Learning Forum

[AlexC]

Hello,

I have a question about setting up the porous medium simulation in FLUENT. Below is a screen shot. There are two approaches to setup porous medium simulation. 

(1) Setup C1 and C2 based on S=C1*mu*v+C2*rho/2*v^2

(2) Set up C0 and C1 based on S=C0*v^C1

Is the "Fluid porosity" box an input only for the C0-C1 approach? Or is it an input for both approaches? 

 

Do I need to give the right porosity in "fluid porosity" box? I did a porous medium simulation with different fluid porosity. I didn't notice any effects. There is no "fluid porosity" in the formulation of source term S. So i don't understand how fluid porosity plays a role in the simulation.

 

Please let me know if you need any more information from me. 

Thank you.

Alex

[Karthik R]

Hello,

Yes, you are right. Porosity term does not get called in the definitions of both your resistances. 

However, porosity is used in the estimation of material properties for the porous cell zone. In addition to this, you have two types of formulations in Fluent - superficial and physical velocity. The physical velocity and superficial velocities are scaled using the porosity term.

Moreover, the porosity is used in the prediction of heat transfer in the medium and in the time-derivative term in the scalar transport equations for unsteady flow. It also impacts the calculation of reaction source terms and body forces in the medium. These sources will be proportional to the fluid volume in the medium. If you want to represent the medium as completely open (no effect of the solid medium), you should set the porosity equal to 1.0 (the default). When the porosity is equal to 1.0, the solid portion of the medium will have no impact on heat transfer or thermal/reaction source terms in the medium.

Please have a look at the following link: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/flu_ug/flu_ug_sec_bc_porous_media.html?q=porous%20media.

If you are looking for help on how to access this link, please look for instructions here. https://forum.ansys.com/forums/topic/how-to-access-the-ansys-online-help/

I hope this answers your question. 

Thank you.

Karthik

[AlexC]

Thank you Karthik! This helps a lot!