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

porosity

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 3, 2005, 04:46
Default porosity
  #1
Giorgio Crasto
Guest
 
Posts: n/a
I'm using the porosity functions VPOR and EPOR, HPOR and NPOR to simulate a 3D windbreak, a canopy. I'd like to know if the velocity calculated by the Phoenics's solver is a Darcy velocity or a seepage velocity (real velocity but spatially averaged).

regards,

Giorgio
  Reply With Quote

Old   June 16, 2005, 12:15
Default Re: porosity
  #2
mick
Guest
 
Posts: n/a
All the VPOR,HPOR etc do is to reduce vol/area etc, therefore flow will accelerate over these cells if fraction < 1 and > 0.

There is no in built resistance, you will have to put this in yourself, or through using plate object in the VR-Editor with the menu chosen resistance.

I have no idea what darcy/seepage terminology means, but now you know what VPOR HPOR do !--Volume / Area reduction.
  Reply With Quote

Old   July 12, 2005, 15:43
Default Re: porosity
  #3
Steven Beale
Guest
 
Posts: n/a
I believe the writer wishes to know what the independent terms and also what the convection coefficients are in the momentum equations; namely if they are U1, V1,.. or , VPOR*U1 etc. The first is based on the pore or interstitial velocity and the latter is a filter or superficial velocity (smaller).

There are several possibilities but turning on the porosities is equivalent to the independent values ('convected' velocities) being interstitial values and the convection fluxes ('convecting' velocities) the superficial values. (You can also imagine the convection fluxes to be superficial and the values to be interstitial if you like)...
  Reply With Quote

Old   August 21, 2005, 05:52
Default Re: porosity
  #4
mick
Guest
 
Posts: n/a
Thanks for that Steven, maybe you could help me further. I am about to do a consultancy where I plan to use a sub-model to determine a pressure drop across a complicated grill arrangement. I will calculate the DP's from varying velocity profiles and put a suitable resistance 'curve' into the full model from the results of this sub model. Of course In the fuller model I will not representing the complexity of the grille.

In this case I will not be changing porosities as I do not see that I need to.

I can imagine that another approach might be to use porosities to represent the flow free-volume and apply a suitable resistance, (which would be different to the above resistance in that it would somehow take into account the reduced volume). This resistance I have in the back of my mind as being called a darcy resistance.

I imagine that this type of information comes from engineers tables/handbooks, and would be an approximation related to different types of say grille or porosity structures but I have not 100% certain.

So my question is what are the pros and cons here? is it just that the second method would save you from doing the sub-model, that is if you could get some suitable resistance formula from a text. And is there a definitive reference to this.

  Reply With Quote

Old   August 21, 2005, 17:59
Default Re: porosity
  #5
Steven
Guest
 
Posts: n/a
Mick:

You're absolutely right that you do not need to change the porosity. This is one of the 'other' formulations mentioned in the previous note. We've done it, and it works provided either the whole region is the same and/or the porous region is sufficiently impermeable that only the source (Darcy resistance) and pressure gradient terms are important in the momentum equations (potential flow). Under these circumstances both 'convected' and 'convecting' velocities are the superficial values and the effect is to multiply each and every term in the momentum equations with 1/porosity, ie all the forces are bigger by the same amount. This is essentially the formulation given in the original paper by Patankar and Spalding on the distributed resistance analogy (DRA).

The problem is that if, say, only part of the domain contains the porous media (as in your case) the above formulation renders a force balance which is inconsistent between the fluid/porous-fluid zones (and similar errors in the energy/species equations). Under these circumstances I would set the porosities to the fluid volume fraction.

In general the DRA will usually work well when there are two distinct lengths scales ie the bodies which are being volume averaged are small in comparison to the main flow regime (grid), and also when the "Darcy" resistance is isotropic with respect to flow direction. I have heard of situations where the DRA generates significant errors, and others where it is quite realistic.

You might get something from the paper by Beale and Zhubrin in the June edition of Numerical Heat Transfer-B (e-mail me your address and I can send you a copy)

You should try and get your drag data from experiments if at all possible. If not do a detailed simulation as per your posting.

Hope this helps

Steven

  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
UDF for porosity cfd-novice FLUENT 2 August 20, 2009 03:19
porosity ravi FLUENT 2 December 13, 2007 21:50
porosity ravi FLUENT 0 December 13, 2007 02:31
help on porosity ravikanth FLUENT 0 January 21, 2005 13:14
Help on porosity Leon Mills Phoenics 1 June 18, 2002 08:59


All times are GMT -4. The time now is 12:21.