|
[Sponsors] |
[snappyHexMesh] SnappyHexMesh with Empty patches in blockMesh |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 6, 2022, 08:21 |
SnappyHexMesh with Empty patches in blockMesh
|
#1 |
Member
Ilan
Join Date: Dec 2018
Posts: 52
Rep Power: 7 |
Hello Foamers,
I really hope someone will see this soon, cause I am stuck here :/ So, I am working on a project using oversets. I used the wolfdynamics tutorials as basis to build my simulation. In those, the meshes containing the structures uses snappyHexMesh without problems. Their front and back are defined in the blockMesh as symmetryPlane. In the overall mesh (backgroud), front and back patches were defined as "empty". and the overset is working well. My problem is, I need to use snappyHexMesh to localy improve my 2D mesh but with empty patches in blockmesh, there is a point the calcul stop sending a warning : Code:
Correcting 2-D mesh motion--> FOAM Warning : From void Foam::twoDPointCorrector::calcAddressing() const in file twoDPointCorrector/twoDPointCorrector.C at line 163 The number of points in the mesh is not equal to twice the number of edges normal to the plane - this may be OK only for wedge geometries. Please check the geometry or adjust the orthogonality tolerance. Number of normal edges: 1066710 number of points: 1269000 I solved the problem by defining front and back as symmetryPlane but... doing that, the overset stopped working: in my simulation my moving meshes controled by the overset seems completly independant of the background mesh... I indentified 4 potential solutions upto now but don't know how to apply them or which one would be the best : - Include my mesh refinement in the blockmeshdict. I don't like this solution because it strongly limits my possibilities. - Find a way to use snappyHexMesh with empty front and back patches. I already tried to reorder the points before using snappy, but it did not change a thing. - Find another kind of patch that will not interfer with my overset. But as a symmetryPlane isn't working, I guess that none of them will. - Putting the symmetryPlane to mesh and removing it with a createPatch -overwrite to empty, but until now, this solution never succeed for some magical reasons, openfoam is refusing to swap back to empty patches... Do any of you have an idea how to solve this ? I would be really grateful. Feel free to ask for informations if you thing something is lacking in the thread, I really need to sort the things out ! Have a amazing day ! Magi |
|
May 6, 2022, 09:20 |
|
#2 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,190
Rep Power: 27 |
Hi Magi,
Snappy uses octree structure to split the mesh when refining and AFAIK it cannot deal with 2D meshes. This means the resulting mesh will have several cells in the 3rd direction, which is obviously something your want to avoid for a 2D case. This is why you need to use extrudeMesh to extrude a one layer thickness mesh out of one of the front or back patch. This will give you a clean 2D mesh with only one cell layer in the 3rd direction. changeDictionary can be used to update boundary conditions or patches types, it is great to update boundary types after meshing. I did not check but you should be able to find tutorials using extrudeMesh and changeDictionary. I hope this helps, Yann |
|
May 9, 2022, 06:42 |
|
#3 | |
Member
Ilan
Join Date: Dec 2018
Posts: 52
Rep Power: 7 |
Thank you for your reactivity Yann. The solution seems to work. i changed my boundaries using changeDictionary function :
Quote:
Merci ! |
||
January 22, 2024, 12:56 |
|
#4 | |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 |
Quote:
I tried to do the mentioned steps, except for running extrudeMesh! However, I can't see any changes in the boundary patches!! Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2112 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object changeDictionaryDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dictionaryReplacement { boundary { front { type empty; } back { type empty; } } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2112 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; arch "LSB;label=32;scalar=64"; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 7 ( inlet { type patch; nFaces 80; startFace 266920; } outlet { type patch; nFaces 80; startFace 267000; } top { type patch; nFaces 140; startFace 267080; } bottom { type patch; nFaces 140; startFace 267220; } front { type patch; nFaces 23189; startFace 267360; } back { type patch; nFaces 23189; startFace 290549; } naca { type wall; inGroups 2(nacaGroup wall); nFaces 7232; startFace 313738; } ) // ************************************************************************* // |
||
January 22, 2024, 13:03 |
|
#5 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,190
Rep Power: 27 |
Hello Saeed,
What output do you get when running changeDictionary? If you're using v2112 the syntax should be: Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2112 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object changeDictionaryDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // boundary { front { type empty; } back { type empty; } } // ************************************************************************* // Yann |
|
January 22, 2024, 13:13 |
|
#6 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 |
yeahhh, it worked.
Thanks Yann |
|
January 22, 2024, 13:25 |
|
#7 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 |
Ohhh, changeDictionary works properly, but an error occures in decomposition step!!
