Mesh Manipulation Issues
I am having some issues with using stitchMesh that i dont understand.
My original mesh was created using blockMesh and it was a rotationally periodic domain which was only 1/8th of the full sector. This geometry was created for a RANS calculation where i could work just with this periodicity.
Now that I am moving to LES, I need to look at the full 360 degrees domain and not a sector. For this i took my mesh and used transformPoints to rotate is by 45 degree steps and then i pasted all these 8 meshes together using mergeMeshes utility. After merging, the overlapping faces need to be fused so that openFoam sees them as internal faces and not as boundaries. I wanted to use stitchMesh to do this.
There are a total of 8 such overlaps and so here is my question and problem:
1) Is mergeMesh and then stitchMesh the best way to do this? or can this be done in a different way?
2) If I have multiple overlapping patches that i need to fuse/stitch, can stitchMesh deal with all of them in one-go?
What I did is first tried it with one set of the overlapping patches and it worked. I checked the boundary file and also the geometry in openfoam.
When I do this again for the second overlap, it does not work, i just get an error as follows...
Create mesh for time = 1
Coupling perfectly aligned patches side2a_0 and side1a_315
Resulting (internal) faces will be in faceZone side2a_0side1a_315CutFaceZone
Note: both patches need to align perfectly.
Both the vertex positions and the face centres need to align to within
a tolerance given by the minimum edge length on the patch
--> FOAM FATAL ERROR:
Master or slave face zone contain no faces. Please check your mesh definition.
From function void slidingInterface::checkDefinition()
in file slidingInterface/slidingInterface.C at line 97.
#0 Foam::error::printStack(Foam::Ostream&) in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 Foam::slidingInterface::checkDefinition() in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#3 Foam::slidingInterface::slidingInterface(Foam::wor d const&, Foam::dictionary const&, int, Foam::polyTopoChanger const&) in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#4 Foam::polyMeshModifier::adddictionaryConstructorTo Table<Foam::slidingInterface>::New(Foam::word const&, Foam::dictionary const&, int, Foam::polyTopoChanger const&) in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#5 Foam::polyMeshModifier::New(Foam::word const&, Foam::dictionary const&, int, Foam::polyTopoChanger const&) in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#6 Foam::polyTopoChanger::readModifiers() in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#7 Foam::polyTopoChanger::polyTopoChanger(Foam::polyM esh&) in "/home/vishalsim/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
#9 __libc_start_main in "/lib64/libc.so.6"
Aborted (core dumped)
When I look in the boundary file, it clearly shows that there are faces in those patches and that they are the right overlapping ones (I checked it in openFoam by just selecting those two for display and they overlapped), but the openfoam error states that master and slave contain no faces... Im confused. Any thoughts anyone?
Also, any general advice on how to merge meshes that are periodic to create the full geometry, all inside openfoam?
To add to my post...
1) What are the *Zones files that are created after i do the stitchMesh? Are these required eventually when I use this mesh for simulations?
2) Same question, for meshPhi and also the meshmodifiers file?
Turns out, the problem was in the additional files that were created....
stitchMesh can be used only two patches at a time and so it creates a new time mesh every time you do it and you keep repeating them. But each time you have to delete those additional redundant files before doing the operation. The final mesh boundary files would show these patches to be having 0 faces and become internal... you can then delete them from that file and run paraFoam to show the final mesh and patches as well as check it with checkMesh...
All of this worked for me... just sharing with those who may face this or are facing this issue..
|All times are GMT -4. The time now is 17:55.|