Fluid flow from a pipe

Raza Javed · May 6, 2019, 12:47

Hello Everyone,

I made a very simple geometry in Salome, a rectangular pipe, and I want to model the fluid flow from it.

I try to explain my problem as clear as I can.

My geometry has 2 regions. (one is pipe and other is fluid). You can see the geometry below in the figure. (The yellow region is the fluid and the outer green region is pipe)

I imported this geometry to Openfoam using ideasUnvToFoam. I am using chtMultiRegionSimpleFoam. After changing all the boundary conditions using changeDictionaryDict. When I run the solver, I get the following error:

Code:

Solving for fluid region fluid
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:?
#5  Foam::fluidThermo::nu() const at ??:?
#6  Foam::laminar<Foam::ThermalDiffusivity<Foam::CompressibleTurbulenceModel<Foam::fluidThermo> > >::nuEff() const at ??:?
#7  Foam::linearViscousStress<Foam::ThermalDiffusivity<Foam::CompressibleTurbulenceModel<Foam::fluidThermo> > >::divDevRhoReff(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) const at ??:?
#8  ? at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  ? at ??:?
Floating point exception (core dumped)

It shows that when it starts solving the fluid region, it gives the error. The problem is that I couldn't even understand what is the error?

I am attaching my changeDictionaryDict from system/region_name for your reference:

PIPE

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

T
{
    internalField   uniform 300;
    pipeInlet
    {
        type            wall;

    }
    pipeOutlet
    {
        type            wall;

    }
    defaultFaces
    {
        type            wall;

    }
    boundaryField
    {
        "pipeInlet"
        {
            type            fixedValue;
            value           uniform 300;
        }
        "pipeOutlet"
        {
            type            fixedValue;
            value           uniform 300;
        }
        "defaultFaces"
        {
            type            zeroGradient;

        }

        "pipe_to_.*"
        {
            type            compressible::turbulentTemperatureCoupledBaffleMixed;
            Tnbr            T;
            kappaMethod     solidThermo;
            kappaName       none;
            value           uniform 300;
        }
    }
}

And the boundary file from constant/region_name/polymesh is given below:

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/pipe/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

4
(
    pipeInlet
    {
        type            patch;
        nFaces          36;
        startFace       4896;
    }
    pipeOutlet
    {
        type            patch;
        nFaces          36;
        startFace       4932;
    }
    defaultFaces
    {
        type            patch;
        nFaces          1108;
        startFace       4968;
    }
    pipe_to_fluid
    {
        type            mappedWall;
        inGroups        1(wall);
        nFaces          860;
        startFace       6076;
        sampleMode      nearestPatchFace;
        sampleRegion    fluid;
        samplePatch     fluid_to_pipe;
    }
)

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

And for fluid region, the corresponding files are given below:

FLUID
system/region_name/changeDictionaryDict

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
boundary
{
    fluidInlet
    {
        type            wall;
    }
    fluidOutlet
    {
        type            wall;
    }
}
U
{
    internalField   uniform (0 0 0.001);

    boundaryField
    {
        fluidInlet
        {
            type            fixedValue;
            value           uniform (0 0 0.001);
        }

        fluidOutlet
        {
            type            inletOutlet;
            inletValue      uniform (0 0 0);
        }

        ".*"
        {
            type            noSlip;
        }
    }
}

T
{
    internalField   uniform 300;

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

        fluidOutlet
        {
            type            inletOutlet;
            inletValue      uniform 300;
        }

        ".*"
        {
            type            zeroGradient;
            value           uniform 300;
        }

        "fluid_to.*"
        {
            type            compressible::turbulentTemperatureCoupledBaffleMixed;
            Tnbr            T;
            kappaMethod     fluidThermo;
            value           uniform 300;
        }
    }
}


epsilon
{
    internalField   uniform 0.01;

    boundaryField
    {
        minX
        {
            type            fixedValue;
            value           uniform 0.01;
        }

        maxX
        {
            type            inletOutlet;
            inletValue      uniform 0.01;
        }

        ".*"
        {
            type            epsilonWallFunction;
            value           uniform 0.01;
        }
    }
}

k
{
    internalField   uniform 0.1;

    boundaryField
    {
        minX
        {
            type            inletOutlet;
            inletValue      uniform 0.1;
        }

        maxX
        {
            type            zeroGradient;
            value           uniform 0.1;
        }

