
[Sponsors] 
May 27, 2013, 06:17 
error on turbulence scheme

#1 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17 
Hi
I set a second order turbulence scheme with an error: Code:
divSchemes { default none; div(tauMC) Gauss linear; div(phi) Gauss linearUpwindV; div(phi,omega) Gauss upwind; div(phi,k) Gauss linearUpwind; div(phi,gas) Gauss limitedLimitedLinear 1 0 1; div(phi,epsilon) Gauss linearUpwind; } Code:
> FOAM Warning : From function polyBoundaryMesh::groupPatchIDs() const in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 474 Patch empty specifies a group empty which is also a patch name. This might give problems later on. Reading field U Reading field gas Creating turbulence model Selecting turbulence model type RASModel Selecting RAS turbulence model realizableKE realizableKECoeffs { Cmu 0.09; A0 4; C2 1.9; sigmak 1; sigmaEps 1.2; Prt 1; } fluxScheme: Kurganov Starting time loop Mean and max Courant Numbers = 3.858134887 23.51635184 deltaT = 2.083333333e09 Time = 2.08333e09 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 diagonal: Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0 diagonal: Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0 [0] swak4Foam: Allocating new repository for sampledGlobalVariables [1] swak4Foam: Allocating new repository for sampledGlobalVariables [2] swak4Foam: Allocating new repository for sampledGlobalVariables [3] swak4Foam: Allocating new repository for sampledGlobalVariables smoothSolver: Solving for Ux, Initial residual = 0.999875462, Final residual = 1.076653513e16, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 7.204656079e17, No Iterations 2 diagonal: Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0 smoothSolver: Solving for h, Initial residual = 2.679038313e06, Final residual = 5.013352019e08, No Iterations 2 time step continuity errors : sum local = 0, global = 0, cumulative = 0 [0] [0] [0] > FOAM FATAL IO ERROR: [0] attempt to read beyond EOF [0] [0] file: /home/ehsan/Desktop/Central/nonUniformMesh/test2/processor0/../system/fvSchemes.divSchemes.div(phi,epsilon) at line [3] [1] [2] [2] 61. [0] [0] From function ITstream::read(token&) [0] in file db/IOstreams/Tstreams/ITstream.C at line 83. [0] FOAM parallel run exiting [0] [1] [1] > FOAM FATAL IO ERROR: [1] attempt to read beyond EOF [1] [1] file: IOstream.divSchemes.div(phi,epsilon) at line 0 [2] > FOAM FATAL IO ERROR: [2] attempt to read beyond EOF [2] . [1] [1] From function ITstream::read(token&) [1] in file db/IOstreams/Tstreams/ITstream.C at line 83. [1] FOAM parallel run exiting [1] [3] [3] > FOAM FATAL IO ERROR: [3] attempt to read beyond EOF [3] [3] file: IOstream.divSchemes.div(phi,epsilon) at line 0. [3] [3] From function ITstream::read(token&) [3] in file db/IOstreams/Tstreams/ITstream.C at line 83. [3] FOAM parallel run exiting [3] [2] file: IOstream.divSchemes.div(phi,epsilon) at line 0. [2] [2] From function ITstream::read(token&) [2] in file db/IOstreams/Tstreams/ITstream.C at line 83. [2] FOAM parallel run exiting [2]  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.   mpirun has exited due to process rank 1 with PID 11063 on node Ehsancom exiting without calling "finalize". This may have caused other processes in the application to be terminated by signals sent by mpirun (as reported here).  [Ehsancom:11055] 3 more processes have sent help message helpmpiapi.txt / mpiabort [Ehsancom:11055] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages Killing PID 11052 PyFoam WARNING on line 232 of file /usr/local/lib/python2.7/distpackages/PyFoam/Execution/FoamThread.py : Process 11052 was already dead thanks.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

May 27, 2013, 08:21 

#2  
New Member
Phillip
Join Date: Mar 2012
Location: Germany
Posts: 27
Rep Power: 5 
Quote:
the question to me is, which version of OpenFoam you are using (the syntax is different in different versions) ? In OpenFoam 2.2.0 just do: Code:
divSchemes { default none; div(phi,U) bounded Gauss linearUpwindV grad(U); div(phi,k) bounded Gauss linearUpwind grad(k); div(phi,omega) bounded Gauss linearUpwind grad(omega); } 

May 27, 2013, 12:33 

#3 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17 
thanks Philip
yes,I use version 2.2.0 now I'm using rhoCentralFoam and it doesn't have a div(phi,U) in it. what to do with div(phi) instead? my case is unsteady and compressible. when we have to use bounded keyword?what conditions the problem should have? thanks.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

May 27, 2013, 16:50 

#4 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,503
Blog Entries: 34
Rep Power: 86 
Greetings to all!
@Ehsan: "bounded" is the default option that OpenFOAM 2.2 indicates it will use, if not present in the respective line. For more information on this characteristic, see section "4.4.2 Surface normal gradient schemes" on the User Guide. Personally, I have no clue when "bounded" or other methods should be used... But the descriptions shown in the User Guide seem selfexplanatory!? And as Phillip hinted, the problem you were having was the missing "grad(epsilon)": Code:
div(phi,epsilon) bounded Gauss linearUpwind grad(epsilon); Best regards, Bruno
__________________


