[louisgag]

Hello all,

I've sucessfully used GGI and AMI in the past to simulate a rotating part within a fixed domain.

Now, I want to know if it is possible to have a rotating mesh embed within another rotating mesh. Has anyone achieved this?

Thanks


-Louis

[minger]

Wow, I was actually getting ready to post the same question. I have looked through the mixer2d tutorials in pimpleDyMFoam and think I have a decent grasp of what's going on there. However, I am hoping to be able to "nest" a rotating zone within another.

[louisgag]

For those wondering if it works, yes it does. I had to do a tiny C++ modification to ensure that the origin of the internal AMI zone rotates with the external one and voilà.
-Louis

[minger]

Would you mind attaching a case zipped up?

[louisgag]

The project is confidential so I can't put all the data online, but it should be fairly easy to replicate.

In my case I modified oscillatingRotatingMotion.C as such,

Foam::solidBodyMotionFunctions::oscillatingRotatingMotion::
transformation() const
{
    scalar t = time_.value();

    vector eulerAngles = amplitude_*sin(omega_*t);

    // Convert the rotational motion from deg to rad
    eulerAngles *= pi/180.0;

    scalar omegaBlop_ =  73.304; // outter AMI zone info
    scalar originBlop_ =  3.048;
    scalar radBlop_ =  0.6096;
    scalar omgOffsetBlop = pi/2; // offset from the right hand axis when simulation starts

    vector blop_ = vector (originBlop_+radBlop_*cos(omegaBlop_*t + omgOffsetBlop),
            originBlop_+radBlop_*sin(omegaBlop_*t + omgOffsetBlop), 0);

//    Info<< "LOUIS: " << blop_ << endl;

    quaternion R(eulerAngles.x(), eulerAngles.y(), eulerAngles.z());
//    septernion TR(septernion(origin_)*R*septernion(-origin_));
    septernion TR(septernion(blop_)*R*septernion(-blop_));

    Info<< "solidBodyMotionFunctions::oscillatingRotatingMotion::"
        << "transformation(): "
        << "Time = " << t << " transformation: " << TR << endl;

And in the dynamic mesh dictionary I ensure that the outer AMI zone angular velocity matches the modified one in the C++ file...

[louisgag]

here is the code for OpenFoam 2.3.x, copy in your user folder and

wmake libso

[louisgag]

Along with a test case from which I removed the confidential data... You will need to change the foil U boundary condition because it is a one I've coded myself...

http://ecbiz103.inmotionhosting.com/...leEmbedAMI.zip

any feedback is welcome !

[diego_angeli]

Hi Louis,

here Diego from UNIMORE. We don't know each other but I think we will soon

I just downloaded your myOscillatingRotatingMotion and the test case, thanks for sharing and congratulations for the nice work.

If it's ok for you I will try to use them on a similar case as yours, for CROP..

I'll let you know ASAP how are we faring on that.

Regards

[louisgag]

Hello Diego,
It will be a pleasure to collaborate with you. Please use this thread to communicate with me so that everyone can follow. Obviously we'll have to avoid confidential project data.
Regards,
-Louis

[diego_angeli]

Hi Louis,
thanks for the support.
So, Andrea and me managed to reproduce a moving mesh analogous to your case, starting from a mesh generated from us with another meshing tool. The workflow is ok on the mesh side.
Now we should work on the boundary condition for U on the foils, then maybe we will come back to you to agree on the case setup.

Best regards

[louisgag]

The link for the test case I had posted above is broken. Please use the following instead: louisgagnon.com/temporaire/exampleEmbedAMI.zip

-Louis

[bullmut]

Hi Louis
from what i read in this thread i think i am trying to achieve the same thing.
I am trying to implement you test case and have compiled your libmyDynamicFvMesh.so
However when i run the case it is trying to load "libmyFiniteVolume.so", to allow for the definition of your foils as patch type myMovingWallSlip. Can you explain your modification in the making of this patch type of supply files for the wmake of the latter .so ?

Regards

[louisgag]

Hi Gareth,

I choose to use a boundary condition that imposes a slip and respects the moving wall velocity for my simulation: http://www.cfd-online.com/Forums/ope...tml#post509989

You can use another boundary condition if you prefer...

Regards,


-Louis

[bullmut]

Hi Louis

Thanks for the info and explanation.
I was trying to run the code as is, with minimal alterations. But i get what you mean by a different BC.

Thanks again for the code. Kinda what i needed, but definitely a step in the right direction.

Regards

[louisgag]

Dear Everyone,
I've created a GitHub repository with the updated version of the code and test case for OpenFOAM-4.x
https://github.com/louisgag/OpenFOAM-embedded-AMI
Enjoy,
-Louis