
[Sponsors] 
August 18, 2009, 05:03 
Porous domain in a flow field

#1 
Senior Member

Hi, All,
I am running a model consisting of two plates which sepatated for a distance, about 30mm. The upper plate is a solar panel that will absorb solar energy, and the lower plate is a netlike one where small holes on. I would like to get the flow field when the twolayer plates are in parallel with the wind, mainly on the flow rate through the space between plates. Porous model was used on the lower plate for problem simplifing, since the holes are too small and too many. A fluid domain was created and a submodel of the lower plate was specified to set porous loss. After setting heat fluxes on some walls to get the effects of radiation, a .def file created to run within CFXSolver. But an error occurs at iteration 3. ================================================== ==================== OUTER LOOP ITERATION = 1 CPU SECONDS = 2.141E+01   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  0.00  2.6E07  2.6E06  1.1E+04 F   VMom  0.00  5.2E10  1.9E08  8.8E+05 F   WMom  0.00  4.3E11  1.0E08  2.6E+10 *   PMass  0.00  9.6E11  3.1E09  9.5 4.5E+04 F  ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 2.5% of the faces, 3.2% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: Outlet.   The fluid name is: Air Ideal Gas.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  0.00  1.3E03  1.2E01  5.8 5.1E04 OK ++++++  KTurbKE  0.00  2.7E03  7.8E01  5.8 7.5E03 OK  EDiss.K  0.00  4.2E03  1.0E+00  7.5 7.6E03 OK ++++++ ++  Notice: The maximum Mach number is 1.369E+02.  ++ ================================================== ==================== OUTER LOOP ITERATION = 2 CPU SECONDS = 1.790E+02   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom 99.99  1.9E03  1.7E01  4.2E04 OK  VMom 99.99  2.5E03  1.6E01  4.0E04 OK  WMom 99.99  3.3E03  2.5E01  1.3E03 OK  PMass 99.99  5.2E06  9.1E04  9.5 7.6E01 ok ++++++ ++  ****** Notice ******   A wall has been placed at portion(s) of an OUTLET   boundary condition (at 10.9% of the faces, 17.2% of the area)   to prevent fluid from flowing into the domain.   The boundary condition name is: Outlet.   The fluid name is: Air Ideal Gas.   If this situation persists, consider switching   to an Opening type boundary condition instead.  ++  HEnergy  1.10  1.4E03  8.8E01  5.8 3.7E03 OK ++++++  KTurbKE  0.26  6.9E04  2.0E01  5.8 5.6E03 OK  EDiss.K  0.39  1.6E03  1.0E+00  33.8 7.3E08 OK ++++++ ++  Notice: The maximum Mach number is 5.623E+01.  ++ ================================================== ==================== OUTER LOOP ITERATION = 3 CPU SECONDS = 3.341E+02   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++ ++  ERROR #004100018 has occurred in subroutine FINMES.   Message:   Fatal overflow in linear solver.  ++ Rates of velocity and Pmass are 99.99 in iteration 2 which is abnormal. I can not figure out what is the evil, so beg for help here. Would some one give me some hints? Thank you very much. In addition, the inlet velocity is 3.5 m/s, and 0 Pa at outlet. Refernce pressure is set to 1 atm. Other surrounding surfaces are wallls. You can image that this twolayer plates were placed in a wind tunnel whose inlet & outlet boundary are set as mentioned above. Thanks for any information. 

August 18, 2009, 08:23 

#2 
New Member
Martin Heiser
Join Date: Apr 2009
Posts: 11
Rep Power: 13 
The steep rates of momentum and Pmass in your second iteration are not that abnormal if you start with automatic initialisation, which usually sets the velocity field to 0m/s as the initial guess. Since there is a lot of change in the values during the first iterations there's nothing wrong with those high rates. But they may give a hint that there's another problem.
The Mach number is quite high, are you sure about correct dimensions of geometry and boundary conditions? The message "A wall has been placed at portion(s) of an OUTLET" usually means that your 'wind tunnel' is too short to simulate a onedirectional flow free of backflow, which could be the reason for the solver to crash. Try to increase the length of your windtunnel at first. If that doesn't help you could set up an initial guess manuelly, e.g. set the velocity in the free flow of the windtunnel to 3.5m/s and in porous media to 0m/s 

August 18, 2009, 19:23 

#3 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,401
Rep Power: 127 
Hi,
Looks like you are using a compressible fluid. Why are you doing that? It sounds like an incompressible fluid, possibly with buoyancy if that is significant would be more appropriate. It will be much easier to converge. Glenn 

August 18, 2009, 22:08 

#4 
Senior Member

Thank you very much, Martin & Glenn.
Martin, I have tried manually setting initial condition to 3.5m/s, the same error came out. In addition, the rear length of the wind tunnel is about 4~5 times of the plate length in wind direction. In such a low speed, I think this is enough. Glenn, Yes, I am using Air Ideal Gas because buoyancy need to be taken into consideration. Surface temperature will be much higher than ambient temperature because of radiation. If Air at 25 Degree was used instead, there will be no density difference, also no buoyancy. If there is any misunderstanding, please feel free to correct. Thank you very much. 

August 18, 2009, 22:19 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,401
Rep Power: 127 
You don't need ideal gas to model buoyancy. As I recommended, use an incompressible fluid with buoyancy activated. This uses a bousinesq buoyancy force and is much easier to converge than a compressible gas. As long as you temperature range is not too large this approximation works very well.


August 19, 2009, 03:52 

#6 
Senior Member

Thank you, Glenn. I will try this configuration.
In addition, when I setting a porous loss, can I left the permeability and loss coefficient blank because I have no experimental data? Is there any difference by specifing the porous media as domain and subdomain? Many thanks for any help. 

August 19, 2009, 09:01 

#7 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,401
Rep Power: 127 
Hi,
If you don't know the resistance for the porous material then remove it completely. BUT  you should be able to work out an approximate resistance. If you assume it is made of zillions of little holes in a plate then you can assume each is a little oriface plate. The resistance of an oriface plate is well known (usually as flow rate v pressure drop at various Re numbers) and you can derive an approximate resistance of a perforated sheet from that. Glenn 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
flow thru porous media, PLEASE HELP  Goker  FLUENT  4  September 8, 2012 05:02 
Porous Media coupled with internal flow  Samuel Andrade  FLUENT  2  August 26, 2012 10:43 
initialize flow field with steady state solution  holg  FLUENT  0  July 13, 2009 18:10 
Question for modelling flow in porous media  legendyxg  FLUENT  9  April 21, 2009 23:24 
Problem with rhoSimpleFoam  matteo_gautero  OpenFOAM Running, Solving & CFD  0  February 28, 2008 07:51 