindrical extrudates as packing material.I want to use porous media for this. Its a two phase k-e model. I am having problems in defining direction vectors.Can some help me please.

A k-epsilon model will almost certainly give wrong results for packed beds with porosities under 0.9. None of the underlying assumptions (because cascading eddies not possible, eddy size is limited by pore size) of the k-e model are valid, or very limited valid. If effects like for example fluid dispersion are important you need to consider this, you cannot just use the model and assume the results will be correct.

Having that out of the way, what problems so you have with direction vectors?

Erwin, Thank you for your response. As i used k-e model for my earlier simulations with other models i go for the same in porous media too. so with your suggestion i will think over reconsidering my model. The problem which i am facing in defining direction vectors as it is a randomly packed bed with cyllindrical extrudates. I am finding it very difficult to have synchronization between resitence values and corresponding D.Vs. so i assumed a 1D model and specified Resitence values in only Z-direction(flow direction towards gravity). but still i am not getting satisfactory result.Am I right with this approach. your suggestion will do the great favor to me. Thank you

No, don't use a 1D resistance specification, the resistance should be equal in all directions. Use the Ergun equation to specify the values for alpha and C2, the Fluent manual shows exactly how to do that. I have had good results following this approach.

Erwin,

have you modelled dispersion in a packed bed - how did you do it???

I have been modelling packed beds with the Ergun equantion and porosity of around 30-50%. I find that a laminar flow is generally acceptable for my application and available data, though I have played around with the tubulence models. I don't like the FLUENT treatment - instead I use the k-e model with a source term from Ahohe, which had the effect of damping turbulence, to the extent that it no longer had any effect. I didn't implement the second source term, which was for the inertial term and does have the capability to enhance turbulence .... it looks too difficult to implement in FLUENT easily.

Since in some apps I have natural convection in a void space together with the packed bed, I use the k-e model and apply the damping term and a zero turbulent viscosity in the porous zone (making it laminar) and have the standard k-e model in the void zone (where its turbulent). This works well (although convergence of the coupled system is tricky).

I am interested in modelling dispersion efffects in 2D/3D in packed beds and haven't come up with a good approach for doing so as yet. Any ideas? References??

Thanks

Greg

hi If I am right you are trying to simulate trickle bed using porous media. As the flow in trickle bed always remains laminar why you are using k-e model.I think you actually mean k-fluid(Eulerian) model. Is it so?

I looked into it briefly a while ago and found two articles that may contain interesting approaches:

Turbulence Model for flow through porous media - T. Matsuoka and Y. Takatsu - Int. J. Heat Mass Transfer, Vol.39, No 13, 1996

A general two-equation macroscopic turbulence model for incompressible flow in porous media - B. Antohe, J. Lage - Int. J. Heat Mass Transfer, Vol.40, No 13, 1997

I never got around to implementing anything in Fluent.

Hope it helps, good luck.

Thanks Erwin

..I have the paper by Antohe and used their source term in my FLUENT implementation described above.As I said there I found that model essentially made my porousmedia macroscopically laminar as well.

I'll look up the other paper, thanks.

Greg

dear erwin, Thanks for your coperation and valueable suggestions. as per your suggestion i tried out the isometric 3d model, i give the same resistence values in all dimensions and i tried this for both k-e as well as laminar model. but i am not getting the results. it is showing a 100% reverse flow at centre and looking like fluid is being circulated inside the bed. I dont know where the mistake is. to choose the direction vectors i use plane tool in YZ plane where Z is vertically downwrad. can you help me regarding how did you go for choosing DVs. may it is the point of my mistake. plz help. thanking you

Hi pravesh, i have learnt about UDFs and just tried to include the drag coefficient through UDF. i tried the example given in Fluent UDF manual. Its getting compiled but as i specify in the phase interaction panel the fluent gives an error Error: Set_Property: null user-defined-function name Error Object: ()

How did you used your UDFs??

For a packed bed you don't need to change the default direction vectors because the hydraulic resistance is isotropic. The default direction vectors are 1,0,0 for vector 1 and 0,1,0 for vector 2. This means that the default vectors are the standard cartesian coordinates. So change those vectors back to these values and enter the same inertial and/or viscous coefficient for all three direction vectors. If you then still find a recirculation area then that might be caused by your mesh/model.