|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Suyash Shrestha
Join Date: Jul 2021
Posts: 6
Rep Power: 5 ![]() |
Hi everyone,
I am working on simulating the flow around a square cylinder using the k-omega SST IDDES model in OpenFOAM-v2106. Prior to this, I ran the IDDES on the same mesh using the Spalart Allmaras model and that gave satisfactory results. The simulation with the k-omega SST model, however, was giving some strange results for the eddy viscosity as shown in the attached .png file. Furthermore, the RANS modelled region in the domain was also looking incorrect where the region far away from the wall was being modelled with RANS as shown in the other .png file. I have attached my case files for the k-omega SST case (the constant/polymesh folder is not included as the folder exceeded the maximum upload file size). Could someone please help me figure out what I am doing wrong? Last edited by Suyash.S; July 27, 2021 at 07:15. |
|
![]() |
![]() |
![]() |
![]() |
#2 |
New Member
Arturo Alanís
Join Date: Oct 2021
Posts: 9
Rep Power: 4 ![]() |
Hello. Sorry I cannot help you with your problem. I hope by this time you managed to solve it. However I have a question on the implementation of kw SST IDDES in openFOAM. I found it is implemented by choosing LES as the simulation type in the turbulenceProperties dictionary and setting the LESModel to be kOmegaSSTIDDES.
I did this but when I try to run the simulation it crashes, telling me there's no such model. The list it gives me as valid models is the following: DeardorffDiffStress Smagorinsky SpalartAllmarasDDES SpalartAllmarasDES SpalartAllmarasIDDES WALE dynamicKEqn dynamicLagrangian kEqn kOmegaSSTDES Could it be due to the distribution or the version of openFOAM? |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Suyash Shrestha
Join Date: Jul 2021
Posts: 6
Rep Power: 5 ![]() |
It is possible. I was using OpenFOAM v2106 from ESI.
|
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Arturo Alanís
Join Date: Oct 2021
Posts: 9
Rep Power: 4 ![]() |
Yeah I installed v 2112 and it has it. It seems that this model isn't implemented in openfoam org distribution. Thank you for your reply!
|
|
![]() |
![]() |
![]() |
![]() |
#5 | |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
Quote:
I am trying to run this turbulence model. But, I have come across Unknown discretisation type DEShybrid error! By the way, I'm including libs ("libturbulenceModelSchemes.so") in controlDict. would you please tell me how can I handle it? thanks. |
||
![]() |
![]() |
![]() |
![]() |
#6 |
New Member
Suyash Shrestha
Join Date: Jul 2021
Posts: 6
Rep Power: 5 ![]() |
Try using
libs (turbulenceModelSchemes); instead, in system/controlDict. If that also does not work, you need to verify if the modules were correctly installed in the OpenFOAM install directory. |
|
![]() |
![]() |
![]() |
![]() |
#7 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
Thank you for the reply.
