[rsingh7]

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

[wyldckat]

Quick answer: If you really are using OpenFOAM 2.3, then you should upgrade to the more recent versions of OpenFOAM or OpenFOAM+.

[rsingh7]

Hi Bruno,

Thanks for your response in my post. I have tried fro OpenFOAM 5.0 and got following errors.

****************************************************
[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);
    }
********************************************************

Help for resolving this issue would be appropriated.

Thanks in advance.

[wyldckat]

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:

separationVector (-0.0534 0 0);

[rsingh7]

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

*************************************************************
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  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

[wyldckat]

Quick answer: Try running the following command before you run the solver:

export FOAM_ABORT=1

this should tell the solver to give us a bit more information before it crashes.

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

[rsingh7]

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

[calf.Z]

Originally Posted by galap

Hello,

I encountered the same problem and I could solve it by defining rotational periodicity and then by declaring the corresponding vertices in ICEM as periodic. Then Right Click on Faces in the Blocking tree -> Periodic Faces -> ensure that really every periodic face is colored accordingly. createPatch went fine after this procedure.

Thank you for the solution. It helps me to avoid the error:"does not match neighbor..." But I am not sure why it should work. Any more explanations?

[fedez91]

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:

            transform rotational;
            rotationAxis (0 0 1);
            rotationCentre (0 0 0);

has to be removed or commented. Once that was removed everything went great. The issue came from the template provided by foamGet, that had those three lines included.

Hope this help.

Federico

[Miguel.Mendez]

Originally Posted by wyldckat

Quick answer:

1. Check the file "applications/utilities/mesh/manipulation/createPatch/createPatchDict" for a more complete example.
2. If the patches are not perfectly cyclic, try using "cyclicAMI".

Hi Bruno!

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.