Code:
Create mesh for time = 0 Read dictionary changeDictionaryDict with replacements for dictionaries 1(boundary) Reading polyMesh/boundary file to extract patch names Loaded dictionary boundary with entries 7(inlet outlet top bottom front back naca) Extracted patch groups: group nacaGroup with patches 1(naca) group wall with patches 1(naca) Replacing entries in dictionary boundary Special handling of boundary as polyMesh/boundary file. Merging entries from 2(front back) fieldDict: { inlet { type patch; nFaces 80; startFace 266920; } outlet { type patch; nFaces 80; startFace 267000; } top { type patch; nFaces 140; startFace 267080; } bottom { type patch; nFaces 140; startFace 267220; } front { type empty; nFaces 23189; startFace 267360; } back { type empty; nFaces 23189; startFace 290549; } naca { type wall; inGroups 2 ( nacaGroup wall ); nFaces 7232; startFace 313738; } } Writing modified boundary End - Decomposition /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2112 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112 Arch : "LSB;label=32;scalar=64" Exec : decomposePar Date : Jan 22 2024 Time : 20:52:31 Host : DESKTOP-TK3D7CI PID : 22616 I/O : uncollated Case : /mnt/e/OpenFoam/Run/naca2412 nProcs : 1 trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Decomposing mesh Create mesh Calculating distribution of cells Decomposition method simple [6] (region region0) Finished decomposition in 0.03 s Calculating original mesh data Distributing cells to processors Distributing faces to processors Distributing points to processors Constructing processor meshes Reading hexRef8 data : cellLevel Reading hexRef8 data : pointLevel Reading hexRef8 data : level0Edge Processor 0 Number of cells = 8373 Number of faces shared with processor 1 = 316 Number of faces shared with processor 3 = 496 Number of processor patches = 2 Number of processor faces = 812 Number of boundary faces = 6387 Processor 1 Number of cells = 21279 Number of faces shared with processor 0 = 316 Number of faces shared with processor 2 = 823 Number of faces shared with processor 4 = 717 Number of processor patches = 3 Number of processor faces = 1856 Number of boundary faces = 5268 Processor 2 Number of cells = 18482 Number of faces shared with processor 1 = 823 Number of faces shared with processor 5 = 432 Number of processor patches = 2 Number of processor faces = 1255 Number of boundary faces = 15362 Processor 3 Number of cells = 23717 Number of faces shared with processor 0 = 496 Number of faces shared with processor 4 = 618 Number of processor patches = 2 Number of processor faces = 1114 Number of boundary faces = 9761 Processor 4 Number of cells = 10810 Number of faces shared with processor 1 = 717 Number of faces shared with processor 3 = 618 Number of faces shared with processor 5 = 210 Number of processor patches = 3 Number of processor faces = 1545 Number of boundary faces = 3007 Processor 5 Number of cells = 13607 Number of faces shared with processor 2 = 432 Number of faces shared with processor 4 = 210 Number of processor patches = 2 Number of processor faces = 642 Number of boundary faces = 14265 Number of processor faces = 3612 Max number of cells = 23717 (47.8186% above average 16044.7) Max number of processor patches = 3 (28.5714% above average 2.33333) Max number of faces between processors = 1856 (54.1528% above average 1204) Time = 0 --> FOAM FATAL IO ERROR: (openfoam-2112 patch=220610) inconsistent patch and patchField types for patch type empty and patchField type zeroGradient file: 0/cellLevel.boundaryField.front at line 96315. From static Foam::tmp<Foam::fvPatchField<Type> > Foam::fvPatchField<Type>::New(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = double] in file /usr/src/packages/BUILD/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 141. FOAM exiting
The error refers to this part in cellLevel: Screenshot (271).jpg Last edited by saeed jamshidi; January 22, 2024 at 16:04. |
|
January 23, 2024, 04:40 |
|
#8 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,190
Rep Power: 27 |
Hello Saeed,
changeDictionary modified your patch type to empty in the mesh (specifically in the constant/polyMesh/boundary file) but it didn't update these patches in the 0 directory since you didn't specify it. cellLevel is a variable written by snappy while meshing, so it has the same patch type as the ones defined during meshing. decomposePar complains because the front and back patches are now type empty in the boundary file, but the boundary conditions defined for those patches in 0 directory are incompatible (it should be empty too) To solve this issue you should also update the files in 0 directory: Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2112 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object changeDictionaryDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // boundary { front { type empty; } back { type empty; } } cellLevel { front { type empty; } back { type empty; } } // Same thing for all variables which need to be updated in 0 directory // ************************************************************************* // |
|
January 23, 2024, 06:07 |
|
#9 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 |
Hello Yann, thank you for the reply.
I adopted the following changeDictionary for my case, however, it gave me additional repetitive patches for front and back!! Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2112 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object changeDictionaryDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // boundary { front { type empty; } back { type empty; } } cellLevel { front { type empty; } back { type empty; } } // ************************************************************************* // |
|
January 23, 2024, 06:11 |
|
#10 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,190
Rep Power: 27 |
My bad, this should be the proper syntax for the changeDictionaryDict file:
Code:
cellLevel { boundaryField { front { type empty; } back { type empty; } } } |
|
January 23, 2024, 06:14 |
|
#11 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 |
Ohhh yeahh, I think I need some rest to recharge my batteries
Thanks again. |
|
Tags |
blockmesh, patches, snapphhexmesh |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] Patches disappearing after snappyHexMesh | obiscolly50 | OpenFOAM Meshing & Mesh Conversion | 3 | April 14, 2023 14:24 |
[mesh manipulation] createpatch not working when using layer addition in snappyHexMesh | Dikkeunit | OpenFOAM Meshing & Mesh Conversion | 0 | February 3, 2020 10:46 |
This mesh contains patches of type empty but is not 1D or 2D | oric | OpenFOAM Running, Solving & CFD | 36 | November 28, 2016 08:12 |
[snappyHexMesh] snappyHexMesh does not create boundary patches from .stl files | bug_or_feature | OpenFOAM Meshing & Mesh Conversion | 7 | August 30, 2016 20:18 |
[mesh manipulation] mirrorMesh and undoing the joining of patches | chegdan | OpenFOAM Meshing & Mesh Conversion | 3 | October 21, 2015 09:09 |