CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

hotRoom tutorial with atmosphere boundary condition

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

Like Tree1Likes
  • 1 Post By Toorop

Reply
 
LinkBack Thread Tools Display Modes
Old   May 25, 2012, 09:51
Default hotRoom tutorial with atmosphere boundary condition
  #1
Member
 
Tibor Nyers
Join Date: Jul 2010
Location: Hungary
Posts: 91
Rep Power: 6
Toorop is on a distinguished road
Hi,

I would like to specify atmosphere boundary condition in the hootRoom tutorials. The default case uses walls on the sides and at the top, so the only modification is the change in boundary conditions.
Code:
alphat
{
        type            calculated;
        value           uniform 0;
}

epsilon
{
        type            inletOutlet;
        inletValue      uniform 0.01;
        value           uniform 0.01;
}

k
{
        type            inletOutlet;
        inletValue      uniform 0.1;
        value           uniform 0.1;
}

kappat
{
        type            calculated;
        value           uniform 0;
}

nut
{
        type            calculated;
        value           uniform 0;
}

p
{
        type            calculated;
        value           0;
}

p_rgh
{
        type           totalPressure;
        p0              uniform 0;
        U               U;
        phi             phi;
        rho             rhok;
        psi             none;
        gamma      1;
        value         uniform 0;
}

T
{
        type            inletOutlet;
        inletValue      uniform 300;
        value           uniform 300;
}

U
{
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
}
Unfortunately, the BC that I set is not giving me the results I'm looking for. The air won't exit the domain in the upward direction as expected, it makes an U shape path (picture attached). The solvers were buoyantBoussinesqPimpleFoam and buoyantBoussinesqSimpleFoam.

It would be great if someone could share his setup to achieve correct behaviour at the boundary. Thanks!
Attached Images
File Type: png stream.png (50.9 KB, 109 views)
Attached Files
File Type: gz hotRoom_Simple_atm.tar.gz (3.2 KB, 21 views)
Toorop is offline   Reply With Quote

Old   May 25, 2012, 12:26
Default
  #2
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 10
MartinB is on a distinguished road
Hi,

you can try as BC for both p_rgh and U:
Code:
ceiling
{
      type zeroGradient;
}
Martin
MartinB is offline   Reply With Quote

Old   May 29, 2012, 06:13
Default
  #3
Member
 
Tibor Nyers
Join Date: Jul 2010
Location: Hungary
Posts: 91
Rep Power: 6
Toorop is on a distinguished road
Hi,

thanks for the tip. With the modifications the case produces a nice expected outflow in the early stages of the simulation. But then a crossflow develops across the domain - with both solvers. I think the pRefCell / pRefValue "hijacks" the flow - with the original BC there was no need for pRef. Any ideas how to overcome this situation?
Attached Images
File Type: png stream_zG.png (29.0 KB, 76 views)
Toorop is offline   Reply With Quote

Old   May 31, 2012, 10:50
Default
  #4
Member
 
Tibor Nyers
Join Date: Jul 2010
Location: Hungary
Posts: 91
Rep Power: 6
Toorop is on a distinguished road
Hi,

I have managed to solve the problem!

The combustion/fireFoam/les/smallPoolFire cases uses the boundary conditions I wanted to create, so I just copied and modified it to adjust to the buoyant solvers. I really don't now how on earth I couldn't find it sooner ...

Of course if anyone has some suggestion, please share it! Thanks.
Attached Images
File Type: png stream_correct.png (66.1 KB, 104 views)
Attached Files
File Type: gz hotRoom_Pimple_atm_tP.tar.gz (3.3 KB, 89 views)
Sherlock_1812 likes this.
Toorop is offline   Reply With Quote

Old   June 2, 2012, 10:03
Default
  #5
New Member
 
Eric
Join Date: Aug 2010
Posts: 14
Rep Power: 5
tunkers is on a distinguished road
Hello Tibor,


Thanks for posting this excellent example! In the past I've always had difficulty defining boundary conditions for the buoyant compressible flow solvers with inlets/outlets.

I've been trying to adapt your buoyantBoussinesqPimpleFoam solver example above so that it also works with the buoyantPimpleFoam solver (no boussinesq approximation). It runs for a while, but then the solver blows up after about 50 iterations with a "maximum iterations exceeded" error

Any ideas on how to get your example working in buoyantPimpleFoam?



--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const
in file /mnt/data3/OpenFOAM/OpenFOAM-2.1.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69.

FOAM aborting


tunkers is offline   Reply With Quote

Old   June 4, 2012, 05:35
Default
  #6
Member
 
Tibor Nyers
Join Date: Jul 2010
Location: Hungary
Posts: 91
Rep Power: 6
Toorop is on a distinguished road
Hi Eric,

I have altered the BC to conform with buoyantPimpleFoam and it runs without a problem, but doesn't produce the desired flow, or at least it looks strange (octopus shape).

Possible source of errors:
  • there's zero rho iterations in the log file
  • the system/fvSolution file rho solver section has 0 for tolerance and relTol (copied from the hotRoom tutorial) - changing it has no effect for me

I have limited experience with buoyant solvers so I have no idea how to fix it, maybe you can pinpoint the source of the problem.
Attached Images
File Type: png octopus.png (40.2 KB, 63 views)
Attached Files
File Type: gz hotRoom_CompressiblePimple_atm_tP.tar.gz (3.2 KB, 39 views)
Toorop is offline   Reply With Quote

Old   June 5, 2012, 07:20
Default
  #7
New Member
 
Eric
Join Date: Aug 2010
Posts: 14
Rep Power: 5
tunkers is on a distinguished road
Hi Tibor, Your modified buoyantPimpleFoam case is very helpful. I will experiment further with it to see if the results seem reasonable. Thanks for your help

Best Regards,

Eric
tunkers is offline   Reply With Quote

Old   June 21, 2013, 02:26
Smile Experimental results to validate the results
  #8
EOC
New Member
 
Join Date: Jun 2013
Posts: 4
Rep Power: 3
EOC is on a distinguished road
Hi everyone,

I am doing a similar simulation of natural convection from horizontal heated plate.Were you guys able to finish your simulation. I am doing a similar simulation and I got similar octopus shaped streamlines.

I want to ask if there is any data available to validate our simulation results.

Regards,
EOC
EOC is offline   Reply With Quote

Reply

Tags
atmosphere, buoyantboussinesq, hotroom

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
Setting outlet Pressure boundary condition using CAFFA code Mukund Pondkule Main CFD Forum 0 March 16, 2011 04:23
Domain Imbalance HMR CFX 3 March 6, 2011 20:10
asking for Boundary condition in FLUENT Destry FLUENT 0 July 27, 2010 00:55
problem with boundary condition??? smn CFX 5 November 24, 2009 06:37
CFX Solver : Sudden crash Hervé CFX 2 June 16, 2008 06:40


All times are GMT -4. The time now is 03:10.