|
[Sponsors] |
[Commercial meshers] Problem with cyclic boundaries in Openfoam 2.3, mesh import from ICEM |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
February 28, 2018, 14:34 |
Problem with cyclic boundaries in Openfoam 2.3, mesh import from ICEM
|
#21 |
New Member
Rajesh Singh
Join Date: Jun 2010
Posts: 15
Rep Power: 16 |
Hi Bruno,
Can I use cyclicAMI in the translational periodic boundary in VOF method. I did try but simulation failed. However, VOF simulation with cyclic BC was working with mesh generated using SnappyHexMesh. We need very fine mesh near the wall of a complex geometry. This is why we want to third party mesh to import. Help for this would be appreciated. Thanks in advance |
|
March 4, 2018, 16:34 |
|
#22 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Quick answer: If you really are using OpenFOAM 2.3, then you should upgrade to the more recent versions of OpenFOAM or OpenFOAM+.
__________________
|
|
March 5, 2018, 15:02 |
|
#23 |
New Member
Rajesh Singh
Join Date: Jun 2010
Posts: 15
Rep Power: 16 |
Hi Bruno,
Thanks for your response in my post. I have tried fro OpenFOAM 5.0 and got following errors. Code:
**************************************************** [sing956@constance01 AMI]$ setFields /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 5.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 5.0 Exec : setFields Date : Mar 05 2018 Time : 10:52:48 Host : "constance01.pnl.gov" PID : 43729 I/O : uncollated Case : /people/sing956/Structure/Counter/Water/AMI nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading setFieldsDict Setting field default values Setting internal values of volScalarField alpha.water AMI: Creating addressing and weights between 8712 source faces and 8701 target faces --> FOAM Warning : From function void Foam::AMIMethod<SourcePatch, TargetPatch>::checkPatches() const [with SourcePatch = Foam::PrimitivePatch<Foam::face, Foam::SubList, const Foam::Field<Foam::Vector<double> >&>; TargetPatch = Foam::PrimitivePatch<Foam::face, Foam::SubList, const Foam::Field<Foam::Vector<double> >&>] in file lnInclude/AMIMethod.C at line 57 Source and target patch bounding boxes are not similar source box span : (2.84217e-17 0.026 0.0911) target box span : (0 0.026 0.0911) source box : (0 -0.013 -0.0851) (2.84217e-17 0.013 0.006) target box : (0.0534 -0.013 -0.0851) (0.0534 0.013 0.006) inflated target box : (0.0486631 -0.0177369 -0.0898369) (0.0581369 0.0177369 0.0107369) --> FOAM FATAL ERROR: Unable to find initial target face ************************************************************** The boundary for the corresponding patch is sideXneg { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 8712; startFace 2233503; matchTolerance 0.0005; transform translational; neighbourPatch sideXpos; separationVector (-0.0267 0 0); } sideXpos { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 8701; startFace 2242215; matchTolerance 0.0005; transform translational; neighbourPatch sideXneg; separationVector (0.0267 0 0); } ******************************************************** Thanks in advance. Last edited by wyldckat; March 5, 2018 at 19:46. Reason: Added [CODE][/CODE] markers |
|
March 5, 2018, 19:50 |
|
#24 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Quick answer: Isn't the separation vector defined with the wrong values? From what the output tells us, it should be something like twice the value:
Code:
separationVector (-0.0534 0 0);
__________________
|
|
March 5, 2018, 23:06 |
|
#25 |
New Member
Rajesh Singh
Join Date: Jun 2010
Posts: 15
Rep Power: 16 |
Hi Bruno,
Thank you very much for prompt response. I have fixed the separation vector by altering the sign of separation vector in the both faces. I got following errors. I am newb in OpenFOAM and don't have nay idea for this. help for resolving this problem would be highly appreciated. Thanks in advance Rajesh Code:
************************************************************* /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 5.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 5.0 Exec : ./interFoam Date : Mar 05 2018 Time : 19:01:48 I/O : uncollated nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 PIMPLE: Operating solver in PISO mode Reading field p_rgh AMI: Creating addressing and weights between 8712 source faces and 8701 target faces AMI: Patch source sum(weights) min/max/average = 0, 1, 0.999873 AMI: Patch target sum(weights) min/max/average = 0.94373, 1, 0.999988 Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Selecting turbulence model type laminar Selecting laminar stress model Stokes Reading g Reading hRef Calculating field g.h No MRF models present No finite volume options present DICPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 Courant Number mean: 0 max: 0 Starting time loop Courant Number mean: 0 max: 0 Interface Courant Number mean: 0 max: 0 deltaT = 1.1999e-05 Time = 1.1999e-05 PIMPLE: iteration 1 smoothSolver: Solving for alpha.water, Initial residual = 0, Final residual = 0, No Iterations 0 Phase-1 volume fraction = 0 Min(alpha.water) = 0 Max(alpha.water) = 1 MULES: Correcting alpha.water MULES: Correcting alpha.water Phase-1 volume fraction = 0 Min(alpha.water) = 0 Max(alpha.water) = 1 #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib64/libc.so.6" #3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ??:? #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:? #5 ? at ??:? #6 __libc_start_main in "/lib64/libc.so.6" #7 ? at ??:? Floating point exception Last edited by wyldckat; March 6, 2018 at 16:52. Reason: Added [CODE][/CODE] markers |
|
