[wyldckat]

Greetings Vasava,

Many thanks for sharing your solution!
I have to say that it's interesting to see a situation where a partial transient solution is useful for initializing a steady-state simulation.

The explanation for this should be easy enough: the transient simulation accounts for the full dynamics of the simulation, while the steady-state does essentially an averaged solution.
This is similar to the situations where increasing the mesh resolution makes it harder to converge a simulation, precisely because the additional resolution reveals new physical details that give a new solution to the simulation... which may be incomplete, due to an incomplete mesh resolution.

Anyway, beyond the existentialist point of view of temporal-spacial discretization, the problem you're seeing could related to a similar situation, for example, imagine this:

1. You have a box that has a heat-flux inlet and a temperature outlet.
2. As a steady-state simulation, the simulation will never converge and could possibly heat up or freeze up endlessly.
3. While the transient simulation will not heat up or freeze up.
4. The reason for this is exactly because of the real time vs averaging situation: averaging the heat exchange effect in some cases will not result in a real steady-state situation.

In your case, you got an extreme situation: the heating as a steady-state simulation resulted in an accelerated heat-up of a particular region, while the transient simulation was able to dissolve the heat properly over time.

Best regards,
Bruno

[vasava]

Thank you Bruno Santos for the explanation!! It nice to begin the week by learning something new. I still consider my self a beginner at both: the CFD and the openFoam. Its nice to learn and discover new things everyday!!

One more thing to add: During my initial experiments I used to initialize the region where the hot fluid is flowing with maximum temperature and the region where the cold fluid is flowing with minimum temperature. This would also cause a very high temperature gradients at the very thin pipe walls (also divergence). But initializing all the domains with minimum temperature and allowing the simulation take its own course gave me quite reasonable solutions.

[Tushar@cfd]

Originally Posted by vasava

Thank you Bruno Santos for the explanation!! It nice to begin the week by learning something new. I still consider my self a beginner at both: the CFD and the openFoam. Its nice to learn and discover new things everyday!!

One more thing to add: During my initial experiments I used to initialize the region where the hot fluid is flowing with maximum temperature and the region where the cold fluid is flowing with minimum temperature. This would also cause a very high temperature gradients at the very thin pipe walls (also divergence). But initializing all the domains with minimum temperature and allowing the simulation take its own course gave me quite reasonable solutions.

Thanks for briefing your views. I totally agree with you, when you start your simulation with large difference/error (as hot/cold fluid in your case) it is more likely to have stability issues. It's always better to follow your approach for stable solutions.

-
Best Regards!

[dafe]

Hi everyone, I am new to open foam and trying to model heat transfer in a closed circuit pipe/tube(rectangular shape for simplicity). In my blockMeshDict when specifying boundary; for the leftwall for example, do i just take the extreme outer face or do i have to specify both faces on the left side (inside and outside). Most tutorials i have seen are basically cavity types which have only one wall to the left. Thanks

[wyldckat]

Quick answer: http://www.cfd-online.com/Forums/ope...egionfoam.html

[dafe]

thanks for the link, will check it out and get back to you.

[laurent98]

@Vasava
thanks so much for this idea, i'm facing this problem for weeks, i must run before chtMultiRegionFoam .? ( I’m also a beginner, build a solver look like a hard job to me...)
thank you very much.

[MBttR]

Hi!

In the end I want to simulate a cylinder generating heat in a flow of air with some other blocking geometries as well, but seeing how the rule is to start of simple and increase complexity I started with the planeWall2D tutorial by Bruno Santos, accompanied by the report by Maaike van der Tempel.

I thought I understood everything so went to my next step of complexity; modelling a 3D cylinder of 350K suspended in a volume of air of 300K. This however crashed after a couple of iterations (not the first one) due to temperatures going very high (100,000K), then very low/negative. At one point I could get it such that the temperature fluctuated for tens of thousands of Kelvin and then settled around more reasonable 345K values. This however seemed like complete bogus to me so I went back a step on the complexity ladder.

