[zhangxc0223]

Hi, I am building a simple model for a fully turbulent flow passing through a pipe. My idea is to use the “turbulentInlet” type at the inlet to achieve a random turbulence, and then to let the flow go through a long enough pipe, to achieve fully developed turbulence at the end of the pipe.

However, the model I built doesn’t show an expected result. The movement of turbulent flow is just on the plane of inlet, like it’s showing in the picture 1. How to let the turbulence go along the pipe?

1.jpg
picture 1

By the way, in the results of mine, at the time step of 0.001, the velocity of flow is -10m/s all over the pipe (picture 2 and 3). Is this reasonable? And why? The length of my pipe is 200m, the velocity of the flow is -10m/s. The deltaT and writeInterval I used in controlDict are 0.001 and 1 respectively.

00.jpg
picture 2. the velocity of t=0

11.jpg
picture 3. the velocity of t=0.001

The code of U is as follows and the icoFoam is used in this model.

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    inlet0
    {
        type            turbulentInlet;
        referenceField uniform (0 -10 0);
        fluctuationScale (0.5 0.5 0.5);
        value uniform (0 -10 0);
    }
    outlet
    {
        type            pressureInletOutletVelocity;
        inletValue      uniform (0 0 0);
        value           uniform (0 0 0);
    }
    sideWall
    {
        type            zeroGradient;
    }
}

Are there any faults in my code for achieving a turbulence? I would very appreciate for your answers.

[RobertHB]

icoFoam solves the incompressible laminar Navier-Stokes equations using the PISO algorithm.

From openfoamwiki.net.
So i guess your solver might not be able to support turbulence. Have you tried transient turbulent solvers like pisoFoam? And remember to include a turbulence model (RAS/LES) in your turbulenceProperties.dict.

[zhangxc0223]

Originally Posted by RobertHB

From openfoamwiki.net.
So i guess your solver might not be able to support turbulence. Have you tried transient turbulent solvers like pisoFoam? And remember to include a turbulence model (RAS/LES) in your turbulenceProperties.dict.

Really thank you for your answer. I would like to ask, can I use icoFoam as an DNS model for solving the model? If so, what should I modify in the solver? If not, what can I use for a DNS turbulance model?

[RobertHB]

I think the DNS solver of OpenFOAM is called dnsFoam. Additionally there are multiple threads on this forum about DNS calculations [1] [2] [3]. Maybe those are helpful.

[ykanani]

Originally Posted by zhangxc0223

Really thank you for your answer. I would like to ask, can I use icoFoam as an DNS model for solving the model? If so, what should I modify in the solver? If not, what can I use for a DNS turbulance model?

You are correct Mattew. You can do that but DNS needs very fine grids to resolve nearly all turbulence scales and I believe that your grid is surprisingly coarse. That is one issue. The second issue is that the random fluctuations are far from the real turbulence and hence decay very fast. You can try other methods like the one proposed by Jarrin. Search synthetic eddy method. There is a very similar method called Lemos inflow generator (developed under Openfoam).

Just search for inflow turbulence generator and you will find various methods and research on this.
I also suggest that you familiarize yourself more with turbulence to get better idea about length scales.

Without using those methods, my suggestion is to refine the grid in all directions and increase the intensity of inflow turbulence.

Robert- you are also right the only dedicated solver for DNS in OpenFOAM is dnsFoam. But that is for decaying homogeneous isotropic turbulence. I believe other solvers can be used for DNS as long as:
-there is no turbulence modeling
-mesh requirements are met
-proper schemes are used

Regards,