I tryed libs (turbulenceModelSchemes) instead of libs ("libturbulenceModelSchemes.so"), it does not work. However, according to https://openfoam.com/documentation/g...8H_source.html, I should use the second lib. in OpenFoam v2112. Besides, I didn't get: you need to verify if the modules were correctly installed in the OpenFOAM install directory. would you please clarify it for me? Error: Code:
--> FOAM FATAL IO ERROR: (openfoam-2112 patch=220610) Unknown discretisation type DEShybrid Valid discretisation types : 63 ( CoBlended Gamma GammaV LUST MUSCL MUSCLV Minmod MinmodV OSPRE OSPREV Phi QUICK QUICKV SFCD SFCDV SuperBee SuperBeeV UMIST UMISTV biLinearFit blended cellCoBlended clippedLinear cubic cubicUpwindFit deferredCorrection downwind filteredLinear filteredLinear2 filteredLinear2V filteredLinear3 filteredLinear3V fixedBlended limitWith limitedCubic limitedCubicV limitedLinear limitedLinearV limiterBlended linear linearFit linearPureUpwindFit linearUpwind linearUpwindV localBlended localMax localMin midPoint outletStabilised pointLinear quadraticFit quadraticLinearFit quadraticLinearUpwindFit quadraticUpwindFit reverseLinear skewCorrected upwind vanAlbada vanAlbadaV vanLeer vanLeerV weighted weightedFlux ) file: system/fvSchemes.divSchemes.div(phi,U) at line 31. From static Foam::tmp<Foam::surfaceInterpolationScheme<Type> > Foam::surfaceInterpolationScheme<Type>::New(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>] in file lnInclude/surfaceInterpolationScheme.C at line 114. FOAM exiting saeed |
|
![]() |
![]() |
![]() |
![]() |
#8 |
New Member
Suyash Shrestha
Join Date: Jul 2021
Posts: 6
Rep Power: 5 ![]() |
In your foam install directory, check the following directory
/src/TurbulenceModels/schemes/ In there, there should be a directory called "DEShybrid" which should have "DEShybrid.C" "DEShybrid.H" inside it. |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
Yes, there are.
So what is the problem? ![]() As you can see from previous message, openfoam illustrate that there is not such discretisation ! Besides, I can run periodic hill case with SpalartAllmarasIDDES turbulent model, so there should not be problem with DEShybrid! Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2112 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default backward; } gradSchemes { default Gauss linear; grad(p) Gauss linear; } divSchemes { default none; div(phi,U) Gauss DEShybrid linear // scheme 1 linearUpwind grad(U) // scheme 2 hmax 0.65 // DES coefficient, typically = 0.65 1 // Reference velocity scale 0.028 // Reference length scale 0 // Minimum sigma limit (0-1) 1 // Maximum sigma limit (0-1) 1; // 1.0e-03; // Limiter of B function, typically 1e-03 div(phi,k) Gauss limitedLinear 1; div(phi,nuTilda) Gauss limitedLinear 1; div((nuEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } wallDist { method meshWave; nRequired yes; } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2112 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default backward; } gradSchemes { default leastSquares; } divSchemes { default none; div(phi,U) Gauss DEShybrid linear // scheme 1 linearUpwind grad(U) // scheme 2 hmax // LES delta name, e.g. 'delta', 'hmax' 0.65 // DES coefficient, typically = 0.65 1 // Reference velocity scale 0.04 // Reference length scale 0 // Minimum sigma limit (0-1) 1 // Maximum sigma limit (0-1) 1.0e-03; // Limiter of B function, typically 1e-03 div(phi,k) Gauss limitedLinear 0.1; div(phi,B) Gauss limitedLinear 0.1; div(B) Gauss linear; div(phi,omega) Gauss limitedLinear 0.1; div((nuEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear orthogonal; } interpolationSchemes { default linear; } snGradSchemes { default orthogonal; } wallDist { method meshWave; nRequired yes; } // ************************************************************************* // |
|
![]() |
![]() |
![]() |
![]() |
#10 |
New Member
Suyash Shrestha
Join Date: Jul 2021
Posts: 6
Rep Power: 5 ![]() |
It seems OpenFOAM is not recognising the DESHybrid scheme. An alternative approach could be to just use a simple limitedLinear scheme. That should work just fine. If you really want to use the DESHybrid scheme, you could try a different OpenFOAM version. I have used the Hybrid scheme in OpenFOAM version 2106 so you could try using that version.
|
|
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
Dear Suyash.S, thank you for your time.
I could run PeriodicHil case with DEShybrid, so there shoud be another reasions.... ![]() |
|
![]() |
![]() |
![]() |
![]() |
#12 |
New Member
Suyash Shrestha
Join Date: Jul 2021
Posts: 6
Rep Power: 5 ![]() |
Could you try running the periodic hill case with the k-omega model?
|
|
![]() |
![]() |
![]() |
![]() |
#13 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
I have not tested yet.
