[mahtin360]

Hi,

I've been working on simulating flow past a rotor using PimpleDyMFoam for a while now and got everything working so far.

Now I'm trying to add a second rotor to my case and run into troubles rotating both at the same time. It seems from a few test cases, with up to 4 AMI zones, that only the AMI zone that is last mentioned in my case files is actually rotating.
Has anyone managed to have seperate rotating regions within a single domain, what is the correct way of defining the dynamic mesh regions?
Any input would be much appreciated.


Edit: Just came across multiSolidBodyMotionFvMesh. I'll leave this here as I did not come across much mentioning of this, maybe someone else will stumble over this and find it helpful.

This is the changed dynamicMeshDict for multiple AMI (slightly changed format compared to before)

dynamicFvMesh   multiSolidBodyMotionFvMesh;

motionSolverLibs ( "libfvMotionSolvers.so" );

multiSolidBodyMotionFvMeshCoeffs
{
    cylinder
    {
      solidBodyMotionFunction  rotatingMotion;
    rotatingMotionCoeffs
    {
        origin      (0 0 0);
        axis        (1 0 0);
        omega       -110; // rad/s
    }
    }

    cylinderR
    {
    solidBodyMotionFunction  rotatingMotion;
    rotatingMotionCoeffs
    {
        origin      (0.84 0.42 0);
        axis        (1 0 0);
        omega       -110; // rad/s
    } 
    }
    
    cylinderL
    {
    solidBodyMotionFunction  rotatingMotion;
    rotatingMotionCoeffs
    {
        origin      (3.36 0.84 0);
        axis        (1 0 0);
        omega       -110; // rad/s
    }
    }
}

Regards,
Martin

[Simone81]

Hi,

I am having the same issue, did you manage to solve it?

Thank you!

[donQi]

Hello,

in OpenFOAM1712 (https://www.openfoam.com/releases/openfoam-v1712/)
you can find the tutorial
OpenFOAM/OpenFOAM-v1712/tutorials/mesh/moveDynamicMesh/relativeMotion

inside take a look at the file :
OpenFOAM-v1712/tutorials/mesh/moveDynamicMesh/relativeMotion/box2D_moveDynamicMesh/constant/dynamicMeshDict

You need to put your rotating components inside the "dynamicMultiMotionSolverFvMeshCoeffs" subdictionary.
For convenience I copy below the dictionary

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  plus                                  |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      dynamicMeshDict;
}

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

dynamicFvMesh dynamicMultiMotionSolverFvMesh;   //dynamicMotionSolverFvMesh;


// Specification of rotation around centre
rotation1
{
    solidBodyMotionFunction  rotatingMotion;
    rotatingMotionCoeffs
    {
        origin      (0 0 0);
        axis        (0 0 1);
        omega       10; // rad/s, 1rad/s=9.5rpm
    }
}


dynamicMultiMotionSolverFvMeshCoeffs
{
    rotor1
    {
        solver solidBody;
        cellZone rotor;
        solidBodyCoeffs
        {
            $rotation1;
        }
    }

    dualWing1
    {
        cellZone dualWing;

        // Solve displacement on top of solid-body rotation
        solver solidBodyDisplacementLaplacian;

        solidBodyDisplacementLaplacianCoeffs
        {
            solidBodyMotionFunction  multiMotion;
            multiMotionCoeffs
            {
                rotation_1
                {
                    $rotation1;
                }
                rotation_2
                {
                    // Apply counter rotation to keep dualWing aligned
                    solidBodyMotionFunction rotatingMotion;
                    rotatingMotionCoeffs
                    {
                        origin      (-0.43 0 0);
                        axis        (0 0 1);
                        omega      -10; // rad/s, 1rad/s=9.5rpm
                    }
                }
            }
            diffusivity quadratic inverseDistance (wing2);
        }
    }
}

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

So for example if you want to simulate a flying object with 2 rotors, like an chinook helicopter for example, the dictionary will be:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  plus                                  |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      dynamicMeshDict;
}

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

dynamicFvMesh dynamicMultiMotionSolverFvMesh;  

dynamicMultiMotionSolverFvMeshCoeffs
{
    rotor1
    {
        solver solidBody;
        cellZone cylinder1;
        solidBodyCoeffs
        {
            solidBodyMotionFunction  rotatingMotion;
            rotatingMotionCoeffs
            {
                origin      (5 0 0);
                axis        (0 0 1);
                omega       100; // rad/s, 1rad/s=9.5rpm
            }
        }
    }

    rotor2
    {
        solver solidBody;
        cellZone cylinder2;
        solidBodyCoeffs
        {
            solidBodyMotionFunction  rotatingMotion;
            rotatingMotionCoeffs
            {
                origin      (-5  0  0);
                axis        (0  0 1);
                omega       -100; // minus 100 since contra-rotating blades 
            }
        }
    }   
}

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

[mahtin360]

In addition to the details given by Al, I had issues with my mesh generation and the specification of the AMI surfaces. What happened was that the cells were still attached to each other and deformed with each step of rotation, leading to the calculation to fail after a while (my time steps were very small).

Using mergeOrSplitBaffles -split -overwrite solved the issues for me.

[bksuman]

I tried the given multi rotor library with openFoam 7, and it is showing error, may you please let me know on which version of this library is accessible.


Thank you