CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

Common setup for p_rgh in complete open domains

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

Like Tree17Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 14, 2020, 15:47
Default
  #21
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
I don't think it is a solver-bug but there is probably something missing I don't get until now or there is no appropriate boundary condition (and I don't have time to investigate into that problem). So you have to check it out yourself.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   October 6, 2021, 08:48
Lightbulb
  #22
Member
 
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 62
Rep Power: 14
thiagopl is on a distinguished road
Hi everybody,

I'm currently working on a problem of natural convection in a open domain using buoyantPimpleFoam and, as many of you, I faced the same problems on the outlet boundary, say, backflow, accelarating flow, divergence, etc. I tried different combinations of boundary conditions, most of them discussed here in this thread.
Recently I found this work which suggests the combination for p_rgh/U of fixedFluxPressure/zeroGradient for the top boundary and totalPressure/pressureInletOutletVelocity for the sides and bottom boundaries.
I tried those on a test case attached and I've got a good result for the flow field on outlet (see video). In my case the bottom part of the domain is a wall. The boundary conditions were the following:

Pressure: p_rgh
Code:
dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 101325;

boundaryField
{
    outlet
    {
        type            fixedFluxPressure;
        value           $internalField;        
    }
    sides
    {
        type            totalPressure;
        p0              $internalField;
        value           $internalField;
    }
    heat
    {
        type            fixedFluxPressure;
        value           $internalField;
    } 
    base
    {
        type            fixedFluxPressure;
        value           $internalField;
    }
    frontAndBack
    {
        type            empty;
    }
}
Velocity: U
Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    outlet
    {
        type            zeroGradient;      
    }
    sides
    {
        type            pressureInletOutletVelocity;
        inletValue	 uniform (0 0 0);     
        value           uniform (0 0 0);
    }
    heat
    {
        type            noSlip;
    }    
    base
    {
        type            noSlip;
    }
    frontAndBack
    {
        type            empty;
    }
}
Temperature: T
Code:
dimensions      [0 0 0 1 0 0 0];

internalField   uniform 293.15;

boundaryField
{
    outlet
    {
        type            inletOutlet;
        inletValue      uniform 293.15;
        value           uniform 293.15;
    }
    sides
    {
        type            inletOutlet;
        inletValue      uniform 293.15;
        value           uniform 293.15;
    }
    heat
    {
        type            fixedValue;
        value           uniform 303.15;        
    } 
    base
    {
        type            zeroGradient;
    }
    frontAndBack
    {
        type            empty;
    }
}
Hope it helps.
Attached Images
File Type: png domain.png (40.9 KB, 93 views)
bambiker likes this.
__________________
Fields of interest: buoyantFoam, chtMultRegionFoam.

Last edited by thiagopl; October 6, 2021 at 09:29. Reason: Deleting comments on the p_rgh file.
thiagopl is offline   Reply With Quote

Old   May 11, 2022, 03:27
Default
  #23
New Member
 
Marco Müller
Join Date: Feb 2013
Location: Germany
Posts: 23
Rep Power: 13
marco.müller is on a distinguished road
Just contributing my findings, since I had the same issue, in case someone will find it helpful:

- I was not able to solve my (steady state) problem with buoyantBoussinesqSimpleFoam. It seems to have a current (v2006 for me) implementation that makes it difficult to deal with openings, see:
Wrong implementation of the Boussinesq assumption in heat transfer solvers
- Using buoyantSimpleFoam worked fine for me (without momentumPredictor, which introduced the same artificial convection with middle speed velocities as buoyantBoussinesqSimpleFoam)
- BC setup:
--- lower opening ("inlet"): prghTotalPressure + pressureInletOutletVelocity
--- upper opening ("outlet"): fixedFluxPressure + pressureInletOutletVelocity
- lastly - since I also had forced convection inside my domain -, I successfully used the limitVelocity option to get a stable initialization
bambiker and Voulet like this.
marco.müller is offline   Reply With Quote

Old   July 26, 2023, 08:30
Default
  #24
Senior Member
 
Join Date: Dec 2021
Posts: 216
Rep Power: 5
Alczem is on a distinguished road
Following the release of OpenFOAM v11, I also want to share some recent tests I did about natural convection and open boundaries since I have been looking into it quite a lot. I think I finally have a decent setup for a steadystate simulation using the fluid solver of OF v11 (similar to buoyantSimpleFoam).

My case is a simple hot box inside a fully open domain, so the air can come and leave frome any side.

