[mahendra]

Dear Foamers

I am having an annulus mesh with 90 degree sector. The faces on the sector are defined as cyclicGgi and bottom is specified as inlet with some velocity and the top as outlet with zero pressure.

when I am running simpleFoam, it solves for Ux, Uy and Uz for one iteration and when it comes for pressure, it is exiting the simpleFoam application.

Please can anyone help me with this.

This is my boundary file:

6
(
per2
{
type cyclicGgi;
nFaces 1000;
startFace 34160;
shadowPatch per1;
zone right;
separationOffset (0 0 0);
rotationAxis (0 0 1);
rotationAngle 90; // Degrees
bridgeOverlap off;
}
per1
{
type cyclicGgi;
nFaces 1000;
startFace 35160;
shadowPatch per2;
zone left;
separationOffset (0 0 0);
rotationAxis (0 0 1);
rotationAngle 0; // Degrees
bridgeOverlap off;
}
bottom
{
type wall;
nFaces 240;
startFace 36160;
}
top
{
type wall;
nFaces 240;
startFace 36400;
}
wall
{
type wall;
nFaces 600;
startFace 36640;
}
shaft
{
type wall;
nFaces 600;
startFace 37240;
}
)


U file:

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

internalField uniform ( 0.0 0.0 0.0 );

boundaryField
{
per2
{
type cyclicGgi;
value uniform (0 0 0);
}
per1
{
type cyclicGgi;
value uniform (0 0 0);
}
bottom
{
type fixedValue;
value uniform (0 0 0.01);
}
top
{
type zeroGradient; //fixedValue;
//value uniform (0 0 0);
}
wall
{
type fixedValue;
value uniform (0 0 0);
}
shaft
{
type fixedValue;//rotatingWallVelocity;
// origin (0 0 0);
// axis (0 0 1);
// omega 10;
value uniform (0 0 0);
}
}

p file:

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0.0;

boundaryField
{
per2
{
type cyclicGgi;
value uniform 0;
}
per1
{
type cyclicGgi;
value uniform 0;
}
bottom
{
type zeroGradient;
}
top
{
type fixedValue;
value uniform 0;
}
wall
{
type zeroGradient;
}
shaft
{
type zeroGradient;
}
}


and this is the output in the console

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model laminar

Starting time loop

Creating ggi check
Time = 201

smoothSolver: Solving for Ux, Initial residual = 0.20210891, Final residual = 0.0001459087 1, No Iterations 11
smoothSolver: Solving for Uy, Initial residual = 0.2028729, Final residual = 0.00014988579 , No Iterations 11
smoothSolver: Solving for Uz, Initial residual = 4.9124799e-08, Final residual = 4.9124799 e-08, No Iterations 1
openfoam-1.5-dev@Clust7:


Thanks
Mahendra.

[hjasak]

Doh!

per2: rotation angle = 90;
per1: rotation angle = 0;

See the problem? Please switch on some GGI debugging, which will produce a VTK file of the original and transformed cyclic GGI surface and then look at it in paraview: they should be on top of each other.

Also, there is a check in the source code which says:

if
(
(mag(rotationAngle()) - mag(cyclicShadow().rotationAngle())) > SMALL
|| cmptSum(rotationAxis() - cyclicShadow().rotationAxis()) > SMALL
)
{
FatalErrorIn("void cyclicGgiPolyPatch::check() const")

Therefore, your case with the boundary file you listed above WILL fail.

Hrv

[mahendra]

Hello Sir,

My case started working after looking into the code and changing the rotation angle in the boundary file.

per2: -90
per1: 90

Thanks and Regards
Mahendra

[enry]

Hi prof Hrvoje Jasak,
first of all Thank you for the 1.5-dev development.
Sorry if I write here but I need to ask you a simple question: Can I use RealizableKE model for turbulent simulation involving Ggi?
I know from FLUENT manual that :
"One limitation of the realizable k- model is that it produces non-physical turbulent
viscosities in situations when the computational domain contains both rotating and sta-
tionary fluid zones[...] In FLUENT, the term −2 ijk ωk is, by default, not included in the calculation of Ωij . This is an extra rotation term that is not compatible with cases involving sliding meshes or multiple reference frames."

So I understand that in FLUENT I can use RealizableKe model without any problems, even if I use sliding interface, because the extra rotation term is not included by default in calculation.
What about OF 1.5-dev?
Thanks in advance.
Regards.
Enry.