# Porous domain in a flow field

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

 August 18, 2009, 04:03 Porous domain in a flow field #1 Senior Member   Rikio Join Date: Mar 2009 Location: SH, China Posts: 182 Blog Entries: 1 Rep Power: 8 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 net-like one where small holes on. I would like to get the flow field when the two-layer 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 CFX-Solver. But an error occurs at iteration 3. ================================================== ==================== OUTER LOOP ITERATION = 1 CPU SECONDS = 2.141E+01 ---------------------------------------------------------------------- | Equation | Rate | RMS Res | Max Res | Linear Solution | +----------------------+------+---------+---------+------------------+ | U-Mom | 0.00 | 2.6E-07 | 2.6E-06 | 1.1E+04 F | | V-Mom | 0.00 | 5.2E-10 | 1.9E-08 | 8.8E+05 F | | W-Mom | 0.00 | 4.3E-11 | 1.0E-08 | 2.6E+10 * | | P-Mass | 0.00 | 9.6E-11 | 3.1E-09 | 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. | +--------------------------------------------------------------------+ | H-Energy | 0.00 | 1.3E-03 | 1.2E-01 | 5.8 5.1E-04 OK| +----------------------+------+---------+---------+------------------+ | K-TurbKE | 0.00 | 2.7E-03 | 7.8E-01 | 5.8 7.5E-03 OK| | E-Diss.K | 0.00 | 4.2E-03 | 1.0E+00 | 7.5 7.6E-03 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 | +----------------------+------+---------+---------+------------------+ | U-Mom |99.99 | 1.9E-03 | 1.7E-01 | 4.2E-04 OK| | V-Mom |99.99 | 2.5E-03 | 1.6E-01 | 4.0E-04 OK| | W-Mom |99.99 | 3.3E-03 | 2.5E-01 | 1.3E-03 OK| | P-Mass |99.99 | 5.2E-06 | 9.1E-04 | 9.5 7.6E-01 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. | +--------------------------------------------------------------------+ | H-Energy | 1.10 | 1.4E-03 | 8.8E-01 | 5.8 3.7E-03 OK| +----------------------+------+---------+---------+------------------+ | K-TurbKE | 0.26 | 6.9E-04 | 2.0E-01 | 5.8 5.6E-03 OK| | E-Diss.K | 0.39 | 1.6E-03 | 1.0E+00 | 33.8 7.3E-08 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 P-mass 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 two-layer plates were placed in a wind tunnel whose inlet & outlet boundary are set as mentioned above. Thanks for any information.

 August 18, 2009, 07:23 #2 New Member   Martin Heiser Join Date: Apr 2009 Posts: 11 Rep Power: 8 The steep rates of momentum and P-mass 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 one-directional flow free of backflow, which could be the reason for the solver to crash. Try to increase the length of your wind-tunnel 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 wind-tunnel to 3.5m/s and in porous media to 0m/s

 August 18, 2009, 18:23 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,805 Rep Power: 85 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, 21:08 #4 Senior Member   Rikio Join Date: Mar 2009 Location: SH, China Posts: 182 Blog Entries: 1 Rep Power: 8 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, 21:19 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,805 Rep Power: 85 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, 02:52 #6 Senior Member   Rikio Join Date: Mar 2009 Location: SH, China Posts: 182 Blog Entries: 1 Rep Power: 8 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, 08:01 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,805 Rep Power: 85 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

 August 25, 2009, 22:39 #8 Senior Member   Rikio Join Date: Mar 2009 Location: SH, China Posts: 182 Blog Entries: 1 Rep Power: 8 I am sorry for the late reply. Thanks for your guidance very much, Glenn. And many thanks to all helpers.

 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 Goker FLUENT 4 September 8, 2012 04:02 Samuel Andrade FLUENT 2 August 26, 2012 09:43 holg FLUENT 0 July 13, 2009 17:10 legendyxg FLUENT 9 April 21, 2009 22:24 matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51

All times are GMT -4. The time now is 20:08.