CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... (http://www.cfd-online.com/Forums/openfoam-meshing-other/)
-   -   Usage of createPatchDict (http://www.cfd-online.com/Forums/openfoam-meshing-other/107664-usage-createpatchdict.html)

Bombolati October 3, 2012 10:55

Usage of createPatchDict
 
Hi, yesterday I opened a thread with a problem with the utility foamToVTK, and this shows me a new problem about my mesh. Bruno Santos (the moderator) gives me a valuable advice to check my mesh with checkMesh utility. And for my particular boundary condition says me to looking for a thread useful for me with the keywords foam3DMeshToFluent cyclic.
Now I've read the forum with this keywords but in every thread with cyclicle boundary condition problems the problem is not solved. I'm unlucky!
So I want to summarize the problem.
I convert the mesh with fluent3DMeshToFoam. ok.
I run the checkMesh utility and there isn't a problem yet. ok.
Now I need to change some patch from type patch to type cyclic.
The first time I have changed directly the boundary file with this keywords for the patch 1:
matchTolerance 0.0001; neighbourPatch patch 2; transform rotational; rotationAxis (0 0 1); rotationCentre (0 0 0);
for the patch 2:
matchTolerance 0.0001; neighbourPatch patch 1; transform rotational; rotationAxis (0 0 1); rotationCentre (0 0 0);
This attempt give the error above when I run the checkMesh utility.
Now I'm trying to use the createPatch utility but I don't understand which is its behaviour. I have find the example between the OF file but it isn't clear.
I try to explain what I have understand. This is the createPatchDict that I have done.

{
name patch1 (The patch name that I want change);
patchInfo (this is the section in which i set the new patch features)
{
type cyclic;
neighbourPatch patch2;
transform rotational;
rotationAxis (0 0 1);
rotationCentre (0 0 0);
}
constructForm patches (I have no idea what is this keyword);
patches (periodic1) (I have no idea);
}
{
name patch2 (The patch name that I want change);
patchInfo (this is the section in which i set the new patch features)
{
type cyclic;
neighbourPatch patch1;
transform rotational;
rotationAxis (0 0 1);
rotationCentre (0 0 0);
}
constructForm patches (I have no idea what is this keyword);
patches (periodic1) (I have no idea);
}

If I run the utility it starts and have finish with a warning that says:in file meshes/polymesh/polyBoundaryMesh/polyboundaryMesh.c at line 573 OF can't find any patch names matching periodic1
This error occurs two times. The funny things is that this utility doesn't convert any patch in my boundary file, but create a directory named 1e-07 (as the value of deltaT in the controlDict file) in which there is an other polyMesh directory that contains the same file of that one in the constant directory.

Please help me, I'm looking for a solution all day in the forum, please forgive any grammatical errors I'm so tired. Thanks a lot.

blacksquirrel October 4, 2012 04:00

Hello Bombolati,

After using fluent3DMeshtoFoam you have two patches ("patchA" and "patchB") which should be cyclic but are labeled with "patch" or "wall".
Then you can use the createPatch utility.

In the createPatchDict you write
name patch1;
this is the new name of your cyclic patch

patchInfo (this is the section in which i set the new patch features)
{
type cyclic;
neighbourPatch patch2;
transform rotational;
[...]

constructFrom patches;
which means, that there are existing patches that are used to create the new patches. (It is possible to create patches from faces, then you have to write construct from faceSet)
and
patches (patchA)
which means, your new cyclic patch "patch1" is constructed from "patchA" (it is possible to construct a new patch from two or more existing patches)

and the same then for patch2:
constructFrom patches;
patches (patchB) ;

Bombolati October 4, 2012 05:52

Thank you very much blacksquirrel, the conversion is ok and the checkMesh utility gives no error.

sivakumar October 5, 2012 14:59

Hi there,
I have converted the .msh in to foam.
I got 2 errors,
firstly as follows,

