# Help :Porous media flow

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 22, 2001, 11:46 Help :Porous media flow #1 Wole Guest   Posts: n/a Dear CFX users, I wonder wether anyone is well aquainted enough with porous media flow to give me advice on this. I am trying to simulate 2-D axisymmetric free surface flow on a porous substrate using CFX4.4 and run into huge problems so far... Also does anyone know anything about specifying resistances for porous flows apart from the normal volume porosity quantity. I would be very grateful for any advice, this is really doing my head in . Cheers.. Wole

 August 26, 2001, 22:34 Re: Help :Porous media flow #2 S. H. Kim Guest   Posts: n/a I had similar problems before. One of my colleagues told me the solution. "You can obtain the required pressure drop by specifying R_c or R_f to the porous region. The volume porosity does not induce the pressure drop during the calculation when you use R_c or R_f in the body force section." Good luck. S. H. Kim

 August 27, 2001, 05:14 Re: Help :Porous media flow #3 Tadiwos Guest   Posts: n/a Kim, I am interested on your reply to Wole, but what does it mean R_c or R_f?

 August 27, 2001, 07:45 Re: Help :Porous media flow #4 S. H. Kim Guest   Posts: n/a Tadiwos, You can find the details at 'Physical models and fluid properties, BODY FORCES' in the Solver manual. Briefly, the body force term in the momentum equation is written as B=B_F-(R_C+R_F |V|)V. To check the effect of volume porosity and R_c to the pressure drop, I had performed a series of tests for this. The geometry is a 15-m long rectangular duct with a 0.1mx0.1m crosssection. The working material is water. The porous media region is exist at the last 10m. The inlet condition is given as 1m/sec uniformly. The results are 1) Volume porosity 1.0 : dp=1.44Kpa 2) Volume porosity 0.5 : dp=5.41Kpa 3) Volume porosity 0.5 and R_C=1000 : dp=20.78Kpa If R_c term is induced the pressure drop, dp = R_c X V X L = 1000 X 2 X 10 = 20000Pa=20.0Kpa From these crude tests, I concluded that the pressure drop by volume porosity disappeared when the body force command is specified in that region. S. H. Kim

 August 27, 2001, 07:46 Re: Help :Porous media flow #5 Wole Guest   Posts: n/a Thanks Kim for your advice. I understand the Keywords R_c and R_f to be the resistant constant and Resistant speed factor respectively. Do you have advice as to how to specify them (i.e what their magnitudes should be) as CFX documentation seems to leave us completely in the dark about this Cheers Wole

 August 27, 2001, 20:00 Re: Help :Porous media flow #6 S. H. Kim Guest   Posts: n/a Wole, T. hohne applied the porous approach in the paper, 'Coolant mixing in pressurized water reactors' that is found in technotes of CFX community. He suggested that R_F=\zeta \over{A}{V} \over{\rho}{2} where zeta is the flow resistance coefficient, A the crosssectional area, V the volume. If zeta is constant, you can use this equation. If not, I don't have idea right now. Good luck S. H. Kim

 August 30, 2001, 12:17 Re: Help :Porous media flow #7 Wole Guest   Posts: n/a Thanks Kim, Although the said paper does not seem to exist on the site anymore although I found another paper by T. Hoehne titled "Numerical investigation of the coolant mixing during fast deboration transients in konvoi type reactors" which says nothing about resistances. I could locate the paper through CFX though. Meanwhile, your message explained how to specify R_f (Resistant speed factor). At the moment I'm more concerned about R_c (Resistant constant). Have you got info on this as well?.

 August 30, 2001, 20:32 Re: Help :Porous media flow #8 S. H. Kim Guest   Posts: n/a Wole, One of my colleagues specified R_c by dp/V_avg, where V_avg is the average normal velocity in the porous media and dp the intended pressure drop, R_f=0. Good luck. S. H. Kim

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Axius FLUENT 2 August 7, 2014 10:34 JoFFe CFX 2 November 1, 2010 04:50 lee CFX 3 August 31, 2007 01:12 Nirmal Kumar Pathak Siemens 8 November 23, 2005 07:18 Desheng Kong Main CFD Forum 3 December 19, 2000 11:07

All times are GMT -4. The time now is 10:24.

 Contact Us - CFD Online - Privacy Statement - Top