[FlyBob91]

Hello to all,
i have to simulate the flow in a duct and to save some time i saw many people use periodic boundary conditions at the inlet and outlet.
Now i set them correctly in the blockMeshDict

    inlet
    {
        type cyclic;
        neighbourPatch  outlet; 
        faces
        (
            (0 4 7 3)
        );
    }

    outlet
    {
        type cyclic;
        neighbourPatch  inlet;
        faces
        (
            (1 2 6 5)
        );
    }

but i don't know how to set them in the initial condition file. I know the entry velocity but what should i do with the other conditions?


Thanks for help,
Roberto

[arvindpj]

Here are some possible options:

Originally Posted by ngj

Hi Jitender

Another approach is to look in the example

~/OpenFOAM/OpenFOAM-1.6.x/tutorials/incompressible/pisoFoam/les/pitzDailyDirectMapped

where a mapping procedure is carried out between to planes with a given offset between them. The profile from the interior plane is mapped back on to the inlet, hence between these two planes you basically have an infinitely long pipe, and since you are considering laminar flows, then the distance between the two planes is of minor importance as far as the validity of the velocity (and turbulence) profile(s) goes.

I have some nice pictures of a laminar jet in a laminar cross flow on which I performed a POD-analysis, so if you are interested in seeing the results just drop me an email.

Happy New Year,

Niels

Originally Posted by wenterodt

If you want to simulate a fully developed channel flow in constant cross sections or in a periodically repeating geometry, the cyclic boundary condition for the U-field is what you need. The easiest way to prescribe a pressure drop between inlet and outlet is to use the fan-boundary condition. I.e. in constant/polyMesh/blockMeshDict use e.g.

cyclic inout
  (
    (4 7 3 0)
    (6 5 1 2)
  )

Then in 0/U

  inout
  {
    type cyclic;
    value uniform (0 0 0);
  }

In 0/p write

inout
  {
    type fan;
    patchType cyclic;
    f List<scalar> 1(-0.005); // p_OF = p_real / rho
    value uniform 0;
  }

and mind that the OpenFOAM pressure is divided by the density in incompressible flow. The pressure drop (here 0.005*rho) that is needed for a certain mean velocity can be calculated by the Poisseuille number (if available) or must be guessed and then corrected. (Yes, I know there is channelFoam, but I cannot recommand that for various reasons.)
Here the "value"-entries are only used for the first iteration (and to prevent paraFoam from crashing) and are then overwritten.
Good luck!

[FlyBob91]

Hi arvindpj,
hanks for your reply


I don't understand 3 things about your suggestion comment,

1) why he used only one name for both inlet and outlet and how they are defined. I would like to take them saparated because i have to extract the velocity profile at the outlet

2) why the velocity is null

3) and this part in the p boundary condition

f List<scalar> 1(-0.005); // p_OF = p_real / rho

[arvindpj]

I don't understand 3 things about your suggestion comment,

1) why he used only one name for both inlet and outlet and how they are defined. I would like to take them separated because i have to extract the velocity profile at the outlet

There are inlet and outlet present. This set-up corresponds to a flow through a duct driven by a fan in the middle. inout in the previous post is the cyclic patch in the middle.

The inlet and outlet U bc's are:

 
     inlet           
    {
        type            pressureInletVelocity;
        phi             phi;
        value           uniform (0 0 0);
    }

    outlet          
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           uniform (0 00 0);
    }

2) why the velocity is null

Velocity is not NULL, it's BC is cyclic. and value uniform (0 0 0); is a place holder and is overridden.

3) and this part in the p boundary condition

f List<scalar> 1(-0.005); // p_OF = p_real / rho

The f above is a list of polynomial coefficients in the pressure jump definition

delta p = f_1 + f_2 * v + f_3 * v^2 + ...

Above only f_1 is assigned, f_1 = -0.005

[FlyBob91]

Many thanks arvindpj, you are opening me a world but, unfortunately, i haven't understand yet the p boundary condition.
Is the f_1 value constant or should i calculate it? Is the condition the same for both inlet and outlet?

As i mentioned the only data i know is the inlet velocity and and the flow rate.

Sorry for my multiple questions

[arvindpj]

Originally Posted by FlyBob91

Many thanks arvindpj, you are opening me a world but, unfortunately, i haven't understand yet the p boundary condition.
Is the f_1 value constant or should i calculate it? Is the condition the same for both inlet and outlet?

As i mentioned the only data i know is the inlet velocity and and the flow rate.

Sorry for my multiple questions

Could you describe a little bit more about your problem? What are you trying to achieve?

[FlyBob91]

Originally Posted by arvindpj

Could you describe a little bit more about your problem? What are you trying to achieve?

Sure

As you can see, thanks to the image i liked, my problem is a simple 3D channel with the flow that followes the y-direction. The flow enters throught the inlet with a velocity of 0.42 m/s and this is the only data i know.

Now my aim is to find the outlet velocity profile with a fully developed boundary layer.
Because the length of the channel is very large, my professor suggested to me to use a periodic boundary condition to save time during the calculation. In this manner i could use a not so long channel and obtain the fully developed flow saving time.

Then i have to use the outlet velocity profile as inlet profile in a second simulation (but this is another problem).

I hope to have been clear.

[FlyBob91]

Sorry for the bump

[arvindpj]

Originally Posted by FlyBob91

Sorry for the bump

Opps!

In order to get a fully developed velocity profile at outlet bc, using the mapped bc would suffice.

In blockMeshDict:

 inlet
    {
        type mappedPatch;
        offsetMode      uniform;
        offset          (2 0 0);  // Plane to be mapped
        sampleRegion    region0;
        sampleMode      nearestCell;
        samplePatch     none;
        faces
        (
            (0 4 7 3)
        );
    }

In 0/U:

    inlet
    {
        type            mapped;
        field           U;
        setAverage      1;
        average         (0.1335 0 0);  // Velocity Magnitude
        interpolationScheme cell;
        value           uniform (0.1335 0 0);
    }

Attached is a sample 2D Channel Flow case with Mapped inlet. This is similar to the pitzdaily tutorial, I had mentioned in my earlier post.

Cheers,

[FlyBob91]

Many thanks arvindpj
i'll test it as soon as possible.

Best regards,
Roberto