March 6, 2018, 16:59 |
|
#26 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Quick answer: Try running the following command before you run the solver:
Code:
export FOAM_ABORT=1 If it does not give much more information, then the only way to diagnose the problem is to have access to the case. See this page for more details on how to proceed: How to give enough info to get help |
|
July 2, 2018, 15:27 |
|
#27 |
New Member
Rajesh Singh
Join Date: Jun 2010
Posts: 15
Rep Power: 16 |
Hi Bruno,
I have imported StarCCM+ mesh to openfoam 5.0 and quality of mesh was also good. The CCM mesh is trimmed mesh with polyhedral cells. The flow simulation for interFoam with species transport equation diverges after some iterations. Below is report of the checkMesh. Help for resolving this issuw would be appreciated. ******************************* Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 2709670 faces: 7273254 internal faces: 6550582 cells: 2217107 faces per cell: 6.23508 boundary patches: 10 point zones: 0 face zones: 1 cell zones: 1 Overall number of cells of each type: hexahedra: 1558763 prisms: 17795 wedges: 1051 pyramids: 73 tet wedges: 51 tetrahedra: 184093 polyhedra: 455281 Breakdown of polyhedra by number of faces: faces number of cells 4 4 5 43 6 76272 7 247451 8 4264 9 70800 10 3318 11 356 12 16481 13 700 14 204 15 35328 16 60 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology floweriod1 110302 113851 ok (non-closed singly connected) flow:sheet1 229147 166554 ok (non-closed singly connected) flow:sheet2 228457 166118 ok (non-closed singly connected) flowutg 9532 9665 ok (non-closed singly connected) flow:wallt 9576 9998 ok (non-closed singly connected) floweriod2 110292 113851 ok (non-closed singly connected) flow:inl 5071 5594 ok (non-closed singly connected) flow:wallb 10551 11107 ok (non-closed singly connected) flowutl 5792 6040 ok (non-closed singly connected) flow:ing 3952 4069 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-0.0133625 -0.013 -0.0851) (0.0133628 0.013 0.007) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (4.18881e-14 -2.88815e-15 1.82866e-17) OK. Max cell openness = 2.78469e-16 OK. Max aspect ratio = 9.20971 OK. Minimum face area = 1.10391e-11. Maximum face area = 6.4e-07. Face area magnitudes OK. Min volume = 5.01959e-16. Max volume = 5.12e-10. Total volume = 3.4427e-05. Cell volumes OK. Mesh non-orthogonality Max: 57.8894 average: 11.7876 Non-orthogonality check OK. Face pyramids OK. Max skewness = 3.2775 OK. Coupled point location match (average 0) OK. Mesh OK. End |
|
November 15, 2019, 09:15 |
|
#28 | |
Senior Member
Jianrui Zeng
Join Date: May 2018
Location: China
Posts: 157
Rep Power: 8 |
Quote:
|
||
January 2, 2020, 16:07 |
Possible Solution
|
#29 |
Member
Federico Zabaleta
Join Date: May 2016
Posts: 47
Rep Power: 10 |
Hi everyone,
I've been dealing with this issue for a few hours until I found the solution. In my case it was a pretty simple solution.. but I want to share it just in case someone is dealing with a similar problem. My cyclic boundaries were parallel to each other, so basically the part of the createPatchDict that says: Code:
transform rotational; rotationAxis (0 0 1); rotationCentre (0 0 0); Hope this help. Federico |
|
October 6, 2020, 22:14 |
|
#30 | |
New Member
Miguel David Méndez Bohórquez
Join Date: Sep 2016
Location: Bogotá
Posts: 10
Rep Power: 10 |
Quote:
I have a similar problem with imported meshes and cyclic boundary conditions (more specific from gmsh). May you suggest me how should I set up a case with cyclic BC and an imported mesh? I have ran a case with these BC but with a mesh from blockMesh. Thanks in advance. Miguel. EDIT: After reading other posts, and a bit of the documentation, I guess I have gotten it. Last edited by Miguel.Mendez; October 7, 2020 at 01:34. |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Commercial meshers] A problem to use the mesh made by ICEM in openfoam | 278379rea | OpenFOAM Meshing & Mesh Conversion | 3 | June 6, 2016 03:54 |
Ansys 14.5 Problem Import Mesh from ICEM CFD to CFX | Smiling Assassin | CFX | 1 | May 9, 2014 03:27 |
[Commercial meshers] ICEM tetra mesh for OpenFoam | cfGreen | OpenFOAM Meshing & Mesh Conversion | 4 | October 24, 2013 07:13 |
[ICEM] ICEM Structured Mesh Problem | OMJT | ANSYS Meshing & Geometry | 3 | March 22, 2013 11:06 |
[Gmsh] 2D Mesh Generation Tutorial for GMSH | aeroslacker | OpenFOAM Meshing & Mesh Conversion | 12 | January 19, 2012 04:52 |