PeriodicHill works based on spallartAlmarasIDDES model, if I change turbulence model to K-omega IDDES, the case will be similar to present case. |
|
![]() |
![]() |
![]() |
![]() |
#14 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
I installed openfoam2106, and still it doesn't work
![]() ![]() Could you share your blockMesh file, this would be my last shot. thanks. Code:
saeedfoam@DESKTOP-TK3D7CI:~/OpenFOAM-v2106/tutorials/incompressible/pimpleFoam/LES/cylinder3D$ mpirun -np 4 pimpleFoam -parallel -------------------------------------------------------------------------- WARNING: Linux kernel CMA support was requested via the btl_vader_single_copy_mechanism MCA variable, but CMA support is not available due to restrictive ptrace settings. The vader shared memory BTL will fall back on another single-copy mechanism if one is available. This may result in lower performance. Local host: DESKTOP-TK3D7CI -------------------------------------------------------------------------- /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2106 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : _40a7d5d6-20210727 OPENFOAM=2106 patch=211215 Arch : "LSB;label=32;scalar=64" Exec : pimpleFoam -parallel Date : Nov 08 2023 Time : 22:21:20 Host : DESKTOP-TK3D7CI PID : 2315 I/O : uncollated Case : /home/saeedfoam/OpenFOAM-v2106/tutorials/incompressible/pimpleFoam/LES/cylinder3D nProcs : 4 Hosts : ( (DESKTOP-TK3D7CI 4) ) Pstream initialized with: floatTransfer : 0 nProcsSimpleSum : 0 commsType : nonBlocking polling iterations : 0 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 --> FOAM Warning : From void* Foam::dlLibraryTable::openLibrary(const Foam::fileName&, bool) in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 188 Could not load "libadaptiveFvMesh.so" libadaptiveFvMesh.so: cannot open shared object file: No such file or directory Create mesh for time = 0 PIMPLE: Operating solver in PISO mode Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model type LES Selecting LES turbulence model kOmegaSSTIDDES Selecting LES delta type IDDESDelta Selecting LES hmax type maxDeltaxyzCubeRoot Selecting patchDistMethod meshWave LES { LESModel kOmegaSSTIDDES; printCoeffs yes; turbulence yes; delta IDDESDelta; IDDESDeltaCoeffs { hmax maxDeltaxyzCubeRoot; maxDeltaxyzCubeRootCoeffs { } } Ce 1.048; alphaK1 0.85; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.856; gamma1 0.5555555556; gamma2 0.44; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; b1 1; c1 10; F3 false; decayControl false; kInf 0; omegaInf 0; kappa 0.41; CDESkom 0.82; CDESkeps 0.6; Cdt1 20; Cdt2 3; Cl 5; Ct 1.87; } No MRF models present No finite volume options present Courant Number mean: 0.003575439151 max: 0.5 forceCoeffs forceCoeffs1: rho: rhoInf Freestream density (rhoInf) set to 1000 Not including porosity effects Starting time loop Courant Number mean: 0.003575439151 max: 0.5 deltaT = 0.0125 Time = 0.0125 PIMPLE: iteration 1 [2] [2] [2] --> FOAM FATAL IO ERROR: (openfoam-2106 patch=211215-------------------------------------------------------------------------- MPI_ABORT was invoked on rank 2 in communicator MPI_COMM_WORLD with errorcode 1. NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes. You may or may not see output from other processes, depending on exactly when Open MPI kills them. -------------------------------------------------------------------------- ) [2] Unknown discretisation type DEShybrid Valid discretisation