[MechaZ]

Hello everyone,

I previously worked on ANSA with static meshes just fine ! Now, I am trying to make a dynamic mesh by using nonConformalCouple BC type.
The tutorial case in openFOAM uses Baffles to create two neighboring patches and rotate one relative to the other.
Long story short I couldn't use the feature ANSA offers for dynamic mesh (it exports as a regular patch) so I'm trying to create a baffles that I'll split manually with openFOAM code. faceZones file is empty when I export from ANSA (the code takes a facezone and duplicates it to rotate one and fix the other), while my PIDs are set correctly somehow it doesn't export faceZones (I'm not even 100% sure I need faceZones) and the boundary file is also weirdly defined, here's the boundary file :

FoamFile
{
	version 2.0;
	format binary;
	class polyBoundaryMesh;
	location "";
	object boundary;
}
/*---------------------------------------------------------------------------*/
/*---------------------------------------------------------------------------*/


4
(

	MovingWall
	{
		type wall;
		startFace 157169;
		nFaces 256;
	}

	InnerCylinder       // the faceZone or surface i want to rotate
	{
		type wall;                 // PID is set to be baffle, why is it wall idk !
		startFace 157425;
		nFaces 1982;
	}

	InnerCylinder_shadow    // Somehow a shadow was created 
	{
		type wall;               // it's a good sign but idk where i'll need it
		startFace 159407;
		nFaces 1982;
	}

	Farfield
	{
		type patch;
		startFace 161389;
		nFaces 378;
	}

)

If you have any idea on how to set up dynamic mesh in ANSA for openFOAM I'd be grateful for your help. Please tell me if I'm completely heading in the wrong direction here !

[tomf]

Hi,

Not sure if there is an option to use the NCC directly from ANSA, but if you want to export the surfaces as faceZones you have to set the ANSA type to internal and have the checkBox use in model checked.

For the ESI versions there are options to setup the cyclicAMI in ANSA, but you need to make sets of faces, its a bit too complicated to explain in a single post.

Now you have basically two baffles in your exported mesh, maybe some mesh manipulation tools (createPatch/createBaffles?) in OpenFOAM can create the NCC from the baffles, or from the faceZones if you export them as such?

Regards,
Tom

[MechaZ]

Originally Posted by tomf

Hi,

Not sure if there is an option to use the NCC directly from ANSA, but if you want to export the surfaces as faceZones you have to set the ANSA type to internal and have the checkBox use in model checked.

For the ESI versions there are options to setup the cyclicAMI in ANSA, but you need to make sets of faces, its a bit too complicated to explain in a single post.

Now you have basically two baffles in your exported mesh, maybe some mesh manipulation tools (createPatch/createBaffles?) in OpenFOAM can create the NCC from the baffles, or from the faceZones if you export them as such?

Regards,
Tom

Thank you Tom for answering my post, your solution seems to solve my problem.
I've put this project on hold and continued with other work that's why I'm only answering now, here's how this solves my issue (for future reference) :

I did as you said and set the ANSA type as internal, making sure the use in model is checked. This wrote the faceZones I needed, next I ran these commands that call the proper files :

> createBaffles -overwrite

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  11
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    object      createBafflesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

internalFacesOnly true;

baffles
{
    nonCouple
    {
        type        faceZone;
        zoneName    innerCylinder;

        patches
        {
            owner
            {
                name        nonCouple1;
                type        patch;
            }

            neighbour
            {
                name        nonCouple2;
                type        patch;
            }
        }
    }
}

> splitBaffles -overwrite

(note : I don't have a splitBafflesDict file, as I understand it, it's a function that openFOAM knows, where in opposition, to create them (baffles) OF needs to know the names and original patches etc...)

> renumberMesh -noFields -overwrite

(note : as I understand it, this edits the U, P, Epsilon... files to have the correct BC)

> createNonConformalCouples -overwrite nonCouple1 nonCouple2

> decomposePar -noFields

(for parallel run where you specify the number of cores in the next command)

> mpirun -np 6 pimpleFoam -parallel

> reconstructPar

I hope that this might help someone who is experimenting with dynamic meshes for the first time, just like me.

kind regards,
Zack