        ".*"
        {
            type            kqRWallFunction;
            value           uniform 0.1;
        }
    }
}


p_rgh
{
    internalField   uniform 0;

    boundaryField
    {
        fluidInlet
        {
            type            zeroGradient;
            value           uniform 0;
        }

        fluidOutlet
        {
            type            fixedValue;
            value           uniform 0;
        }

        ".*"
        {
            type            fixedFluxPressure;
            value           uniform 0;
        }
    }
}

p
{
    internalField   uniform 0;

    boundaryField
    {
        ".*"
        {
            type            calculated;
            value           uniform 0;
        }
    }
}

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

and Constant/region_name/polymesh/boundary

Code:

FoamFile
{
    version     0.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/fluid/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


3
(
    fluidInlet
    {
        type            wall;
        nFaces          32;
        startFace       5723;
    }

    fluidOutlet
    {
        type            wall;
        nFaces          30;
        startFace       5755;
    }

    fluid_to_pipe
    {
        type            mappedWall;
        inGroups        1 ( wall );
        nFaces          860;
        startFace       5785;
        sampleMode      nearestPatchFace;
        sampleRegion    pipe;
        samplePatch     pipe_to_fluid;
    }

)

I shall be thankful if someone can guide, what exactly this error is? and How can I rectify it?

Thank you

alexeym · May 6, 2019, 13:07

Hi,

The error is division by zero during calculation of fluid kinematic viscosity. It is calculated using dynamic viscosity and density. So the question is, why density of your fluid is zero? It could be due tu your initial conditions or due to supplied thermophysical properties.

sheaker · May 6, 2019, 13:19

Hello.

Why did You modeled structure of pipe? It looks like You are only interested in fluid flow.

Best regards,
Oskar

Raza Javed · May 7, 2019, 05:56

Quote:

Originally Posted by alexeym

Hi,

The error is division by zero during calculation of fluid kinematic viscosity. It is calculated using dynamic viscosity and density. So the question is, why density of your fluid is zero? It could be due tu your initial conditions or due to supplied thermophysical properties.

Thank you so much for your answer. It solved my problem.

I have one more question, that how can I see the fluid flow from my geometry?

I mean, when I run my simulation, I want to visualize the fluid flow from my rectangular pipe. but I don't exactly know, how to do it.

I have read somewhere, that I need to have "alpha1" in my "0" directory.
Can you please help me in this?

Thank you

Raza Javed · May 7, 2019, 06:18

Quote:

Originally Posted by sheaker

Hello.

Why did You modeled structure of pipe? It looks like You are only interested in fluid flow.

Best regards,
Oskar

Thank you so much for your reply.

Yes I am interested in fluid flow.

I made two regions in my geometry. As you can see in the figure, the outer green region is pipe and the inner yellow region is fluid.

And I want to see, the fluid flowing from inlet to outlet in Paraview.

But I am unable to do it because I don't know what exactly to put into the region directories of fluid and pipe.

I thought I need to select "U" in Paraview to see the fluid flowing, but when I do it, it shows nothing.

I don't know If I am making mistakes in writing the boundary conditions OR I am missing something to put into the region directories.

Maybe, I am not so clear in explaining my problem. Please let me know if you need any clarification to answer my question.

Thank you

Raza Javed · May 7, 2019, 06:27

One more question here,

Why do we use "alpha1" file in the "0" directory?

If I want to visualize the fluid flow from a pipe then do I need "alpha1" file?

Thank you

alexeym · May 7, 2019, 06:59

It is not quite clear what difficulties you encounter during visualisation. You open case in ParaView, you select your pipe region, you do the visualisation.

alpha1 in 0 folder appears in two-phase simulations (eg. interFoam solver). For CHT simulations, usually there is no need in alpha1.

Raza Javed · May 7, 2019, 07:05

Quote:

Originally Posted by alexeym

It is not quite clear what difficulties you encounter during visualisation. You open case in ParaView, you select your pipe region, you do the visualisation.

alpha1 in 0 folder appears in two-phase simulations (eg. interFoam solver). For CHT simulations, usually there is no need in alpha1.

Thank you for your reply. OK it means I don't need alpha1.

Yes I open case in paraview, I select the fluid region and I want to see the velocity profile. and it shows the following (figure below)

It looks like from the figure that the velocity becomes zero right after inlet surface.

