# Porous zone input

 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 11, 2007, 08:29 Porous zone input #1 Jonathan Guest   Posts: n/a Hi... Can anyone help me to input values( viscous and inertial sink terms) in porous zone. I have pressure drop and velocity values with me. I have calculated '1/alpha' and 'C2' values. But I do not know how to input these values into FLUENT. It asks for direction vectors. My porous zone is in X direction. are these inertial and viscous resistances really '1/alpha' nd 'C2'. How to input these values in different directions. Can anyone help. My data doesn't allow me to use Power law model. Jonathan

 January 11, 2007, 11:04 Re: Porous zone input #2 Hugo Guest   Posts: n/a Hi Viscous resistance is the 1/alpha number (make sure you've got your value in units of 1/m2) and inertial resistance is th C2 value (again, make sure you've got units of 1/m), both of whih you put in the define/boundaryconditions/fluid/porous box. Concerning directions: is your model 2D or 3D? and is the resistance to flow the same in all directions (isotropic)? If it is isotropic, then you put the same value in all of the viscous resistance boxes, and the same value in all of the inertial resistance boxes. Hope that helps, Hugo.

 January 12, 2007, 02:59 Re: Porous zone input #3 Jonathan Guest   Posts: n/a Thanks Hugo... My model is 3D. And I have porous media thickness in X-direction of the model. My model is anisotropic. And i have higher resisitence in -direction. But i dont know what valus to give for Y and Z directions. But I'm confused about how to define these direction vectors. (esp 1,0,0.. 0,1,0 thing)... And i check my convergence with respect to the mass flow at outlet. Is it correct..?

 January 12, 2007, 04:39 Re: Porous zone input #4 Hugo Guest   Posts: n/a You've got a 3D case, so you only need to define two (perpendicular) direction vectors (the other is perpendicular to both the other two). Inputs for direction vectors: let the first be the x-direction so the inputs are x=1, y=0, z=0; let the second be the y-dirN so the inputs are x=0, y=1, z=0. You have mesured p and q for the x direction, and reduced the data to get 1/ALFAx and C2x. Those go in viscous resistance direction-1 and inertial resistance direction-1. To get 1/ALFAy, 1/ALFAz, C2y and C2z you will wither have to guess given the degree of anisotrpopy of your porous medium and the values for x-direction, or measure p-Q curve for a sample of the medium in ythe y and z directions. Up to you. What's the application? Checking the convergence against flow rate depends on what's important to you, but yes, seems like a vaguely sensible thing to do. Good luck and let us know how you get on, Hugo.

 January 12, 2007, 05:19 Re: Porous zone input #5 Jonathan Guest   Posts: n/a Thanks Hugo. The application is a heat exchanger... Where i make a porous assumption for the cross baffles. I dont understand what is 'Q' in what you have mentioned. what is P-Q curve. All I have is pressure drop to velocity data...DeltaP- V curve. As said in Fluent user guide, I have fit a trend line and got an equation from which I derived 'C2' & '1/Alpha' by equating coefficents with the general momentum sink equation. Incase Q is discharge, then i think my approach is similar to what you said. My references are Fluent 6.2 user guide Chapter 7.19. Is the approach correct. As you said last time, the I'm quite confused with the units of '1/alpha' and 'C2. Your suggestions have really helped me.

 January 12, 2007, 06:27 Re: Porous zone input #6 Hugo Guest   Posts: n/a sorrry - Q is for flow - so you were correct. Good luck, H.

 January 12, 2007, 08:09 Re: Porous zone input #7 Jonathan Guest   Posts: n/a Hi hugo... Your inputs were of great help.. Now I have cleared myself from my doubts on units as well. Now my basics are right. Thank you very much. Jonathan

 January 13, 2007, 01:42 Porous zone input properties #8 Yashodhan patil Guest   Posts: n/a I am doing analysis of air passing through porous media, one is Polyeurethane foam and other is polyfiber. My model is 3D. I am not getting the properties of the Polyeurethane foam & polyfiber such as Power law model values(C0,C1), direction vectors, viscous & inertia resistance which are required to define the porous zone boundary condition in FLUENT.

 January 22, 2007, 01:41 Re: Porous zone input properties #9 Jonathan Guest   Posts: n/a Sorry Yashodan for a delayed response... In fluent you have to specify the porous zone properties by either by Power law model/ Coefficients of inertial and viscous resistances. These values are derived from experimental data. And they are material properties. You can get them from internet if you do not have an experimental data. I'm not aware of the materials you talk about. Regarding direction vectors. These depend on direction of orientation of the porous media in your model. For example if ur porous media is oriented in 45 degrees towards X,Y and Z, you give inputs as 0.707 on all directions. Since you have 2 direction vector inputs, the third is automatically aligned perpendicular to both the vectors...and resistances are given with respect to each direction which you get from ur material properties. Hope you get it...

 January 23, 2007, 05:23 Re: Porous zone input properties #10 Jonathan Guest   Posts: n/a If you are not aware of material properties, ask a manufacturer of the product about permeability and porosity. Or do some experimental investigation. Like testing to find pressure drop with respect to the flowrate.

 June 26, 2010, 14:31 #11 Senior Member   MASOUD Join Date: Mar 2009 Posts: 102 Rep Power: 10 Hi Hugo, Do you mind if I ask you for a couple of questions regarding porous media set-up in Fluent? Masoud

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post tanjinjack FLUENT 2 September 26, 2016 04:10 Tarak OpenFOAM 6 September 9, 2011 17:51 lig FLUENT 0 April 26, 2010 00:47 csvirume FLUENT 2 September 9, 2009 01:08 Karl Kevala FLUENT 4 February 21, 2001 16:52

All times are GMT -4. The time now is 18:43.