[rakesh.a]

Greetings,
I'm trying to solve a case where, flow is going through a pipe. Pipe have a geometry at center of pipe which will disturb flow.
I have done meshing in 'Gmsh'. Which when I convert to openFoam & do checkMesh. It gives me error message of 2 skew faces (see image 01).

When I try to solve this problem with simpleFoam solver (Turbulence ON). It runs for few steps and stops running with back trace error (see image 02).

I have tried reducing relaxation factors, & increasing tolerances. But, it's making output results unrealistic & not converged (Well, results sucks!!)

Can anyone help me resolve this issue. What changes should I do to get converged results. Also, let me know if anything required to get more understanding.

Thanks,
Rakesh

[arjun]

Originally Posted by rakesh.a

Greetings,
I'm trying to solve a case where, flow is going through a pipe. Pipe have a geometry at center of pipe which will disturb flow.
I have done meshing in 'Gmsh'. Which when I convert to openFoam & do checkMesh. It gives me error message of 2 skew faces (see image 01).

When I try to solve this problem with simpleFoam solver (Turbulence ON). It runs for few steps and stops running with back trace error (see image 02).

I have tried reducing relaxation factors, & increasing tolerances. But, it's making output results unrealistic & not converged (Well, results sucks!!)

Can anyone help me resolve this issue. What changes should I do to get converged results. Also, let me know if anything required to get more understanding.

Thanks,
Rakesh

you rmesh check failed. Unless software (openfoam) takes care of these failed cells solver would fail to converge.

[alexeym]

Hi,

Your simulation has diverged. It could be caused by:
- inappropriate initial/boundary conditions
- inappropriate discretisation schemes
- inappropriate solver settings

You provided no details on the first point.

Your mesh is rather non-orthogonal, so your schemes/solver settings should be adopted to the case. You can find recommended settings for highly non-orthogonal meshes in many places (according to log you even do not have non-orthogonal correctors).

You can start by adding fvSchemes/fvSolutions to your post. Then search "open foam non-orthogonal mesh" in your preferred search engine.

[rakesh.a]

I tried changing settings in fvschems/fvsolution as suitable for non-orthogonal meshes.
Also, trying to get mesh more optimized for getting rid of Skewness.

[rakesh.a]

Originally Posted by alexeym

Hi,

Your simulation has diverged. It could be caused by:
- inappropriate initial/boundary conditions
- inappropriate discretisation schemes
- inappropriate solver settings

You provided no details on the first point.

Your mesh is rather non-orthogonal, so your schemes/solver settings should be adopted to the case. You can find recommended settings for highly non-orthogonal meshes in many places (according to log you even do not have non-orthogonal correctors).

You can start by adding fvSchemes/fvSolutions to your post. Then search "open foam non-orthogonal mesh" in your preferred search engine.

Hello,
I have tried meshing model again using different meshing method in gmsh. checkmesh in openFoam shows Mesh as "OK".
Used smoothSolver for pressure & velocity.
Solution is converging after running some steps and then start diverging drastically. And because of that results for first few steps seems alright, but after few steps values of pressure & velocity changing drastically.
I'm attaching my fvSolution & fvSchemes to this post. I'm new to openFoam and trying lot of changes in my case setup.

Thank you!!!!

[alexeym]

Hi,

The post does not have two additional files: checkMesh output and nut boundary conditions. But let's try to analyse what we have got. I will assume, mesh is non-orthogonal with non-orthogonality below 70 degrees (say 65).

fvSchemes:
gradSchemes -> leastSquares (strictly speaking Gauss linear is for orthogonal meshes only)
divSchemes -> everything to upwind (we are trying to converge, later you can change upwind to higher order schemes)
laplacianSchemes -> corrected
snGradSchemes -> corrected

fvSolution:
solvers.p -> PCG
solvers.(U|k|epsilon) -> PBiCGStab

nNonOrthogonalCorrectors -> 2

If it still behaves badly:
consistent -> no
relaxationFactors.equations.U -> 0.7
relaxationFactors.fields.p -> 0.3
relaxation for turbulence equations -> 0.5

Meanwhile, you can also add checkMesh output and nut BC/IC files.

