CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Porous zone input

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 11, 2007, 08:29
Default 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
  Reply With Quote

Old   January 11, 2007, 11:04
Default 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.
  Reply With Quote

Old   January 12, 2007, 02:59
Default 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..?

  Reply With Quote

Old   January 12, 2007, 04:39
Default 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.
  Reply With Quote

Old   January 12, 2007, 05:19
Default 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.
  Reply With Quote

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

Old   January 12, 2007, 08:09
Default 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

  Reply With Quote

Old   January 13, 2007, 01:42
Default 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.

  Reply With Quote

Old   January 22, 2007, 01:41
Default 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...
  Reply With Quote

Old   January 23, 2007, 05:23
Default 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.
  Reply With Quote

Old   June 26, 2010, 14:31
Default
  #11
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 9
MASOUD is on a distinguished road
Hi Hugo,
Do you mind if I ask you for a couple of questions regarding porous media set-up in Fluent?
Masoud
MASOUD is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Modelling Combustion in Porous Zone tanjinjack FLUENT 1 August 31, 2015 04:56
Problem in running ICEM grid in Openfoam Tarak OpenFOAM 6 September 9, 2011 17:51
Need help!:Particle flow through porous zone lig FLUENT 0 April 26, 2010 00:47
Problem in IMPORT of ICEM input file in FLUENT csvirume FLUENT 2 September 9, 2009 01:08
Sliding mesh error Karl Kevala FLUENT 4 February 21, 2001 16:52


All times are GMT -4. The time now is 13:23.