June 2, 2013, 02:19 

#5 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17 
thanks.
You mean 'bounded' is related to snGrad ?or may be different to that? I removed div(phi) without OF complaining. Then OF uses a default method for this term in rhoCentralFoam?
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

June 9, 2013, 10:15 

#6  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,503
Blog Entries: 34
Rep Power: 86 
Quote:
Quote:
But after looking at the source code, here's what I found:
__________________


June 9, 2013, 11:37 

#7 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17 
thanks.
so bounded schemes can be only used in steadystate runs as i have understood. many thanks.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

June 9, 2013, 12:24 

#8 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19 
Hi,
you can use the bounded scheme in non steadystate cases too. http://www.openfoam.org/version2.2.0/numerics.php The functionallity of that scheme is defined in the libOpenSmoke thread. 

June 9, 2013, 13:07 

#9 
Senior Member
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,205
Rep Power: 17 
yes I forgot about that thread.but I yet don't know exactly when bounded scheme should be used.
my case is compressible and unsteady and haven't a convergence problem. then should I use bounded? the fvScheme I use is this,is it correct or which changes I have to do? Code:
fluxScheme Kurganov; ddtSchemes { default CrankNicolson .5; //ddt(rho) CrankNicolson .5; //ddt(rhoU) CrankNicolson .5; //ddt(rhoE) Euler; //ddt(rho,U) Euler; //ddt(rho,e) Euler; //ddt(rho,h) Euler; //ddt(rho,omega) Euler; //ddt(rho,k) Euler; //ddt(rho,gas) Euler; } gradSchemes { default none; grad(U) Gauss linear; grad(rho) Gauss linear; grad(rhoU) Gauss linear; grad((1psi)) Gauss linear; grad(e) Gauss linear; grad((1thermo:psi)) Gauss linear; grad(h) Gauss linear; grad(sqrt(((CpCv)*(1psi)))) Gauss linear; grad(sqrt(((CpCv)*(1thermo:psi)))) Gauss linear; grad(T) Gauss linear; grad(omega) cellMDLimited Gauss linear 1; grad(k) cellMDLimited Gauss linear 1; grad(gas) Gauss linear; grad(epsilon) Gauss linear; } divSchemes { default none; div(tauMC) Gauss linear; div(phi) bounded Gauss linearUpwindV; div(phi,omega) bounded Gauss linearUpwind grad(omega); div(phi,k) bounded Gauss linearUpwind grad(k); div(phi,gas) Gauss limitedLimitedLinear 1 0 1; div(phi,epsilon) bounded Gauss linearUpwind grad(epsilon); } laplacianSchemes { default none; laplacian(muEff,U) Gauss linear corrected; laplacian(alphaEff,e) Gauss linear corrected; laplacian(alpha,e) Gauss linear corrected; laplacian(k,T) Gauss linear corrected; laplacian(DepsilonEff,omega) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DomegaEff,omega) Gauss linear corrected; laplacian(alphaEff,h) Gauss linear corrected; laplacian(muEff,gas) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; } interpolationSchemes { default none; reconstruct(rho) vanLeer; reconstruct(U) vanLeerV; reconstruct(T) vanLeer; interpolate(rho) linear; interpolate(U) linear; interpolate(rhoU) linear; interpolate(muEff) linear; interpolate(tauMC) linear; } snGradSchemes { default none; snGrad(U) corrected; }
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King. To Be or Not To Be,Thats the Question! The Only Stupid Question Is the One that Goes Unasked. 

August 20, 2013, 06:57 

#10 
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 6 
hi
can any one explian that what is the definition of bounded and unbounded schemes, e.g in this table for explain behaviour of interpolation schemes, which one is better, bounded or unbounded schemes? Table 4.10. Behaviour of interpolation schemes used in divSchemes linear : Second order, unbounded skewLinear : Second order, (more) unbounded, skewness correction cubicCorrected : Fourth order, unbounded upwind : First order, bounded linearUpwind : First/second order, bounded QUICK : First/second order, bounded TVD schemes : First/second order, bounded SFCD : Second order, bounded NVD schemes : First/second order, bounded 

August 21, 2013, 06:51 

#11  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,503
Blog Entries: 34
Rep Power: 86 
Hi Saeideh,
You can find some notions of what "bounded" is on the Programmers Guide: http://foam.sourceforge.net/docs/Gui...mmersGuide.pdf Some more mentions are here: http://www.cfdonline.com/Wiki/Appro...grids__Common From the following link  http://cfd.mace.manchester.ac.uk/twi...s/cfd1pt1.pdf  I quote: Quote:
Bruno
__________________


August 21, 2013, 08:45 

#12  
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 6 
Quote:


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Wrong calculation of nut in the kOmegaSST turbulence model  FelixL  OpenFOAM Bugs  27  March 27, 2012 09:02 
how to understand high resolution scheme and high order scheme  iilw1314  Main CFD Forum  3  September 30, 2010 10:43 
Natural convection  Inlet boundary condition  max91  CFX  1  July 29, 2008 20:28 
Analyze Turbulence  Camilo Costa  CFX  7  December 4, 2006 12:00 
Stabilizing turbulence equation in channel flow  Biga  Main CFD Forum  5  March 22, 2005 21:06 