CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   cavity 3D in OpenFOAM Extend (http://www.cfd-online.com/Forums/openfoam-solving/105176-cavity-3d-openfoam-extend.html)

alquimista July 24, 2012 12:26

cavity 3D in OpenFOAM Extend
 
Hello,

I'm trying to run a cavity 3D case in OpenFOAM Extend, I have change the blockMeshDict of the $FOAM_TUTORIALS/incompressible/icoFoam/cavity tutorial with the next new line:

hex (0 1 2 3 4 5 6 7) (100 100 100) simpleGrading (1 1 1) [as suggested here]

I check that everything works in OpenFOAM-2.1.0 but I obtain the next error in OpenFOAM Extend:

--> FOAM FATAL ERROR:
This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.

From function emptyFvPatchField<Type>::updateCoeffs()
in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 151.

FOAM exiting


Any idea? I'm not especially interested on this case. I just need to make a benchmark with a 3D blocks model from the tutorial.

Thanks in advanced.

owayz July 24, 2012 14:51

What I understand is that you are trying to extend the 2D cavity mesh to 3D.
But the problem is that in 2D the patches normal to direction of flow are given empty BC. And you have increased the number of cells in the normal direction, which means that the mesh is not 2D anymore, but OF sees the empty condition on normal patches and giving an error.
So you need to change these conditions to wall. As you are considering running a 3D cavity simulation.
I hope this will help you.
Regards,
Awais

alquimista July 25, 2012 12:44

Quote:

Originally Posted by owayz (Post 373298)
What I understand is that you are trying to extend the 2D cavity mesh to 3D.
But the problem is that in 2D the patches normal to direction of flow are given empty BC. And you have increased the number of cells in the normal direction, which means that the mesh is not 2D anymore, but OF sees the empty condition on normal patches and giving an error.
So you need to change these conditions to wall. As you are considering running a 3D cavity simulation.
I hope this will help you.
Regards,
Awais

You are right, I dind't check this and the boundary type remains with "empty". Changing it to "wall" solves the problem.

Thank you very much owayz for your time!


PD: Note that with OpenFOAM-2.1.0 there's no error starting the case but it is consider as empty the 3D surfaces.

snowygrouch April 28, 2013 11:54

Extend 2D Cavity to 3D mesh
 
Hi,
I am trying to do the same thing, but when I run "icoFoam"

Anway, it runs, and I go to paraFoam. The box is there looking fine, but U does not change when I run the animation.

http://www.calumdouglas.ch/wp-conten..._3d_Cavity.png

So in other words, when I press play the view above does not change at all.


Changes made to standard case files:

BlockMeshDict:


vertices
(
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
(0 0 1) // this was 0 0 0.1
(1 0 1) // ditto
(1 1 1) // ditto

(0 1 1)
);

blocks
(
hex (0 1 2 3 4 5 6 7) (20 20 20) simpleGrading (1 1 1) // this was 1
);

edges
(
);

boundary
(
movingWall
{
type wall;
faces
(
(3 7 6 2)
);
}
fixedWalls
{
type wall;
faces
(
(0 4 7 3)
(2 6 5 1)
(1 5 4 0)
);
}
frontAndBack
{
type wall; // this was type empty
faces
(
(0 3 2 1)
(4 5 6 7)
);
}
);

mergePatchPairs
(
);



BOUNDARY
(
movingWall
{
type wall;
nFaces 400;
startFace 22800;
}
fixedWalls
{
type wall;
nFaces 1200;
startFace 23200;
}
frontAndBack
{
type wall; // THIS WAS "type empty"
nFaces 800;
startFace 24400;
}
)


P and U


boundaryField
{
movingWall
{
type zeroGradient;
}

fixedWalls
{
type zeroGradient;
}

frontAndBack

type zeroGradient; // this was "empty"
}
}



Any ideas please ?

Many thanks in advance

C.

snowygrouch April 29, 2013 03:31

Versions
 
Sorry some more info:

Am using Paraview and Openfoam as loaded as standard onto CAE Linux 2011.

So thats

Paraview 3.10
OpenFoam 2.0.1

nimasam April 29, 2013 04:01

is there any time directory in your test cases?

if yes! maybe you need to go to display tab in paraview ;) and click on rescale to see the updated value

snowygrouch April 29, 2013 04:22

Many thanks for the reply, I will do that tonight and see if
I get a result.

I do have all the time-step folders in the OFoam cavity folder after
running it, so perhaps its a visualisation issue as you suggest.

snowygrouch May 4, 2013 07:20

it works !
 
Hi,
Its all working now, thanks for the help. :)

I put a load of info on my website about this which might
help openfoam total beginners like me.

http://www.calumdouglas.ch/openfoam-...e-3d-dambreak/

Here is the result:

http://www.youtube.com/watch?v=DB5zWohbSX4


All times are GMT -4. The time now is 23:23.