
[Sponsors] 
April 18, 2017, 01:53 
simpleFoam postProcess func R

#1 
Member
Join Date: Apr 2017
Posts: 68
Rep Power: 9 
Hi,
I have trouble getting results for the Reynold's stresses when using the command Code:
simpleFoam postProcess func R Code:
Build : 4.1 Exec : simpleFoam postProcess func R Date : Apr 18 2017 Time : 07:42:47 Host : "" PID : 10656 Case : /home/.../run16 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Allowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 SIMPLE: convergence criteria field p tolerance 0.01 field U tolerance 0.001 field "(kepsilonomegafv2)" tolerance 0.001 turbulenceFields R: storing fields: turbulenceProperties:R Time = 0 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model type RAS Selecting RAS turbulence model kOmegaSST Selecting patchDistMethod meshWave kOmegaSSTCoeffs { alphaK1 0.85; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.856; gamma1 0.555556; gamma2 0.44; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; b1 1; c1 10; F3 false; } No MRF models present > FOAM Warning : > FOAM FATAL IO ERROR: keyword boundaryField is undefined in dictionary "/home/.../run16/0/turbulenceProperties:R" file: /home/.../run16/0/turbulenceProperties:R from line 18 to line 20. From function const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&) const in file db/dictionary/dictionary.C at line 642. Code:
FoamFile { version 2.0; format ascii; class volSymmTensorField; location "0"; object turbulenceProperties:R; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 2 0 0 0 0]; internalField uniform (0.233333 0 0 0.233333 0 0.233333); 

March 23, 2018, 12:59 

#2 
Member
Andrew O. Winter
Join Date: Aug 2015
Location: Seattle, WA, USA
Posts: 78
Rep Power: 10 
Hello Kaaja,
I realize this is roughly a year later, but I was wondering if you figured out your problem (since I believe I'm having a similar one)? My guess after reading the error is that it looks like you were missing boundary condition definitions for the Reynolds stress tensor since all that the command "<solverName> postProcess func R" does is to generate a file that has the full field data for each cell without specifying any boundary conditions. If this was the case, what sort of boundary conditions did you apply for R? Also, do you have to change the file name from "turbulenceProperties:R" (the file name generated by the postProcess command) to "R" in the time directories? After looking at the source code in "LRR.H" and "LRR.C" it looks like they're using "R". Best regards, Andrew PS  In case it matters, I've attached the error report and I am using Pablo Higuera's "olaDyMFoam" solver, which is a modification of the standard "interFoam" solver to allow for dynamic mesh motion for wave generation boundary conditions (I'm trying to model a piston wave maker in a long flume; see https://github.com/phicau/olaFlow for the solver code). 

March 29, 2018, 09:25 

#3 
Member
Join Date: Apr 2017
Posts: 68
Rep Power: 9 
Hello Andrew,
I am sad to say that I don't remember if I solved that problem, and that I don't have capacity these next 2 months checking it eighter (lot of work). Probably not the same thing, but I found the following 2 posts I did on somewhat related topics How to sample turbulenceProperties:R? https://www.cfdonline.com/Forums/openfoam/187909reportingturbulencefields.html I hope you will work it out! 

March 29, 2018, 17:40 

#4 
Member
Andrew O. Winter
Join Date: Aug 2015
Location: Seattle, WA, USA
Posts: 78
Rep Power: 10 
Thanks kaaja,
I managed to get my LRR simulation working using Rxx = Ryy = Rzz = 2k/3 and Rxy = Rxz = Ryz = 0 for the internalField. I used the following BCs for R in my 0 directory. For a solid wall boundary... Code:
flumeWall { type kqRWallFunction; value uniform (0 0 0 0 0 0); } Code:
atmosphere { type inletOutlet; inletValue uniform (0 0 0 0 0 0); value uniform (0 0 0 0 0 0); } For fvSchemes I used... Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { div(rhoPhi,U) Gauss limitedLinearV 1; div(U) Gauss linear; div(phi,alpha) Gauss vanLeer; div(phirb,alpha) Gauss interfaceCompression; div((muEff*dev(T(grad(U))))) Gauss linear; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,omega) Gauss upwind; div(phi,R) Gauss upwind; div((rhoPhiinterpolate(porosity)),U) Gauss limitedLinearV 1; div(rhoPhiPor,UPor) Gauss limitedLinearV 1; div(rhoPhi,UPor) Gauss limitedLinearV 1; div(rhoPhiPor,U) Gauss limitedLinearV 1; div((phiinterpolate(porosity)),k) Gauss upwind; div((phiinterpolate(porosity)),epsilon) Gauss upwind; div((phiinterpolate(porosity)),omega) Gauss upwind; div((phiinterpolate(porosity)),R) Gauss upwind; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p_rgh; pcorr; alpha.water; } wallDist { method meshWave; } Code:
solvers { "alpha.water.*" { nAlphaCorr 1; nAlphaSubCycles 2; alphaOuterCorrectors yes; cAlpha 1; MULESCorr no; nLimiterIter 3; solver smoothSolver; smoother symGaussSeidel; tolerance 1e8; relTol 0; } "pcorr.*" { solver PCG; preconditioner DIC; tolerance 1e5; relTol 0; } pcorrFinal { $pcorr; relTol 0; } p_rgh { solver PCG; preconditioner DIC; tolerance 1e07; relTol 0.05; } p_rghFinal { $p_rgh; relTol 0; } "(Ukepsilon).*" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e06; relTol 0; } R { solver smoothSolver; smoother symGaussSeidel; tolerance 1e8; relTol 0; } RFinal { $R; tolerance 1e08; relTol 0; } cellDisplacement { solver GAMG; tolerance 1e5; relTol 0; smoother GaussSeidel; cacheAgglomeration false; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } cellDisplacementFinal { $cellDisplacement; relTol 0; } } PIMPLE { momentumPredictor no; nOuterCorrectors 1; nCorrectors 3; nNonOrthogonalCorrectors 0; } relaxationFactors { fields { } equations { ".*" 1; } } 

March 29, 2018, 17:48 

#5 
Member
Andrew O. Winter
Join Date: Aug 2015
Location: Seattle, WA, USA
Posts: 78
Rep Power: 10 
Also, I forgot to say that I ended up just making a brand new R file in my 0 time directory with the boundary conditions I mentioned previously so I got away with not using the recommended approach of first running a simpler model (kEpsilon) and then changing to the RSM model (LRR).
Since my simulation went so well, I also tried using the SSG model in this same manner at first, which blew up after 0.6 s (my endTime is 25 s). Then I tried using the LRR results at 0.5 s as an initial state for switching to the SSG model, but it also blew up near 1 s so for now I'm just sticking with the LRR model. 

Tags 
boundaryfield, reynolds stress 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
postProcess Utility: icoFoam noFunctionObjects Why?How?  TeresaT  OpenFOAM PostProcessing  8  July 26, 2023 02:41 
interFoam vs. simpleFoam channel flow comparison  DanM  OpenFOAM Running, Solving & CFD  12  January 31, 2020 15:26 
postProcess functionality in openFOAM 4  bullmut  OpenFOAM PostProcessing  23  July 21, 2017 09:11 
simpleFoam parallel solver & Fluent polyhedral mesh  Zlatko  OpenFOAM Running, Solving & CFD  3  September 26, 2014 06:53 
Trying to run a benchmark case with simpleFoam  spsb  OpenFOAM  3  February 24, 2012 09:07 