I don't know should it be like this? because fluid should go from inlet to outlet.

sheaker · May 7, 2019, 13:29

Well... I think that walls are no-slip so velocity is always zero. Try to check velocity in interior part.

You don't need to model pipe itself. Just model interior part where fluid flows.

Best regards,
Oskar

Raza Javed · May 8, 2019, 04:09

Quote:

Originally Posted by sheaker

Well... I think that walls are no-slip so velocity is always zero. Try to check velocity in interior part.

You don't need to model pipe itself. Just model interior part where fluid flows.

Best regards,
Oskar

Thank you for your reply. It was really helpful.

I have one more question, Now it is showing me the velocity profile at the surfaces and also inside the geometry.

How can we visualize the fluid flow in this pipe domain?

Thank you

sheaker · May 8, 2019, 13:03

Hello.

I am not using openFoam now, so I cannot reproduce Your case.

If I were You I would model just a half of the domain and use symmetry boundary condition. In that case interior part will be well exposed.
I don't know if this solution will be suitable for You.

Best regards,
Oskar

alexeym · May 10, 2019, 04:17

Hi,

@Raza Javed

Select fluid region and use Clip filter to cut it in half (plane should have normal perpendicular to the tube axis). This way you will be able to see what is inside your tube.

Raza Javed · May 10, 2019, 11:19

Thank you so much for your reply. It was really helpful.

I have one more question related to same geometry.

I know the Pressure, Velocity and Temperature of the fluid at the inlet.

Now, if due to some reason, some temperature rise from the outside of the pipe occurs, that will also raise the temperature of the fluid, then at the outlet the temperature of the fluid will be different. How can I find the temperature at the outlet?

And what boundary conditions for pressure, velocity and temperature would be suitable at inlet and outlet?

I shall be very thankful if you can help me out in this.

Thank you

sufjanst · May 13, 2019, 06:24

There are different ways to find out your outlet temperature.

You can simply do it in paraview or you can use the funciton 'sample'.
I guess the standard boundary conditions should be fine for your inlet and outlet (fixedValue, inletOutlet, noSlip).

I got interested in your thread because you managed to import a Salome Mesh to OpenFOAM. Can you tell me how you did that? I created a mesh but when I try to use ideasUnvToFoam I get the error 'cell type 22 not supported'. I use OpenFOAM 6.

Thank you and good luck

Raza Javed · May 13, 2019, 06:27

Thank you so much for your reply.

Which options/hypothesis did you use while creating a mesh in Salome?

Raza Javed · May 20, 2019, 04:32

Quote:

Originally Posted by alexeym

Hi,

The error is division by zero during calculation of fluid kinematic viscosity. It is calculated using dynamic viscosity and density. So the question is, why density of your fluid is zero? It could be due tu your initial conditions or due to supplied thermophysical properties.

Hello @alexeym,

I have one another problem, and I thought you could help me in this.

I am using chtMultiRegionSimpleFoam and my OpenFoam version is 4.1.

Now, I am able to simulate the fluid. But somehow it doesn't seem to be working well.

I am facing problems in boundary conditions for the fluid region. I am trying different combinations of boundary conditions of (velocity, Pressure and Temperature), but I don't really know that which one is correct, because my solver is not converging as per my understanding.

My requirement is that I need to put some fix velocity at the inlet and there is a temperature change along the fluid region due to some hot plates working as heat sources outside the walls of fluid region. And then, I want to see the temperature change at the outlet of the fluid region. I don't have any particular requirement for pressure in my simulation. With these conditions, I want to check at which value of velocity does my simulation reaches the steady state? Also I defined my fluid to be laminar flow. Is it correct?

My problem is that when I change the values of velocity and pressure, my solver RUNS but after some iterations, it gives an error that "maximum number of iterations exceeded". And then I tried to reduce the time interval in the "controlDict" file, then my solver runs completely without error, but my final residual is too high that it doesn't seem to be converging.

