[schmittp54]

Hello,
I am looking for information about the required order of faces in the faceList when using the constructor

fvMesh(const IOobject &io, const Xfer< pointField > &points, const Xfer< faceList > &faces, const Xfer< labelList > &allOwner, const Xfer< labelList > &allNeighbour, const bool syncPar=true)

.

The following code fragment creates two connected hexahedrons with dimensions (dx,dy,dz)=(0.5,1,1) each. ParaView shows that an extra vertex has been created (first attached image).
If I reorder the faces 0..5 as shown in the commented section of the code, the paraFoam output looks good (second attached image).

Why is the order of the argument "const Xfer< faceList > &faces" relevant, and is the correct order documented anywhere?

Thanks
Patricia

Here is the code fragment, which creates a fvMesh from a pointField, faceList, owner and neighbour list:

pointField p(12);
p[0]=vector(0,0,0);
p[1]=vector(.5,0,0);
p[2]=vector(1,0,0);
p[3]=vector(0,1,0);
p[4]=vector(.5,1,0);
p[5]=vector(1,1,0);

p[6]=vector(0,0,1);
p[7]=vector(.5,0,1);
p[8]=vector(1,0,1);
p[9]=vector(0,1,1);
p[10]=vector(.5,1,1);
p[11]=vector(1,1,1);

faceList f(11);
forAll(f,fI) f[fI]=face(4);

f[0][0]=0;f[0][1]=3;f[0][2]=4;f[0][3]=1;
f[1][0]=1;f[1][1]=4;f[1][2]=10;f[1][3]=7;
f[2][0]=6;f[2][1]=7;f[2][2]=10;f[2][3]=9;
f[3][0]=0;f[3][1]=6;f[3][2]=9;f[3][3]=3;
f[4][0]=3;f[4][1]=9;f[4][2]=10;f[4][3]=4;
f[5][0]=0;f[5][1]=1;f[5][2]=7;f[5][3]=6;
/*
f[0][0]=1;f[0][1]=4;f[0][2]=10;f[0][3]=7;
f[1][0]=3;f[1][1]=9;f[1][2]=10;f[1][3]=4;
f[2][0]=0;f[2][1]=6;f[2][2]=9;f[2][3]=3;
f[3][0]=0;f[3][1]=1;f[3][2]=7;f[3][3]=6;
f[4][0]=0;f[4][1]=3;f[4][2]=4;f[4][3]=1;
f[5][0]=6;f[5][1]=7;f[5][2]=10;f[5][3]=9;
*/
f[6][0]=1;f[6][1]=4;f[6][2]=5;f[6][3]=2;
f[7][0]=2;f[7][1]=5;f[7][2]=11;f[7][3]=8;
f[8][0]=7;f[8][1]=8;f[8][2]=11;f[8][3]=10;
f[9][0]=4;f[9][1]=10;f[9][2]=11;f[9][3]=5;
f[10][0]=1;f[10][1]=2;f[10][2]=8;f[10][3]=7;

labelList owners(11);
for (int i=0;i<6;i++) owners[i]=0;
for (int i=6;i<11;i++) owners[i]=1;
labelList neighbours(1);
neighbours[0]=1;

fvMesh *mesh=new fvMesh(
Foam::IOobject
(
Foam::fvMesh::defaultRegion,
"constant",
runTime,
Foam::IOobject::NO_READ
),
p,f,owners,neighbours
);
mesh->write();

[herbert]

Hi Patricia,

I haven't worked with this constructor yet, but in general the internal faces of a mesh have to be on top of the faceList (in your case only the face 4(1 4 10 7), therefore it must be the first element). I'm not sure, if the order of the boundary faces is important, too, but you can check (just make sure, that the internal face is the first one).

In addition the faces should be defined obeying the right-hand-rule but you have already done this way.

Regards,
Stefan

[schmittp54]

Thank you, Herbert

after reading your reply I have also found this explanation in the Wiki:

faces for each face an ordered list of point labels. The normal (righthand rule) should point away from the owner cell (so the boundary faces point out of the domain)
The face ordering is quite intricate:
- internal faces get ordered such that when stepping through the higher numbered neighbouring cells in incremental order one also steps through the corresponding faces in incremental order (upper-triangular ordering)
- boundary faces are bunched per patch. The boundary file then tells where the start and size of the patch are in the faces list. For coupled faces there is an additional ordering inside the patch:

• cyclics: should be ordered such that face 'i' is coupled to face 'i + size()/2' where size() is the number of faces of the patch. Additionally the 0th point of a face is considered coupled to the 0th point of its coupled face.

• processor: should be ordered such that face 'i' on one processor is coupled to face 'i' on the neighbouring processor. Same additional constraint on the order of the points in a face as cyclics.

Both your answer and the wiki explain why my ordering was wrong.

Thanks
Patricia