I used OpenFOAM v11 because it includes a switch to initialize the hydrostatic pressure in fvSolution so you can use the ph_rgh field and the prghTotalHydrostaticPressure condition in p_rgh. In OpenFOAM v2306, there is a functionObject that does the same initialization but I have yet to try it

Here are the boundary conditions:

p
Code:
internalField   uniform 101325;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

   ".*"
   {
       type            calculated;
       value           uniform 101325;
   }
   
   "(sky|bottom|walls)"
   {
       type            calculated;
       value           uniform 101325;
   }
   
   "vol.*"
    {
        type            empty;
    }
}
p_rgh
Code:
internalField   uniform 0;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    ".*"
    {
        type            fixedFluxPressure;
        
        value           $internalField;
    }

    bottom
    {
        type            prghTotalHydrostaticPressure;
        meanValue        $internalField;
        p0              $internalField;
        value           $internalField;
    }
    
    sky
    {
        type            prghTotalHydrostaticPressure;
        meanValue        $internalField;
        p0              $internalField;
        value           $internalField;
    }
    
    walls
    {
        type            prghTotalHydrostaticPressure;
        meanValue        $internalField;
        p0              $internalField;
        value           $internalField;
    }
    
    "vol.*"
    {
        type            empty;
    }
}
ph_rgh
Code:
internalField   uniform 0;

boundaryField
{
    
    ".*"
    {
        type            fixedFluxPressure;
        
        value           $internalField;
    }

    bottom
    {
        type            fixedFluxPressure;
        meanValue        $internalField;
        p0              $internalField;
        value           $internalField;
    }
    
    sky
    {
        type            fixedValue;
        meanValue        $internalField;
        p0              $internalField;
        value           $internalField;
    }
    
    walls
    {
        type            fixedFluxPressure;
        meanValue        $internalField;
        p0              $internalField;
        value           $internalField;
    }
    
    "vol.*"
    {
        type            empty;
    }

}
U
Code:
internalField   uniform (0 0 0.0);

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    ".*"
    {
        type            fixedValue;
        value           $internalField;
    }
    
    walls
    {
        type            slip;
    }

    bottom
    {
        type            zeroGradient;
        //inletValue        uniform (0 0 0);
        value           $internalField;
    }
    
    sky
    {
        type            zeroGradient; //pressureInletOutletVelocity;
        inletValue        uniform (0 0 0);
        value           $internalField;
    }
    
    walls
    {
        type            zeroGradient; //pressureInletOutletVelocity;
        inletValue        uniform (0 0 0);
        value           $internalField;
    }
    
    "vol.*"
    {
        type            empty;
    }

}
T
Code:
internalField   uniform 293.15;

boundaryField
{
    ".*"
    {
        type            zeroGradient;
        value           uniform 293.15;
        //value           $internalField;
    }
    
    hot_walls
    {
        type            fixedValue;
        value           uniform 393.15;
    }

    "(sky|bottom|walls)"
    {
        type            inletOutlet;
        inletValue      uniform 293.15;
        value           $internalField;
    }
    
    "vol.*"
    {
        type            empty;
    }
        
}
pRef (located in constant, and that's why p_rgh and ph_rgh are set at 0 Pa)
Code:
dimensions      [1 -1 -2 0 0 0 0];
value           101325;
fvSolution
Code:
PIMPLE
{
    momentumPredictor no;
    nNonOrthogonalCorrectors 1;
    //pRefCell        0;
    //pRefValue       0;
    //consistent        yes;
    
    hydrostaticInitialisation yes;
    nHydrostaticCorrectors 10;

}
fvSchemes
Code:
ddtSchemes
{
    default     steadyState;
}

gradSchemes
{
    default     cellLimited Gauss linear 1;
}

divSchemes
{
    default         none;
    div(phi,U)      bounded Gauss linearUpwindV default;
    div(phi,K)      Gauss linearUpwind default;
    div(phi,h)      bounded Gauss linearUpwind default;
    div(phi,k)      bounded Gauss linearUpwind default;
    div(phi,epsilon) bounded Gauss linearUpwind default;
    div(phi,omega)     bounded Gauss linearUpwind default;
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear uncorrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         uncorrected;
}

wallDist
{
    method            meshWave;
}
physicalProperties
Code:
thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

dpdt            off;

mixture
{
    specie
    {
        molWeight       28.96;
    }
    thermodynamics
    {
        Cp              1004.4;
        Hf              0;
    }
    equationOfState
    {
        rho            1.2;
        pRef        101325;
    }
    transport
    {
        mu              1.831e-05;
        Pr              0.705;
    }
}
A few notes:
  • I think the most stable setup for ph_rgh is to have one of the patches at fixedValue and the rest at fixedFluxPressure although it seems to work if fixedFluxPressure is used everywhere but the velocity is not as stable. Using the highest horizontal patch for the fixedValue condition seems ok. I ran the case without any hot patches to see if the air would settle, and the maximume velocity was around 2 cm/s (the domain is 30m tall).
  • Setting the U boundary conditions to zeroGradient or pressureInletOutletVelocity did seem to change anything.
  • Turbulence needs to be on even if nothing is happening inside the domain. The temperature exploded in my case with turbulence off.
  • The main region of interest is too close to the borders of my domain to prevent any perturbations, so I guess better results could be achieved with a larger domain. The vortices are probably due to the narrowness of the domain.
  • Watch out when stopping and running the same case again without any modification. The hydrostatic initialization actually modifies the pressure files which means that stopping and restarting the case will initialize the files that are already initialized. It can lead to an unstable simulation (at least for me).