types : 63 ( CoBlended Gamma GammaV LUST MUSCL MUSCLV Minmod MinmodV OSPRE OSPREV Phi QUICK QUICKV SFCD SFCDV SuperBee SuperBeeV UMIST UMISTV biLinearFit blended cellCoBlended clippedLinear cubic cubicUpwindFit deferredCorrection downwind filteredLinear filteredLinear2 filteredLinear2V filteredLinear3 filteredLinear3V fixedBlended limitWith limitedCubic limitedCubicV limitedLinear limitedLinearV limiterBlended linear linearFit linearPureUpwindFit linearUpwind linearUpwindV localBlended localMax localMin midPoint outletStabilised pointLinear quadraticFit quadraticLinearFit quadraticLinearUpwindFit quadraticUpwindFit reverseLinear skewCorrected upwind vanAlbada vanAlbadaV vanLeer vanLeerV weighted weightedFlux ) [2] [2] [2] file: stream.divSchemes.div(phi,U) at line 0. [2] [2] From static Foam::tmp<Foam::surfaceInterpolationScheme<Type> > Foam::surfaceInterpolationScheme<Type>::New(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>] [2] in file lnInclude/surfaceInterpolationScheme.C at line 114. [2] FOAM parallel run exiting [2] [0] [0] [0] --> FOAM FATAL IO ERROR: (openfoam-2106 patch=211215) [0] Unknown discretisation type DEShybrid Valid discretisation types : 63 ( CoBlended Gamma GammaV LUST MUSCL MUSCLV Minmod MinmodV OSPRE OSPREV Phi QUICK QUICKV SFCD SFCDV SuperBee SuperBeeV UMIST UMISTV biLinearFit blended cellCoBlended clippedLinear cubic cubicUpwindFit deferredCorrection downwind filteredLinear filteredLinear2 filteredLinear2V filteredLinear3 filteredLinear3V fixedBlended limitWith limitedCubic limitedCubicV limitedLinear limitedLinearV limiterBlended linear linearFit linearPureUpwindFit linearUpwind linearUpwindV localBlended localMax localMin midPoint outletStabilised pointLinear quadraticFit quadraticLinearFit quadraticLinearUpwindFit quadraticUpwindFit reverseLinear skewCorrected upwind vanAlbada vanAlbadaV vanLeer vanLeerV weighted weightedFlux ) [0] [0] [0] file: /home/saeedfoam/OpenFOAM-v2106/tutorials/incompressible/pimpleFoam/LES/cylinder3D/system/fvSchemes.divSchemes.div(phi,U) at line 32. [0] [0] From static Foam::tmp<Foam::surfaceInterpolationScheme<Type> > Foam::surfaceInterpolationScheme<Type>::New(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>] [0] in file lnInclude/surfaceInterpolationScheme.C at line 114. [0] FOAM parallel run exiting [0] [1] [1] [1] --> FOAM FATAL IO ERROR: (openfoam-2106 patch=211215) [1] Unknown discretisation type DEShybrid Valid discretisation types : 63 ( CoBlended Gamma GammaV LUST MUSCL MUSCLV Minmod MinmodV OSPRE OSPREV Phi QUICK QUICKV SFCD SFCDV SuperBee SuperBeeV UMIST UMISTV biLinearFit blended cellCoBlended clippedLinear cubic cubicUpwindFit deferredCorrection downwind filteredLinear filteredLinear2 filteredLinear2V filteredLinear3 filteredLinear3V fixedBlended limitWith limitedCubic limitedCubicV limitedLinear limitedLinearV limiterBlended linear linearFit linearPureUpwindFit linearUpwind linearUpwindV localBlended localMax localMin midPoint outletStabilised pointLinear quadraticFit quadraticLinearFit quadraticLinearUpwindFit quadraticUpwindFit reverseLinear skewCorrected upwind vanAlbada vanAlbadaV vanLeer vanLeerV weighted weightedFlux ) [1] [1] [1] file: stream.divSchemes.div(phi,U) at line 0. [1] [1] From static Foam::tmp<Foam::surfaceInterpolationScheme<Type> > Foam::surfaceInterpolationScheme<Type>::New(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>] [1] in file lnInclude/surfaceInterpolationScheme.C at line 