I am posting my solver log and my changeDictionaryDict (boundary conditions).
if you can please have a look, I shall be very thankful because I am not able to interpret the log because I am new to OpenFoam.

changeDictionaryDict File

Code:

boundary
{
    inlet
    {
        type            patch;
    }
    outlet
    {
        type            patch;
    }

}
U
{
    internalField   uniform (0 1e-3 0);

    boundaryField
    {
        inlet
        {
            type                fixedValue;//flowRateInletVelocity;//pressureInletVelocity;//
            //volumetricFlowRate  0.2;
            //extrapolateProfile  yes;
            value               uniform (0 1e-3 0);
        }

        outlet
        {
            type                inletOutlet;//zeroGradient;////
            value               $internalField;//uniform (0 0 0);//
            inletValue          $internalField;
        }
        "fluid_to_box"
        {
            type                noSlip;
        }
    }
}

T
{
    internalField   uniform 300;

    boundaryField
    {
        inlet
        {
            type            fixedValue;
            value           uniform 300;//$internalField;
            
        }

        outlet
        {
            type            inletOutlet;
            value           $internalField;
            inletValue      $internalField;
        }

        "fluid_to_box"
        {
            type            compressible::turbulentTemperatureCoupledBaffleMixed;
            Tnbr            T;
            kappaMethod     fluidThermo;
            value           uniform 300;
        }
    }
}


epsilon
{
    internalField   uniform 0.01;

    boundaryField
    {
        inlet
        {
            type            fixedValue;
            value           uniform 0.01;
        }

        outlet
        {
            type            inletOutlet;
            inletValue      uniform 0.01;
        }

        ".*"
        {
            type            epsilonWallFunction;
            value           uniform 0.01;
        }
    }
}

k
{
    internalField   uniform 0.1;

    boundaryField
    {
        inlet
        {
            type            inletOutlet;
            inletValue      uniform 0.1;
        }

        outlet
        {
            type            zeroGradient;
            value           uniform 0.1;
        }

        ".*"
        {
            type            kqRWallFunction;
            value           uniform 0.1;
        }
    }
}


p_rgh
{
    internalField   uniform 0;

    boundaryField
    {
        inlet
        {
            type            fixedFluxPressure;//zeroGradient;
            value           uniform 0;
        }

        outlet
        {
            type            fixedValue;
            value           uniform 0;
        }

        ".*"
        {
            type            fixedFluxPressure;
            value           uniform 0;
        }
    }
}
p
{
    internalField   uniform 0;

    boundaryField
    {
        inlet
        {
            type            zeroGradient;
            //value           uniform 1;
        }
        outlet  
        {
            type            fixedValue;
            value           uniform 0;
        }        
        "fluid_to_.*"
        {
            type            zeroGradient;
        }
    }
}

Log File

Code:

Time = 4


Solving for fluid region fluid
DILUPBiCG:  Solving for Ux, Initial residual = 0.6911749, Final residual = 0.04280814, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 0.6577878, Final residual = 0.04376797, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 0.5181872, Final residual = 0.02078987, No Iterations 2
DILUPBiCG:  Solving for h, Initial residual = 0.5998981, Final residual = 0.03528898, No Iterations 2


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

     From function Foam::scalar Foam::species::thermo<Thermo,  Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar  (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar,  Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo,  Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar  (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const)  const [with Thermo =  Foam::hConstThermo<Foam::rhoConst<Foam::specie> >; Type =  Foam::sensibleEnthalpy; Foam::scalar = double;  Foam::species::thermo<Thermo, Type> =  Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie>  >, Foam::sensibleEnthalpy>]
    in file /home/ubuntu/OpenFOAM/OpenFOAM-4.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.

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::rhoConst<Foam::specie>  >, Foam::sensibleEnthalpy> > > >::calculate() at ??:?
#3   Foam::heRhoThermo<Foam::rhoThermo,  Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<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)

What combination of boundary condition would be ideal for my case? OR is there something else other than the boundary conditions that I am missing?

Thank you

alexeym · May 20, 2019, 09:03

Hi,

OK. Let's start from the very beginning. Forget about boundary conditions for a minute. Describe your process.

You have a flow inside a tube. You have a liquid with constant temperature are one end (inlet). There are heat sources outside the tube.

So the following questions should be addressed BEFORE any further discussion about suitable boundary conditions:
- Are you interested in temperature distribution inside pipe itself?
- What is your Re?
- Is distribution of the external heat sources constant?
- What flow parameters you have at the inlet? What information you have at the outlet?

Raza Javed · May 20, 2019, 09:38

Thank you so much for your reply.

Pardon me if my language is confusing for you. Since I am new to OpenFoam, I am not familiar with most of the terms. But I will try to explain my level best.

I try to explain my problem from the start.