[rakesh.a]

Originally Posted by alexeym

Hi,

The post does not have two additional files: checkMesh output and nut boundary conditions. But let's try to analyse what we have got. I will assume, mesh is non-orthogonal with non-orthogonality below 70 degrees (say 65).

fvSchemes:
gradSchemes -> leastSquares (strictly speaking Gauss linear is for orthogonal meshes only)
divSchemes -> everything to upwind (we are trying to converge, later you can change upwind to higher order schemes)
laplacianSchemes -> corrected
snGradSchemes -> corrected

fvSolution:
solvers.p -> PCG
solvers.(U|k|epsilon) -> PBiCGStab

nNonOrthogonalCorrectors -> 2

If it still behaves badly:
consistent -> no
relaxationFactors.equations.U -> 0.7
relaxationFactors.fields.p -> 0.3
relaxation for turbulence equations -> 0.5

Meanwhile, you can also add checkMesh output and nut BC/IC files.

Thank you!
Max non-orthogonality is 89.0305.
I have attached checkMesh & nut boundary conditions.

I'm trying to solve & study setup suggested by you.

[alexeym]

Maybe you can use decent mesher? Tetrahedral mesh with almost 90 degrees of non-orthogonality is something strange. Netgen usually generates much nicer meshes compared to Gmsh.

Maybe it will be necessary to revert to limited non-orthogonal correction. I.e. instead of "corrected" you put "limited 0.5" or "limited 0.333".

[rakesh.a]

Followig is error I get everytime ,
Backtrace:
ZN10StackTraceC1Ev [0x705c1465+0x25]
module: C:\PROGRA~1\BLUECF~1\ThirdParty-5.x\platforms\mingw_w64GccDPInt32\lib\libstack_tra ce.dll
ZN4Foam5error10printStackERNS_7OstreamE [0x30b1c88+0x218]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFO AM.dll
ZN4Foam6sigFpe13sigFpeHandlerEi [0x30b2af3+0x33]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFO AM.dll
(No symbol) [0x403cad]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\simpleFoa m.exe
_C_specific_handler [0x7ffbef161196+0x96]
module: C:\WINDOWS\SYSTEM32\ntdll.dll
0_chkstk [0x7ffbef174ecd+0x11d]
module: C:\WINDOWS\SYSTEM32\ntdll.dll
RtlWalkFrameChain [0x7ffbef0f6058+0x1518]
module: C:\WINDOWS\SYSTEM32\ntdll.dll
KiUserExceptionDispatcher [0x7ffbef173dfe+0x2e]
module: C:\WINDOWS\SYSTEM32\ntdll.dll
ZN4Foam18DILUPreconditioner15calcReciprocalDERNS_5 FieldIdEERKNS_9lduMatrixE [0x2f5bf2e+0x8e]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFO AM.dll
ZN4Foam18DILUPreconditionerC2ERKNS_9lduMatrix6solv erERKNS_10dictionaryE [0x2f5bff2+0x52]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFO AM.dll
ZN4Foam9lduMatrix14preconditioner31addasymMatrixCo nstructorToTableINS_18DILUPreconditionerEE3NewERKN S0_6solverERKNS_10dictionaryE [0x31c348f+0x2f]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFO AM.dll
ZN4Foam9lduMatrix14preconditioner3NewERKNS0_6solve rERKNS_10dictionaryE [0x2f52447+0x117]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFO AM.dll
ZNK4Foam9PBiCGStab5solveERNS_5FieldIdEERKS2_h [0x2f56fee+0x4ae]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFO AM.dll
(No symbol) [0x42b02e]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\simpleFoa m.exe
(No symbol) [0x42c235]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\simpleFoa m.exe
(No symbol) [0x42c535]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\simpleFoa m.exe
(No symbol) [0x44e045]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\simpleFoa m.exe
(No symbol) [0x4013f7]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\simpleFoa m.exe
(No symbol) [0x40152b]
module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\simpleFoa m.exe
BaseThreadInitThunk [0x7ffbec7b3574+0x14]
module: C:\WINDOWS\System32\KERNEL32.DLL
RtlUserThreadStart [0x7ffbef13cb81+0x21]
module: C:\WINDOWS\SYSTEM32\ntdll.dll

Anyway, I have setup of Salome meshing with me. I'm going to see if it makes any difference.

[alexeym]

This is typical backtrace produced by a diverged solution (in your case DILU preconditioner was not able to do its job).

You can try reverting to smoothSolver/GaussSeidel pair for velocity and turbulence.