I returned to the planeWall2D case, this time turning it into a 2D block suspended in the air. However, my solution still diverges to a negative temperature after many iterations making the simulaiton crash, as can be seen in the ending of my log.chtMultiRegionSimpleFoam. I will post my code after the error.

Solving for fluid region bottomAir
DILUPBiCG:  Solving for Ux, Initial residual = 0.373465, Final residual = 0.0008348504, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.3983659, Final residual = 0.002457276, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.03343168, Final residual = 7.176597e-05, No Iterations 1
Min/max T:296.7828 345.5452
GAMG:  Solving for p_rgh, Initial residual = 0.2517964, Final residual = 0.001801136, No Iterations 4
time step continuity errors : sum local = 1.80743, global = 0.1183804, cumulative = 0.3588659
Min/max rho:0.8133568 2

Solving for solid region wall
DICPCG:  Solving for h, Initial residual = 0.03221371, Final residual = 0.0003819145, No Iterations 1
Min/max T:min(T) [0 0 0 1 0 0 0] 345.3996 max(T) [0 0 0 1 0 0 0] 345.6923
ExecutionTime = 90.23 s  ClockTime = 90 s

Time = 1313


Solving for fluid region bottomAir
DILUPBiCG:  Solving for Ux, Initial residual = 0.1843478, Final residual = 0.001331729, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.3706879, Final residual = 0.002551714, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.02562959, Final residual = 0.0002373, No Iterations 1
Min/max T:297.6073 345.5416
GAMG:  Solving for p_rgh, Initial residual = 0.2469737, Final residual = 0.002262424, No Iterations 4
time step continuity errors : sum local = 1.180225, global = 0.8575721, cumulative = 1.216438
Min/max rho:0.2 1.670909

Solving for solid region wall
DICPCG:  Solving for h, Initial residual = 0.03223895, Final residual = 0.0003933997, No Iterations 1
Min/max T:min(T) [0 0 0 1 0 0 0] 345.3962 max(T) [0 0 0 1 0 0 0] 345.6887
ExecutionTime = 90.3 s  ClockTime = 90 s

Time = 1314


Solving for fluid region bottomAir
DILUPBiCG:  Solving for Ux, Initial residual = 0.5954829, Final residual = 0.0007776412, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.5604225, Final residual = 0.002729626, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.08661401, Final residual = 0.0003479413, No Iterations 1
Min/max T:-1155.061 345.5381
GAMG:  Solving for p_rgh, Initial residual = 0.4870689, Final residual = 0.001921832, No Iterations 4
time step continuity errors : sum local = 2.404536, global = -0.1866434, cumulative = 1.029795
Min/max rho:0.2 2

Solving for solid region wall
DICPCG:  Solving for h, Initial residual = 0.050871, Final residual = 0.0007805152, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 345.0073 max(T) [0 0 0 1 0 0 0] 345.6852
ExecutionTime = 90.37 s  ClockTime = 90 s

Time = 1315


Solving for fluid region bottomAir
DILUPBiCG:  Solving for Ux, Initial residual = 0.3712775, Final residual = 0.001556036, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.5173233, Final residual = 0.001700514, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.1986274, Final residual = 7.361579e-05, No Iterations 1


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

    From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const
    in file /home/bruno/OpenFOAM/OpenFOAM-2.4.0/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:?
#3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:?
#4  ? at ??:?
#5  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6  ? at ??:?
Aborted (core dumped)

