[williamsj0165]

Good afternoon,

I am attempting to build and run a simple 2D simulation that consists of a rotating cylinder in crossflow. My goal is to study the effect of cylinder rotation on vortex shedding at certain Re.

For the simpler case of a static cylinder, I am able to build and refine a mesh using blockMeshDict and blockMesh. (See attachment for an image of the unrefined mesh.) With a refined mesh, the simulation runs perfectly.

However, I am hung up on adding rotational velocity to the central cylinder. In order to do this, I believe that I must implement the rotatingWallVelocity condition in my 0/U file:

For the static case:

cylinder 
{
    type            fixedValue;
    value           uniform (0 0 0);
}

For the rotating case:

cylinder 
{
    type            rotatingWallVelocity;
    origin		(0 0 0);
    axis		(0 0 1);
    omega		100;
}

However, I am not clear on if I need to modify my blockMeshDict file as well. To my understanding, the file 0/U contains the initial conditions for the velocity, but blockMeshDict is information about the mesh itself, including boundary conditions. I would have thought that I would need to modify blockMeshDict as well:

For the static case:

cylinder
{
    type wall;
    faces
    (

    (0  32  33   1)
    (1  33  34   2)
    (2  34  35   3)
    (3  35  36   4)
    (4  36  37   5)
    (5  37  38   6)
    (6  38  39   7)
    (7  39  32   0)

    );
}

For the rotating case:

cylinder
{
    type	rotatingWallVelocity;
    origin	(0 0 0);
    axis	(0 0 1);
    omega	100;

    faces
    (

    (0  32  33   1)
    (1  33  34   2)
    (2  34  35   3)
    (3  35  36   4)
    (4  36  37   5)
    (5  37  38   6)
    (6  38  39   7)
    (7  39  32   0)

    );
}

Other threads I have viewed that discuss similar situations make no mention of modifying the blockMeshDict file. Any guidance on this issue would be much appreciated. Also, do I need to make any modification to my 0/p file?

[Krapf]

Hi williamsj0165

You don't need to modify blockMeshDict. There you only define the patch type, which is still wall. Take a look here: OpenFOAM v8 User Guide: 5.2 Boundaries.
After the mesh creation you'll find the patch type in constant/polyMesh/boundary.

Because it's still a wall, you don't need to change the pressure boundary condition.

Kind regards
Krapf

[simrego]

Hi!


It is not always true. There are some cases where for example a utility can be called on wall types only. And there could be other stuff too. If it is possible, then set the boundary types properly. If it is a wall, create a wall type. If it is an inlet/outlet, create a patch type. It is not a big work. But of course if a wall will be changed to a wall but with a different BC, it will be still a wall.
And it is also important to set properly if you have some "special" types like cyclic or cyclicAMI, symmetry, etc...

And to clarify. In the 0/files you can set the initial and boundary condition. In the blockMesh dict you set the boundary type which is not equal to the boundary condition.

[williamsj0165]

Hi Krapf, simrego,

Thank you both so much for your responses, they clarified the difference between the purpose and significance of blockMeshDict vs. 0/U etc. files.

Your explanations were very helpful! and I was able to run a few successful simulations. Thanks again!