114. [1] FOAM parallel run exiting [1] [3] [3] [3] --> FOAM FATAL IO ERROR: (openfoam-2106 patch=211215) [3] Unknown discretisation type DEShybrid Valid discretisation types : 63 ( CoBlended Gamma GammaV LUST MUSCL MUSCLV Minmod MinmodV OSPRE OSPREV Phi QUICK QUICKV SFCD SFCDV SuperBee SuperBeeV UMIST UMISTV biLinearFit blended cellCoBlended clippedLinear cubic cubicUpwindFit deferredCorrection downwind filteredLinear filteredLinear2 filteredLinear2V filteredLinear3 filteredLinear3V fixedBlended limitWith limitedCubic limitedCubicV limitedLinear limitedLinearV limiterBlended linear linearFit linearPureUpwindFit linearUpwind linearUpwindV localBlended localMax localMin midPoint outletStabilised pointLinear quadraticFit quadraticLinearFit quadraticLinearUpwindFit quadraticUpwindFit reverseLinear skewCorrected upwind vanAlbada vanAlbadaV vanLeer vanLeerV weighted weightedFlux ) [3] [3] [3] file: stream.divSchemes.div(phi,U) at line 0. [3] [3] From static Foam::tmp<Foam::surfaceInterpolationScheme<Type> > Foam::surfaceInterpolationScheme<Type>::New(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>] [3] in file lnInclude/surfaceInterpolationScheme.C at line 114. [3] FOAM parallel run exiting [3] [DESKTOP-TK3D7CI:02310] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied [DESKTOP-TK3D7CI:02310] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages [DESKTOP-TK3D7CI:02310] 3 more processes have sent help message help-mpi-api.txt / mpi-abort saeedfoam@DESKTOP-TK3D7CI:~/OpenFOAM-v2106/tutorials/incompressible/pimpleFoam/LES/cylinder3D$ |
|
![]() |
![]() |
![]() |
![]() |
#15 |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
It is really funny, finally by burning the midnight oil I found the problem.
It was because of the libs ("libturbulenceModelSchemes.so") location. By chance I changed it from here: Code:
FoamFile { version 2.0; format ascii; class dictionary; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // libs ("libturbulenceModelSchemes.so"); application PimpleFoam; startFrom latestTime; to here: Code:
adjustTimeStep yes; maxCo 0.8; libs ("libadaptiveFvMesh.so"); libs ("libturbulenceModelSchemes.so"); functions { vorticity1 ![]() |
|
![]() |
![]() |
![]() |
![]() |
#16 | |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
Quote:
Did you find your problem? I tried to simulate flow over ellipse, but there were not reasionable results!!! |
||
![]() |
![]() |
![]() |
![]() |
#17 | |
Senior Member
Saeed Jamshidi
Join Date: Aug 2019
Posts: 214
Rep Power: 8 ![]() |
Quote:
I explored some threads about simulating flow around a cylinder and I could not found eny close one except yours. I would appreciate it if you help me with the trobble that I'v stuck! Here is my problem description: Question on simulating turbulent flow around a cylinder Besides, I have attached my full case. Thank you for your time. |
||
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
k Omega SST on a centrifugal fan | Fouch | OpenFOAM Running, Solving & CFD | 2 | July 9, 2021 03:35 |
Derivation of k-omega SST turbulence model. | dweaver123 | Main CFD Forum | 2 | August 7, 2020 12:12 |
k-omega SST blew up after first few iterations | Jinjolee | OpenFOAM | 4 | May 12, 2019 11:51 |
At high Y+ values does the K Omega SST model just behave like the K Epsilon model? | JuPa | CFX | 0 | December 22, 2015 06:44 |
Floating point exception error | lpz_michele | OpenFOAM Running, Solving & CFD | 53 | October 19, 2015 02:50 |