Now for the code; To do this I kept blockMesh the same:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
    (0 0 0)
    (1 0 0)
    (1 1 0)
    (0 1 0)
    (0 0 0.1)
    (1 0 0.1)
    (1 1 0.1)
    (0 1 0.1)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (100 100 1) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
    topAir_top
    {
        type patch;
        faces
        (
            (3 7 6 2)
        );
    }
    bottomAir_bottom
    {
        type patch;
        faces
        (
            (1 5 4 0)
        );
    }
    leftLet
    {
        type patch;
        faces
        (
            (0 4 7 3)
        );
    }
    rightLet
    {
        type patch;
        faces
        (
            (2 6 5 1)
        );
    }
    frontAndBack
    {
        type empty;
        faces
        (
            (0 3 2 1)
            (4 5 6 7)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //

and changed topoSet to:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(
    // wall
    {
        name    wall;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (0.4 0.4 0 )(0.6 0.6 0.1);
        }
    }
    {
        name    wall;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set wall;
        }
    }

    // bottomAir
    {
        name    bottomAir;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (0 0 0 )(1 1 0.1);
        }
    }
    {
        name    bottomAir;
        type    cellSet;
        action  delete;
        source  boxToCell;
        sourceInfo
        {
            box (0.4 0.4 0 )(0.6 0.6 0.1);
        }
    }
    {
        name    bottomAir;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set bottomAir;
        }
    }

);

// ************************************************************************* //

As you can see I deleted topAir from the default case and kept the name bottomAir to keep as much things alike as possible. I then changed the bottomAir changeDictionaryDict to:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dictionaryReplacement
{
    boundary
    {
        bottomAir_bottom
        {
            type            symmetryPlane;
        }
	topAir_top
        {
            type            symmetryPlane;
        }	
    }

    U
    {
        internalField   uniform (0.1 0 0);

        boundaryField
        {
            leftLet
            {
                type            fixedValue;
                value           uniform ( 0.1 0 0 );
            }

            rightLet
            {
                type            inletOutlet;
                inletValue      uniform ( 0 0 0 );
                value           uniform ( 0.1 0 0 );
            }

            bottomAir_bottom
            {
                type            symmetryPlane;
            }
	topAir_top
        {
            type            symmetryPlane;
        }
            
            "bottomAir_to_.*"
            {
                type            fixedValue;
                value           uniform (0 0 0);
            }
        }
    }

    T
    {
        internalField   uniform 300;

        boundaryField
        {
            leftLet
            {
                type            fixedValue;
                value           uniform 300;
            }

            rightLet
            {
                type            zeroGradient;
            }

            bottomAir_bottom
            {
                type            symmetryPlane;
            }
	topAir_top
        {
            type            symmetryPlane;
        }

            "bottomAir_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                Tnbr            T;
                kappa           fluidThermo;
                kappaName       none;
                value           uniform 300;
            }
        }
    }

    epsilon
    {
        internalField   uniform 0.01;

        boundaryField
        {
            leftLet
            {
                type            inletOutlet;
                inletValue      uniform 0.01;
                value           uniform 0.01;
            }

            rightLet
            {
                type            fixedValue;
                value           uniform 0.01;
            }

            bottomAir_bottom
            {
                type            symmetryPlane;
            }
	topAir_top
        {
            type            symmetryPlane;
        }

            "bottomAir_to_.*"
            {
                type            compressible::epsilonWallFunction;
                value           uniform 0.01;
            }
        }
    }

    k
    {
        internalField   uniform 0.1;

        boundaryField
        {
            leftLet
            {
                type            inletOutlet;
                inletValue      uniform 0.1;
                value           uniform 0.1;
            }

            rightLet
            {
                type            fixedValue;
                value           uniform 0.1;
            }

            bottomAir_bottom
            {
                type            symmetryPlane;
            }
	topAir_top
        {
            type            symmetryPlane;
        }