I am attaching my geometry with this. one image is the complete box and the other one is inside box.(3 blue long rectangles and one green pipe with inlet and outlet).

I made this geometry on Salome, and then I imported in Openfoam using UNV file.

Then I put my boundary conditions using system/region_name/changeDictionaryDict.

The answers to your questions are:

1. I am actually interested in the overall temperature change throughout the fluid region.(green pipe in the geometry)

2. I have made these hot rectangles heat sources using fvOptions. I am attaching my fvOptions file also. And I think the distribution of heat sources is constant.

3. To be honest, I didn't check my Reynolds number (Re) because I don't know much about it. I know the formula for that, but don't know what impact it has on my simulation.

4. At inlet, I have flow rate (1 litre per minute) and temperature and velocity (optional).
at outlet, I have no requirement of parameters.

Hope, I answered your questions, if NOT, then please let me know, I would be happy to answer.

Thank you

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

heatSource
{
    type            scalarSemiImplicitSource;
    active          true;
 
    scalarSemiImplicitSourceCoeffs
    {
        selectionMode   all; // all, cellSet, cellZone, points
       // cellZone        hot;        
        //cellSet         c1;
        volumeMode      specific; // absolute;
        injectionRateSuSp
        {
            h     (9e6 0);
        }
    }
}

Raza Javed · May 21, 2019, 10:30

Quote:

Originally Posted by alexeym

Hi,

OK. Let's start from the very beginning. Forget about boundary conditions for a minute. Describe your process.

You have a flow inside a tube. You have a liquid with constant temperature are one end (inlet). There are heat sources outside the tube.

So the following questions should be addressed BEFORE any further discussion about suitable boundary conditions:
- Are you interested in temperature distribution inside pipe itself?
- What is your Re?
- Is distribution of the external heat sources constant?
- What flow parameters you have at the inlet? What information you have at the outlet?

Hi..

I have studied about Reynolds number, and according to my fluid region my Reynolds number is less than 2300 which indicates that it is laminar flow.

Now, this situation rises a question in my mind, that is it possible to have Laminar flow in this type of fluid geometry?

Thank you

alexeym · May 22, 2019, 17:01

OK. We can simulate flow inside the tube as a flow of incompressible fluid. You can simulate is as a laminar flow to start with something (also for turbulence you need better mesh).

On your figure there are three regions: tube, heaters, everything else. What is "everything else" (white area on your figure)? What is the mechanism of heat exchange between the heaters and the tube?

Concerning inlet and outlet boundary conditions for the tube. For inlet you have a set of fixed values for temperature and velocity. At the outlet you assume, that flow is not disturbed, so values at the outlet faces (for temperature and velocity), should be equal to internal values, hence, it should be zero gradient. For the pressure it is vice-versa, as you know, there is no additional pressure at the outlet.

The most interesting part is boundary conditions between your domains. And they depend on the physical processes there. So, what are the processes, that take place at the boundaries between domains?

May 8, 2019, 13:03		#11
sheaker Senior Member Oskar Join Date: Nov 2015 Location: Poland Posts: 184 Rep Power: 11	Hello. I am not using openFoam now, so I cannot reproduce Your case. If I were You I would model just a half of the domain and use symmetry boundary condition. In that case interior part will be well exposed. I don't know if this solution will be suitable for You. Best regards, Oskar __________________ How to set two stroke engine with scavenging? Salome, sliding interface and "Zero length edge detected."

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Pulsatile flow at inlet of pipe model	amsys	CFX	5	July 20, 2016 14:18
Unable to input fluid to flow in a hollow pipe	Mrsimple	CFD Freelancers	3	March 22, 2016 06:18
[snappyHexMesh] Pipe flow / Internal fluid dynamics with SnappyHexMesh	denner	OpenFOAM Meshing & Mesh Conversion	3	October 13, 2011 10:24
My Revised "Time Vs Energy" Article For Review	Abhi	Main CFD Forum	2	July 9, 2002 10:08
Terrible Mistake In Fluid Dynamics History	Abhi	Main CFD Forum	12	July 8, 2002 10:11

May 6, 2019, 13:07		#2
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Hi, The error is division by zero during calculation of fluid kinematic viscosity. It is calculated using dynamic viscosity and density. So the question is, why density of your fluid is zero? It could be due tu your initial conditions or due to supplied thermophysical properties.

