[Tobi]

Is there a reason that you use Salomon and tetraedrals instead of sHM?

[esujby]

Hi,

well, to be honest yes. its allot quicker to find out if theres something wrong with you geometry, especially when its a complex one, like the solar volumetric receiver i am working on. the mesh quality extremely thin surfaces is much better with salome (netgen) and i simply just couldn't mesh my geometry with SHM, it couldn't mesh thin surfaces bellow 0.02 mm. etc

the only reason i use tetrahedral cells is because the tutorial provided bellow. also at my university, all the CFD guys using Ansys for heat transfer simulations use tetrahedral cells, i am the only one using openFOAM in my institution loll...so i have a very limited to no guide with regards to meshing for openfoam.

lastly, i was able to quickly learn how to play around with the features of salome to realise a much better CAD configuration for meshing. so i put my CAD together in solid works, i tune the geometries on salome then straight to open foam. by the way are you recommending using some other option instead of tetrahedral cells?

kind regards


https://www.youtube.com/watch?v=1zQbU-E4k1U

[Tobi]

Originally Posted by esujby

Hi,

well, to be honest yes. its allot quicker to find out if theres something wrong with you geometry, especially when its a complex one, like the solar volumetric receiver i am working on. the mesh quality extremely thin surfaces is much better with salome (netgen) and i simply just couldn't mesh my geometry with SHM, it couldn't mesh thin surfaces bellow 0.02 mm. etc

Hi,

well I am working with salome and foam for more than 6 years now and foam could of course mesh thin surfaces below 0.02mm (:
In my opinion you will find a good mesh with sHM faster than with salome. I think in your case, you are not so familiar with sHM and therefore you get problems (like so many people). Finally everybody think sHM is a bad meshing tool

Anyway. It does not matter which mesher you are using but Tets are always not as good as hexaeder in the topic of numerics.

[alfa_8C]

Hi Tobi

how did you manage to preserve patch names in your tutorial of multi region sHM? I looks like it comes from blockMesh but this seems not obvious to me.

Thanx in advance,
Antonio

[esujby]

Originally Posted by Tobi

Hi,

well I am working with salome and foam for more than 6 years now and foam could of course mesh thin surfaces below 0.02mm (:
In my opinion you will find a good mesh with sHM faster than with salome. I think in your case, you are not so familiar with sHM and therefore you get problems (like so many people). Finally everybody think sHM is a bad meshing tool

Anyway. It does not matter which mesher you are using but Tets are always not as good as hexaeder in the topic of numerics.

Hi Tobi,

i think i didn't explain myself correctly, with all due respect with regards to ur experience using foam, i would still say i don't think meshing my complex geometry using SHM is easily possible yet to be honest. it is not just just a single thin surface. its a geometry made up of multiple concentric cones located inside a fluid region which is also encapsulated by another region ( in other words many regions within regions and so on. i literally spent about 6-9 months doing nothing else but just trying to get SHM to mesh the geometries with no success, set up a debug session with bruno, but still no immediate success and i decided to move to salome, and issue was resolved in a day or two. other geometries greater than greater than 0.02mm about 0.1mm were ok but as u get smaller SHM isn't able to handle it.

i have also max out my work station using SHM. but still....no success.

anther obvious fact is that salome has more features which easily allows one to manipulate CAD and mesh quite easily, which u don't get with SHM.

i guess its a matter of preference maybe but i think salome is definitely easier to use and the best way to start for complex geometries.

thanks you very much for the Hint. i will give herd cells a try now actually.

Kind regards

[anufagbemi]

Hello all,
after hours of try and error of multiple configurations and tools I want to share what I found on how to get splitted patches for a multi region case.
It seems to work now on a the simple construct of the 2 boxes with a splitted patch (all options with the solid/endsolid sections in the stl file did not work, also the experiments with creatPatch and splitMeshRegions -cellZonesOnly -useFaceZones ended in the defect surfaces).

Starting point is the generation of stl-files from salome for each single face or group. They provide a closed surface.
All faces are read in the sHMdict geometry section and get a name.

In the refinementSurfaces section the level defines the refinement level etc. In this example, one part of the interface gets a finer grid.

The key was to use

splitMeshRegions

with the

-blockedFaces

option, which generates regions according to defined faceSets
(see: http://openfoamwiki.net/index.php/SplitMeshRegions:
[I]-blockedFaces FACESET
Specify additional region boundaries that walking does not cross by specifying a faceSet

Hey guys,
I've been diligently going through this thread and I discovered me and @dzi had the same problem of multiple domains created (4 in your case instead of 2) after splitMeshRegions then resolved the problem to an extent by using the

splitMeshRegions -blockedFaces

Is there anyway you guys could assist me with mine. My main aim is just to split my model into 2 regions, I'll worry about the patches later. My geometry is more complex though and I need to carry out FSI simulation with it.

Steps I used were
1. Create a blockMesh for both domains in this case SOLID and FLUID
2. surfaceFeatureExtract
3. snappyHexmesh
4. splitMeshRegions -cellZones -overwrite

and then I get a lot of regions formed instead of FLUID and SOLID.
I tried using several other arguments such as -useFaceZone, -regions <NAME>, but they all gave me just one region.
I also followed dzi's exact procedure of using .setSet file, but none of them worked for me.

My main problem is that my shape needs quite some level of refinement so that the mesh quality is good. When I refine it and have a good mesh, the regions that result after splitMeshRegions are a lot: about 20 instead of 2. However when the refinements are not that fine I obtain my desired 2 regions while the mesh quality suffers.
Please what do you recommend? My case folder can be found here https://yadi.sk/d/w_SfFScN3RKpHM


And btw does anyone also know anything about the "det: " floating exception error in the last line of the following code from this Stress calculation? I got the error before I went back to refine my shape as stated above.