            "bottomAir_to_.*"
            {
                type            compressible::kqRWallFunction;
                value           uniform 0.1;
            }
        }
    }

    p_rgh
    {
        internalField   uniform 1e5;

        boundaryField
        {
            ".*"
            {
                type            fixedFluxPressure;
                value           uniform 1e5;
            }

            bottomAir_bottom
            {
                type            symmetryPlane;
            }
	topAir_top
        {
            type            symmetryPlane;
        }

            leftLet
            {
                type            fixedValue;
                value           uniform 1e5;
            }

            frontAndBack
            {
                type            empty;
            }
          
        }
    }

    p
    {
        internalField   uniform 1e5;

        boundaryField
        {
            ".*"
            {
                type            calculated;
                value           uniform 1e5;
            }

            bottomAir_bottom
            {
                type            symmetryPlane;
            }
	topAir_top
        {
            type            symmetryPlane;
        }

            leftLet
            {
                type            calculated;
                value           uniform 1e5;
            }

            frontAndBack
            {
                type            empty;
            }
          
        }
    }
}

// ************************************************************************* //

and the wall changeDictionaryDict to:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dictionaryReplacement
{
    T
    {
        internalField   uniform 350;

        boundaryField
        {
            ".*Let"
            {
                type            zeroGradient;
                value           uniform 300;
            }
            "wall_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                Tnbr            T;
                kappa           solidThermo;
                kappaName       none;
                value           uniform 300;
            }
        }
    }
}

// ************************************************************************* //

I have changed the relaxationFactor h for airBottom from 0.7 to 0.3, but that maybe gave me a couple more iterations before crashing as well. I know this must be something really simple but I am at a complete loss. I don't see what can be wrong about my boundary conditions, why they should be any different than the standard planeWall2D case. Maybe it is something in fvSchemes or fvSolution but again, I'm not sure why that would be. I decreased timesteps to no avail.

For the sake of completeness I'm attaching the case here as well.

Can anyone shed some light on this? Many thanks! And for those on their way to the workshop in Portugal, have fun.

Greetings,

Bruno

[visheshkapoor06]

Hi Bruno,
I am facing the same problem but my velocity is diverging in the 1st iteration and the temperature in the 2nd.
Can you please tell, how did you corrected it such that the iterations ran and settled after a while?
Also, I am using OpenFOAM 3.0.1, should i try and run the case using openFOAM 2.4.0?

Thank you
Regards
Vishesh

[jaydeep]

Hello everyone,

I have been trying to port the classic PlaneWall 2D case for the latest OF release. I am attaching the zip for all files. The case runs well, but in the end it throws a ton of errors on ParaView and results are in my opinion unrealistic.

Can somebody take a look at it and please let me know what all could be the probable causes ?


Thanks!

P.S. I use OF+ on windows, use native ParaView. Once the simulation is finished, you can open foam.foam file in PV for postprocessing.

[jaydeep]

I guess I could narrow down the errors in ParaView to initial condition. After splitmesh the newly created boundaries do not appear explicitly in 0. And thus ParaView on windows fails to recognize .* . Now I am not sure whether this has to do with the OF for windows, or is it a general problem. Can someone take a look at it?

P.S. Still the results look unreasonable

[sitajeje]

Dear Bruno,

thank you very much first of all for your planeWall2D. I downloaded your case files and run it. But the resultant planeWall2D.OpenFOAM file is empty. The Paraview exit automatically when I press on "apply" button to load the data. My OpenFOAM is V4.0.

I would appreciate greatly if you can help me on this, although it is a 3 year old post.

Best regards,

Hai

[wyldckat]

Quick answers: First of all, sorry to everyone, but:

1. I haven't had enough free time to look into your questions and I won't be able to answer to them all on this post right now.
2. I can't find it right now, but I know I wrote a post... last year, I think... in which I stated that the tutorial was not working properly as of OpenFOAM 2.3. This situation still stands, as I haven't managed to find enough time to study things properly.

The best I can suggest right now is suggest what I suggested to another forum member a few days ago:

Originally Posted by wyldckat

so the best I can do is suggest that you study the course presentation and cases that are provided here: http://www.openfoamworkshop.org/courses - look for the presentation "Learning how to use free surface flows in OpenFOAM 3.0" and click on the download link to the right of the entry "Training Material".