--> FOAM FATAL ERROR:
face 6439 area does not match neighbour by 0.0103693% -- possible face ordering problem.
patch:OLR0 my area:0.000199448 neighbour area:0.000199427 matching tolerance:0.0001
Mesh face:1370739 fc:(0.0966635 -0.0215988 0.729129)
Neighbour fc:(0.0967883 -0.5304 0.500736)
If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.
Rerun with cyclic debug flag set for more information.

then I have increased the matchTolerance 0.0001 to 0.001
then executed paraFoam

after that I am getting the error as follows,



--> FOAM FATAL ERROR:
More than six unsigned transforms detected:
6(((0 0 0) (1 1.57813e-06 -0.000193506 -0.000137946 0.707107 -0.707107 0.000135714 0.707107 0.707107) 1) ((0 0 0) (0.999999 3.64383e-05 -0.00152133 -0.00110151 0.707109 -0.707104 0.00104998 0.707105 0.707108) 1) ((0 0 0) (0.999996 7.7863e-05 -0.00275828 -0.00200544 0.707113 -0.707098 0.00189536 0.7071 0.707111) 1) ((0 0 0) (0.999992 0.000140037 -0.00401223 -0.00293604 0.70712 -0.707087 0.00273811 0.707093 0.707115) 1) ((0 0 0) (1 -0.000137946 0.000135714 1.57813e-06 0.707107 0.707107 -0.000193506 -0.707107 0.707107) 1) ((0 0 0) (0.999999 -0.00110151 0.00104998 3.64383e-05 0.707109 0.707105 -0.00152133 -0.707104 0.707108) 1))

From function void Foam::globalIndexAndTransform::determineTransforms ()
in file primitives/globalIndexAndTransform/globalIndexAndTransform.C at line 225.

can you guys help me.

Thanks,
Siva

michael1023 December 18, 2012 11:43

Quote:

Originally Posted by blacksquirrel (Post 384832)
Hello Bombolati,

After using fluent3DMeshtoFoam you have two patches ("patchA" and "patchB") which should be cyclic but are labeled with "patch" or "wall".
Then you can use the createPatch utility.

In the createPatchDict you write
name patch1;
this is the new name of your cyclic patch

patchInfo (this is the section in which i set the new patch features)
{
type cyclic;
neighbourPatch patch2;
transform rotational;
[...]

constructFrom patches;
which means, that there are existing patches that are used to create the new patches. (It is possible to create patches from faces, then you have to write construct from faceSet)
and
patches (patchA)
which means, your new cyclic patch "patch1" is constructed from "patchA" (it is possible to construct a new patch from two or more existing patches)

and the same then for patch2:
constructFrom patches;
patches (patchB) ;

Hi, blacksquirrel.
As you said, I have changed the createPatchDict. But there is also have a error as below:


--> FOAM FATAL ERROR:
Attempt to cast type patch to type cyclic

From function refCast<To>(From&)
in file lnInclude/typeInfo.H at line 114.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 Foam::cyclicPolyPatch::neighbPatchID() const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#3 Foam::cyclicPolyPatch::calcGeometry(Foam::PstreamB uffers&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::polyBoundaryMesh::calcGeometry() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::polyMesh::addPatches(Foam::List<Foam::polyPa tch*> const&, bool) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/createPatch"
#7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/createPatch"
Aborted

Could you give me some advice for this error? Thank you.

blacksquirrel December 19, 2012 05:35

Ok, have you checked your "boundary" file in constant/polyMesh after using fluentMeshToFoam?
What is the type of your patchA/patchB? Do you have two separate patches?

This error is strange and I've never encountered it. Maybe it helps if you change the type of your patches A and B in the boundary file to "wall" instead of patch and try again.

michael1023 December 19, 2012 06:14

Hi, blacksquirrel.

Thank you for your reply. I made a mistake in createPatchDict. With help of Maddalena, I solve this problem as the link below.
http://www.cfd-online.com/Forums/ope...tml#post398207


All times are GMT -4. The time now is 09:56.