Create dynamic mesh for time = 0

Selecting dynamicFvMesh dynamicMotionSolverFvMesh
Selecting motion solver: velocityLaplacian
Selecting motion diffusion: quadratic
Selecting motion diffusion: inverseDistance
--> FOAM Warning : 
    From function polyBoundaryMesh::patchSet(const wordList&)
    in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 444
    Cannot find any patch names matching interface
 Reading stress mesh
Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar

PIMPLE: Operating solver in PISO mode

Creating fixed displacement boundary condition
Creating fixed displacement boundary condition
Creating fixed displacement boundary condition
Creating fixed displacement boundary condition
Creating traction displacement boundary conditions
Selecting rheology model linearElastic
Creating constitutive model
Selecting coupling scheme Aitken

Starting time loop

Creating beamReport function object.
History point ID: 712654
History point coordinates: (0.00220062 0.00173205 0.00154628)
Reference point coordinates: (0.45 0.15 -0.15)
Time = 0.005 (dt = 0.005)

Create extended GGI zone-to-zone interpolator
Checking fluid-to-solid face interpolator
Fluid-to-solid face interpolation error: 1.81175e-07
Checking solid-to-fluid point interpolator (GGI)
calcMasterPointAddressing() const
Extended GGI, master point distance, max: 1.35234e-07, avg: -1.63421e-12, min: -1.32708e-07
Solid-to-fluid point interpolation error (GGI): 1.35234e-07
Number of uncovered master faces: 0
Number of uncovered slave faces: 0
calcSlavePointAddressing() const
Extended GGI, slave point distance, max: 1.32708e-07, avg: 1.63421e-12, min: -1.35234e-07
Extended GGI, slave point orientation (<0), max: 0.728604, min: -1, nIncorrectPoints: 5/150409
Setting traction on solid patch
Total force (fluid) = (4.73487e-11 3.5512e-11 -9.90773e-11)
Total force (solid) = (-4.73498e-11 -3.5512e-11 9.9077e-11)
Evolving solid solver: unsTotalLagrangianSolid
det: -130.767, 45.3949
Floating point exception (core dumped)

Thanks guys
Samuel

[gtarang]

Originally Posted by dzi

Hello all,
after hours of try and error of multiple configurations and tools I want to share what I found on how to get splitted patches for a multi region case.
It seems to work now on a the simple construct of the 2 boxes with a splitted patch (all options with the solid/endsolid sections in the stl file did not work, also the experiments with creatPatch and splitMeshRegions -cellZonesOnly -useFaceZones ended in the defect surfaces).

Starting point is the generation of stl-files from salome for each single face or group. They provide a closed surface.
All faces are read in the sHMdict geometry section and get a name.

In the refinementSurfaces section the level defines the refinement level etc. In this example, one part of the interface gets a finer grid.

The key was to use

splitMeshRegions

with the

-blockedFaces

option, which generates regions according to defined faceSets
(see: http://openfoamwiki.net/index.php/SplitMeshRegions:
-blockedFaces FACESET
Specify additional region boundaries that walking does not cross by specifying a faceSet
)
in this case: setSet.batch:

faceSet box1FaceSet new zoneToFace box1_top
faceSet box1FaceSet add zoneToFace box1_interface_large
faceSet box1FaceSet add zoneToFace box1_interface_small
faceSet box1FaceSet add zoneToFace box1_walls
faceSet box1FaceSet subset

faceSet box2FaceSet new zoneToFace box2_bot
faceSet box2FaceSet add zoneToFace box2_walls
faceSet box2FaceSet subset

faceSet box1InterfLargeFaceSet new zoneToFace box1_interface_large
faceSet box1InterfSmallFaceSet new zoneToFace box1_interface_small

faceSet borderFaceSet new faceToFace box1FaceSet
faceSet borderFaceSet add faceToFace box2FaceSet 
faceSet borderFaceSet subset

With this faceSets, the complete domain gets splitted into the regions and all patches are preserved using:

splitMeshRegions -blockedFaces borderFaceSet -useFaceZones  -overwrite

Finally,

paraFoam -touchAll

lets you find all regions and patches with paraFoam.

What I did not try yet, is how to proceed with the mesh in regions,
but I guess one can create cellSets from regions and work on them (renaming? refine?).

The clean case is here : https://www.dropbox.com/s/m6hniecba2...ittedpatch.tgz
good luck, dirk

Hi,
I was also facing the same problem to split the interface in multiple patches. I used fluent mesh file. I followed following procedure:
1. I gave the name to the interface patches in the fluent mesh only and exported in msh format.
2.

> fluentMeshToFoam meshFile.msh -writeSets -writeZones

The "-writeSet" flag writes all the patches including interface patches in the set directory.
3. I used topoSetDict to make new faceZones from the (interface) faceSet.
Here is snippet from topoSetDict

    {
        name    left;      //name of the new faceZone we want to create
        type    faceZoneSet;
        action  new;      //we are creating new faceZone from each faceSet
        source  setToFaceZone;
        sourceInfo
        {
            faceSet left;
        }
    }

Create faceZones from all the interface patches
4. Use this command

> splitMeshRegions -useFaceZones -cellZones -overwrite

It will create the interfaces patches based upon the faceZones we created above

Hope someone may find it useful. Also suggest if anything can be done to shorten this process.

Thanks

[Rango]

Hi,

For this case you can use a combination of "topoSet" and "createPatch" for each mesh region separatly to create your desired patches.

The following link shares a test case which demonstrates these steps in action (please note that I have used OpenFoam-5.x to create and run the case):

patchMultiRegion_case

All the steps can be found in "run" bash script. Dictionaries for topoSet and createPatch are stored in separate folders in "system/topoSet" and "system/createPatch".

Cheers