May 6, 2019, 13:19		#3
sheaker Senior Member Oskar Join Date: Nov 2015 Location: Poland Posts: 184 Rep Power: 11	Hello. Why did You modeled structure of pipe? It looks like You are only interested in fluid flow. Best regards, Oskar __________________ How to set two stroke engine with scavenging? Salome, sliding interface and "Zero length edge detected."

May 7, 2019, 06:27		#6
Raza Javed Senior Member Raza Javed Join Date: Apr 2019 Location: Germany Posts: 183 Rep Power: 7	One more question here, Why do we use "alpha1" file in the "0" directory? If I want to visualize the fluid flow from a pipe then do I need "alpha1" file? Thank you

May 7, 2019, 06:59		#7
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	It is not quite clear what difficulties you encounter during visualisation. You open case in ParaView, you select your pipe region, you do the visualisation. alpha1 in 0 folder appears in two-phase simulations (eg. interFoam solver). For CHT simulations, usually there is no need in alpha1.

May 7, 2019, 13:29		#9
sheaker Senior Member Oskar Join Date: Nov 2015 Location: Poland Posts: 184 Rep Power: 11	Well... I think that walls are no-slip so velocity is always zero. Try to check velocity in interior part. You don't need to model pipe itself. Just model interior part where fluid flows. Best regards, Oskar __________________ How to set two stroke engine with scavenging? Salome, sliding interface and "Zero length edge detected."

May 10, 2019, 04:17		#12
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Hi, @Raza Javed Select fluid region and use Clip filter to cut it in half (plane should have normal perpendicular to the tube axis). This way you will be able to see what is inside your tube.

May 10, 2019, 11:19		#13
Raza Javed Senior Member Raza Javed Join Date: Apr 2019 Location: Germany Posts: 183 Rep Power: 7	Thank you so much for your reply. It was really helpful. I have one more question related to same geometry. I know the Pressure, Velocity and Temperature of the fluid at the inlet. Now, if due to some reason, some temperature rise from the outside of the pipe occurs, that will also raise the temperature of the fluid, then at the outlet the temperature of the fluid will be different. How can I find the temperature at the outlet? And what boundary conditions for pressure, velocity and temperature would be suitable at inlet and outlet? I shall be very thankful if you can help me out in this. Thank you

May 13, 2019, 06:24		#14
sufjanst Member Join Date: Mar 2016 Posts: 73 Rep Power: 10	There are different ways to find out your outlet temperature. You can simply do it in paraview or you can use the funciton 'sample'. I guess the standard boundary conditions should be fine for your inlet and outlet (fixedValue, inletOutlet, noSlip). I got interested in your thread because you managed to import a Salome Mesh to OpenFOAM. Can you tell me how you did that? I created a mesh but when I try to use ideasUnvToFoam I get the error 'cell type 22 not supported'. I use OpenFOAM 6. Thank you and good luck

May 13, 2019, 06:27		#15
Raza Javed Senior Member Raza Javed Join Date: Apr 2019 Location: Germany Posts: 183 Rep Power: 7	Thank you so much for your reply. Which options/hypothesis did you use while creating a mesh in Salome?

May 20, 2019, 09:03		#17
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Hi, OK. Let's start from the very beginning. Forget about boundary conditions for a minute. Describe your process. You have a flow inside a tube. You have a liquid with constant temperature are one end (inlet). There are heat sources outside the tube. So the following questions should be addressed BEFORE any further discussion about suitable boundary conditions: - Are you interested in temperature distribution inside pipe itself? - What is your Re? - Is distribution of the external heat sources constant? - What flow parameters you have at the inlet? What information you have at the outlet?

May 22, 2019, 17:01		#20
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	OK. We can simulate flow inside the tube as a flow of incompressible fluid. You can simulate is as a laminar flow to start with something (also for turbulence you need better mesh). On your figure there are three regions: tube, heaters, everything else. What is "everything else" (white area on your figure)? What is the mechanism of heat exchange between the heaters and the tube? Concerning inlet and outlet boundary conditions for the tube. For inlet you have a set of fixed values for temperature and velocity. At the outlet you assume, that flow is not disturbed, so values at the outlet faces (for temperature and velocity), should be equal to internal values, hence, it should be zero gradient. For the pressure it is vice-versa, as you know, there is no additional pressure at the outlet. The most interesting part is boundary conditions between your domains. And they depend on the physical processes there. So, what are the processes, that take place at the boundaries between domains?