[linnemann]

Hi

This is directed towards the cfMesh developers.

Is it possible to make a cellZone when meshing?

This is particular usefull when doing MRF or porous simulations.

For a MRF the cylinder zone the interface/boundary must be captured quite accurate.

You already have the primitives ready

objectRefinements
{
    insideTheBody
    {
        cellSize 10;
        type cone;
        p0  (0 0 -32);
        p1  (0 0 32);
        radius0  200;
        radius1  200;
    }

}

What is basically needed would be to have an option

snapMeshToInterface true;

That way the mesh should/could be clipped directly at the interface.

Then we can use the topoSet utility to extract the zone later on.

[WernerW]

Hi Niels,

I'm very interested in what you're trying to do. I'm trying to implement cfMesh for a case with the pimpleDyMFoam solver.

I guess could we do what you say (split meshes) with the command create Baffles that takes a faceZone and generates the master and slave patches. Is that right ?

there's a problem that I'm trying to solve before I try that. How do I define the patch "innerCylinderSmall" with the code inserted in objectRefinements so that I can create the faceZone "InnerCylinderSmall". Did you solve this already ?

Here the content of my createBafflesDict that I took from the openfoam 2.2.x propeller tutorial.

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createBafflesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

internalFacesOnly true;

// Baffles to create.
baffles
{
baffleFaces
{
//- Use predefined faceZone to select faces and orientation.
type faceZone;
zoneName innerCylinderSmall;

patches
{
master
{
//- Master side patch
name AMI1;
type cyclicAMI;
matchTolerance 0.0001;
neighbourPatch AMI2;
transform noOrdering;
}
slave
{
//- Slave side patch
name AMI2;
type cyclicAMI;
matchTolerance 0.0001;
neighbourPatch AMI1;
transform noOrdering;
}
}
}
}

[linnemann]

I guess could we do what you say (split meshes) with the command create Baffles that takes a faceZone and generates the master and slave patches. Is that right ?

Yes, among other things.

But as said above you can not do zones in cfMesh.

It/when that gets in you can do what you want.

Until then we need to split the meshes in two parts and merge them together and make AMI's that way.

[WernerW]

I was able to create a Cellzone and a faceZone in a Cylinder in cfMesh mainly with the aplication createAMIFaces. I paste some relevant files and my Allrun scripts below.

system/createAMIFaces

actions
( { name innerCylinderSmall;
type cellSet;
action new;
source cylinderToCell;
sourceInfo
{
p1 (-0.03 0 0);
p2 (0.12 0 0);
radius 0.3;
}
}
{
name outerCells;
type cellSet;
action new;
source cellToCell;
sourceInfo
{
set innerCylinderSmall;
}
}
{
name outerCells;
type cellSet;
action invert;
}
{
name innerCylinderSmall;
type cellZoneSet;
action new;
source setToCellZone;
sourceInfo
{
set innerCylinderSmall;
}
}
{
name innerCylinderSmallFace;
type faceSet;
action new;
source cellToFace;
sourceInfo
{
set innerCylinderSmall;
option all;
}
}
{
name innerCylinderSmallFace;
type faceSet;
action subset;
source cellToFace;
sourceInfo
{
set outerCells;
option all;
}
}
{
name innerCylinderSmall;
type faceZoneSet;
action new;
source setsToFaceZone;
sourceInfo
{
faceSet innerCylinderSmallFace;
cellSet innerCylinderSmall;
}
}
}

However the cellZone was formed by the cells whose center are in the Cylinder, what gave me a very rough "surface", if you may call it that way. Actually the mesh seems to be ok

When I executed the solver pimpleDyMFoam it actually ran but without rotating the dynamic Mesh and when I ran the moveDynamicMesh App it crashed with an error that I know only too well but do not understand.

$ moveDynamicMesh -checkAMI

Create time
Create mesh for time = 0

Selecting dynamicFvMesh solidBodyMotionFvMesh
Selecting solid-body motion function rotatingMotion
Applying solid body motion to cellZone innerCylinderSmall
Writing VTK files with weights of AMI patches.

Reading surface description:
zNormal
isoQ
rotor

forces forces:
Not including porosity effects

Time = 0.01
solidBodyMotionFunctions::rotatingMotion::transfor mation(): Time = 0.01 transformation: ((0 0 0) (0.999462 (-0.0327941 0 0)))
AMI: Creating addressing and weights between 2481 source faces and 2481 target faces
AMI: Patch source sum(weights) min/max/average = 0.408486, 4.37964, 1.12602
AMI: Patch target sum(weights) min/max/average = 0, 4.27694, 1.12089
--> FOAM Warning :
From function solidBodyMotionFvMesh::update()
in file solidBodyMotionFvMesh/solidBodyMotionFvMesh.C at line 238
Did not find volVectorField U Not updating Uboundary conditions.
Point usage OK.
Upper triangular ordering OK.
Topological cell zip-up check OK.
Face vertices OK.
Face-face connectivity OK.
Mesh topology OK.
Boundary openness (-1.37305e-17 1.1496e-16 3.12531e-16) OK.
Max cell openness = 3.28818e-16 OK.
Max aspect ratio = 8.16767 OK.
Minimum face area = 1.5248e-07. Maximum face area = 0.0105764. Face area magnitudes OK.
Min volume = 5.76824e-11. Max volume = 0.00107641. Total volume = 9.92291. Cell volumes OK.
Mesh non-orthogonality Max: 64.979 average: 14.3117
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 3.11889 OK.
Mesh geometry OK.
Mesh OK.
Calculating AMI weights between owner patch: AMI1 and neighbour patch: AMI2
ExecutionTime = 2.09 s ClockTime = 5 s

--> FOAM FATAL ERROR:

request for volVectorField U from objectRegistry region0 failed
available objects of type volVectorField are
0()

From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/werner/OpenFOAM/OpenFOAM-2.4.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam:bjectRegistry::lookupObject<Foam::Geometric Field<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3 Foam::Q::execute() at ??:?
#4 Foam::OutputFilterFunctionObject<Foam::Q>::execute (bool) at ??:?
#5 Foam::functionObjectList::execute(bool) at ??:?
#6 Foam::Time::run() const at ??:?
#7 Foam::Time::loop() at ??:?
#8 ? at ??:?
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10 ? at ??:?
Aborted (core dumped)

What could be the source of this error ?

[linnemann]

what gave me a very rough "surface",

To have a rotating or sliding mesh you need an almost perfect interface for the AMI.

http://www.openfoam.org/version2.1.0/ami.php

That is why I proposed that cfMesh made something that splits the mesh at the cylinder interface to be able to have really nice interfaces.

[SailorLiu]

Yes. I also use AMI quite a lot and this is a very good proposal. Interested to know if the developers are adding this to the next release.