The free surface flows are also using the same kind of pressure management as in the chtMultiRegion*Foam solvers.



Now, to answer in detail to a few questions:

Originally Posted by jaydeep

I guess I could narrow down the errors in ParaView to initial condition.

Yes, the internal reader in ParaView does not support all boundary conditions that OpenFOAM supports at the moment. Therefore, ParaView will complain when it doesn't understand a boundary condition

Originally Posted by jaydeep

P.S. Still the results look unreasonable

It's as I indicated at the start of this post that you're reading.

Originally Posted by sitajeje

But the resultant planeWall2D.OpenFOAM file is empty. The Paraview exit automatically when I press on "apply" button to load the data.

Yes, the file is meant to be empty, it's just sort-of a tag for ParaView to know which folder to use.
And it looks like you did not properly ready the wiki page. This is explained here: http://openfoamwiki.net/index.php/Ge...ost-Processing

[sitajeje]

Dear Bruno,

thank you very much for your prompt reply! I am a beginner for OpenFOAM and can easily make stupid mistakes.

I wonder whether I have done anything wrong. After I executed Allrun, I didn't get
planeWall2D{bottomAir}.OpenFOAM planeWall2D{topAir}.OpenFOAM planeWall2D{wall}.OpenFOAM

but only planeWallD.OpenFOAM and planeWallD.blockMesh. The other 7 files begin with log..

I use Ubundu 14.04, and OpenFOAM 4.0. I would appreciate greatly if you can give me a guide.

Thank you very much in advance!

Have a nice evening!

Sitajeje

[vasava]

Originally Posted by MBttR

Can anyone shed some light on this?

I see that you are using ideal gas for fluid. Also, there is negative temperature (around -500 K and I havent investigated the cause of the negative temperature) and it is causing the simulation to diverge.

If you aim is to merely simulate conjugate heat transfer, I recommend you to switch to normal air properties.

[vasava]

Originally Posted by sitajeje

After I executed Allrun, I didn't get
planeWall2D{bottomAir}.OpenFOAM planeWall2D{topAir}.OpenFOAM planeWall2D{wall}.OpenFOAM

but only planeWallD.OpenFOAM and planeWallD.blockMesh. The other 7 files begin with log..

You dont need separate files for separate regions to view results, the file planeWallD.OpenFOAM should be enough.

[zfaraday]

I think you are wrong Paritosh, actually you need those files in order to be able to see the results in each region, otherwise you can't watch the results!

In order to create them, the command to be executed is

paraFoam -touchAll

Regards,

Alex

[sitajeje]

Dear Alex and Paritosh,

thank you very much for your help! I wonder whether you have the planeWall2D case file which you have run through? I would appreciate if you would share it with me. I still cannot get the planeWall2D{bottomAir}.OpenFOAM, planeWall2D{topAir}.OpenFOAM and planeWall2D{wall}.OpenFOAM files.

All the best
sitajeje

[vasava]

Originally Posted by zfaraday

In order to create them, the command to be executed is

paraFoam -touchAll

I use,

paraFoam -builtin

Which creates only one file, case.foam. Works just fine. Just another way.

[sitajeje]

Thank you very much Paritosh! The command "paraFoam -touchAll" exists in the "Allrun" file. After execution, the "planeWall2D.OpenFOAM" is empty. I don't have folders of "bottomAir", "topAir" or "wall" in the "0" folder.

I ran through the tutorial "multiRegionHeater", created files such as "multiRegionHeater{bottomWater}.OpenFOAM" and also folders such as "bottomWater" in the "0" folder. However all the "*.OpenFOAM" files were empty. The command "paraFoam -touchAll" also exists in the "Allrun" file. In paraView I can only find the blockMesh, nothing more. The terminal didn't report an error, and seems to run through all the commands in the "Allrun" file.

I am a beginner for OpenFOAM. I wonder whether my installation was incomplete. I could run the tutorial case "cavity" successfully.

Thank you very much for your help in advance!