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

Porous domain in a flow field

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 18, 2009, 04:03
Default 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
rikio is on a distinguished road
Send a message via Skype™ to rikio
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.
rikio is offline   Reply With Quote

Old   August 18, 2009, 07:23
Default
  #2
New Member
 
Martin Heiser
Join Date: Apr 2009
Posts: 11
Rep Power: 8
mhsr is on a distinguished road
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
mhsr is offline   Reply With Quote

Old   August 18, 2009, 18:23
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is offline   Reply With Quote

Old   August 18, 2009, 21:08
Default
  #4
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 8
rikio is on a distinguished road
Send a message via Skype™ to rikio
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.
rikio is offline   Reply With Quote

Old   August 18, 2009, 21:19
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   August 19, 2009, 02:52
Default
  #6
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 8
rikio is on a distinguished road
Send a message via Skype™ to rikio
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.
rikio is offline   Reply With Quote

Old   August 19, 2009, 08:01
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is offline   Reply With Quote

Old   August 25, 2009, 22:39
Default
  #8
Senior Member
 
Rikio
Join Date: Mar 2009
Location: SH, China
Posts: 182
Blog Entries: 1
Rep Power: 8
rikio is on a distinguished road
Send a message via Skype™ to rikio
I am sorry for the late reply.
Thanks for your guidance very much, Glenn. And many thanks to all helpers.
rikio 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
flow thru porous media, PLEASE HELP Goker FLUENT 4 September 8, 2012 04:02
Porous Media coupled with internal flow Samuel Andrade FLUENT 2 August 26, 2012 09:43
initialize flow field with steady state solution holg FLUENT 0 July 13, 2009 17:10
Question for modelling flow in porous media legendyxg FLUENT 9 April 21, 2009 22:24
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51


All times are GMT -4. The time now is 22:27.