Here is a picture of the temperature field with the surface LIC representation of the velocity. It looks decent to me but I would like to have other opinions on this Cheers!
Attached Images
File Type: jpg flame.jpg (57.9 KB, 46 views)
thiagopl and Yann like this.
Alczem is offline   Reply With Quote

Old   July 26, 2023, 15:54
Thumbs up
  #25
Member
 
Thiago Parente Lima
Join Date: Sep 2011
Location: Diamantina, Brazil.
Posts: 62
Rep Power: 14
thiagopl is on a distinguished road
Hi Alczem,

Nice work. Although I posted this and also proposed this thread, which lead to conclusions, I still have problems in setting up natural convection problems in open domains.

I found that OF v10 also includes this switch to initialize the hydrostatic pressure in fvSolution.

I'm testing your setup, but in a transient case (good results by now!). I 'ill post the case here once I have conclusive results.
__________________
Fields of interest: buoyantFoam, chtMultRegionFoam.
thiagopl is offline   Reply With Quote

Old   July 26, 2023, 16:01
Default
  #26
Senior Member
 
Join Date: Dec 2021
Posts: 216
Rep Power: 5
Alczem is on a distinguished road
Hey!


I remember reading your various posts, I think I read almost every thread related to this kind of simulation


Yep, the switch was already implemented in OF v10, but I mainly use the ESI version and only recently have I been using the foundation version which has some pros (and cons, still figuring it out!).




From some posts (by Tobias Holzmann I think), it sounded as if free convection might only be properly simulated through transient computation, or at least using a transient initial state to initialize the steady run, which is... not encouraging! I tried local time stepping and large CFL numbers but it still so slow, especially if you are simulating fluids and solids in a CHT case hopefully some common setup will emerge from all our tests
Alczem is offline   Reply With Quote

Old   July 27, 2023, 07:38
Default
  #27
Senior Member
 
Join Date: Dec 2021
Posts: 216
Rep Power: 5
Alczem is on a distinguished road
Back again with a similar case to my previous post, only on a much larger domain (which is 2D now and triangles only, I meshed quickly with Salome and had to be fast).


The pressureInletOutletVelocity condition seems actually more stable than zeroGradient, but they achieve very similar results.


A lot of undesired currents remain present near the boundaries and I did not manage to completely mitigate their effects. They are also present when the hot box was disabled to try to reach a perfectly still atmosphere.


Overall I am pleased with the results, but it is slow: it takes more than 5000 iterations to have a satisfactory flow. Maybe the numerics need more tinkering and other boundary conditions can achieve similar results faster. I still take this as a win
Attached Images
File Type: jpg temperature_large_domain.jpg (31.2 KB, 27 views)
File Type: jpg velocity_large_domain.jpg (105.9 KB, 26 views)
File Type: jpg velocity_still_atmosphere.jpg (38.7 KB, 22 views)
Alczem is offline   Reply With Quote

Old   October 5, 2023, 22:19
Default
  #28
New Member
 
Ali
Join Date: May 2016
Location: Sydney, Australia
Posts: 19
Rep Power: 10
AliVali is on a distinguished road
Hi Bodo1993,

It is about three years since your post. I hope you have had found a solution to this problem and are able to share it with me. I am facing exactly the same issue.

Thanks,
Ali
AliVali is offline   Reply With Quote

Old   October 5, 2023, 22:33
Default
  #29
New Member
 
Ali
Join Date: May 2016
Location: Sydney, Australia
Posts: 19
Rep Power: 10
AliVali is on a distinguished road
Quote:
Originally Posted by Bodo1993 View Post
Hi Tobi,

I encounter the same problem in twoLiquidMixingFoam, a solver for two miscible incompressible fluids. In this solver, the mixture density is interpolated linearly (not a constant value). I face the issue of backflow regularly in my simulations. I start to notice the effect once the mixed phase reaches the outlet boundary. I have tried almost all combinations of the outlet and inlet boundaries, but the problem persists. As you mentioned, when I turn the gravity off, I do not observe a back flow. It tells me that there is an issue with the buoyancy term here. I wish there is a solution for this problem and I am wondering if it is a bug in the solver.

I would greatly appreciate your thoughts and suggestions.

Hi Bodo1993,

It is about three years since your post. I hope you have had found a solution to this problem and are able to share it with me. I am facing exactly the same issue.

Thanks,
Ali
AliVali is offline   Reply With Quote

Reply

Tags
p_rgh open domain

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
MESHING A complete wing setup with SLAT,WING,FLAP for ACOUSTICS AS_Aero Pointwise & Gridgen 3 July 25, 2013 08:27
Problem installing on Ubuntu 9.10 -> 'Cannot open : No such file or directory' mfiandor OpenFOAM Installation 2 January 25, 2010 09:50
Version 15 on Mac OS X gschaider OpenFOAM Installation 113 December 2, 2009 10:23
DxFoam reader update hjasak OpenFOAM Post-Processing 69 April 24, 2008 01:24
OpenFOAM with IBM AIX matthias OpenFOAM Installation 20 March 25, 2008 02:36


All times are GMT -4. The time now is 21:01.