
[Sponsors] 
October 22, 2010, 13:19 
ControlDict: How to only get one time folder for the results?

#1 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
hi
Is possible with simpleFoam in time directory write only one data time directory? I want start my simulation from lastTime and when it finish my result must be overwrite on startTime directory, then i restar my simulation and again new result must be overwrite. I want only a directory Thanks 

October 22, 2010, 14:23 

#2 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,746
Rep Power: 29 
Hi Daniele
Then you should consider the purgeWrite option. Its functionality is described in details in the User Guide. However, note that it requires the use of the timeStep as writeControl option. Hope it helps and enjoy your weekend, Niels 

October 23, 2010, 11:37 

#3 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
I tried but i have one directory for each simulation, and would only one for many simulation...


October 23, 2010, 12:51 

#4 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108 
Greetings Danielle and Niels,
Interesting requirement Danielle, but "overwrite" argument option only exists for meshers, AFAIK, otherwise it would be the perfect solution for you. But you also left out one crucial piece of information: are the simulations meant to end at the same time snapshot? For example, there are three scenarios I can think of:
The concept is quite simple, so here is one solution (out of N possible solutions ) for each scenario, based on the same principle:
Best regards, Bruno
__________________


October 23, 2010, 13:02 

#5 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
I think that my case is 3! But i try to explain better my problem. I have a evolutive simulation and I use a matlab code that execute at each time step OpenFoam to calulate wall shear stress, with new wall shear matlab calculate new domain shape and I modify mesh and restart openfoam from lastTime, the problem is that on my university server I have a limited space and the simulation are very long and I can't use a lot of space!


October 23, 2010, 13:33 

#6 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108 
Hi Danielle,
Then Niels's solution should also be possible for you, as long as you:
Best regards, Bruno
__________________


October 23, 2010, 14:33 

#7 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
"Increment the endTime for each new iteration+simulation, therefore you would have to update controlDict for each simulation."
But I don't know endTime, each OpenFoam simulation stop when residuals are down 

October 23, 2010, 15:08 

#8 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,746
Rep Power: 29 
Hi Daniele
The overall framework by Bruno is functional, and if your solver stops at a given residual, you put endTime to something really, really large. Would that work? If your question about not knowing the endTime is a Matlab issue regarding which time folder to enter to do the postprocessing step, I could imagine that you might do as follows inside matlab: Code:
[s,w] = unix('ls d [09]  sort g  tail 1  tr d ''\n'''); % The ''\n'' is needed, otherwise cd(w) won't work cd(w); Best regards, Niels 

October 23, 2010, 15:15 

#9 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
Thanks
Doing a small summary, Would you post me an example of a controlDict file to see if i understand yours routine? Daniele 

October 23, 2010, 15:22 

#10 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,746
Rep Power: 29 
Honestly no. Merely combine posts #6 and #8 and you should be fine.
/ Niels 

October 23, 2010, 15:25 

#11 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
Thanks for all.
In this way Have I always only one time directory ? 

October 24, 2010, 05:27 

#12 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
Uhmm purgeWrite don't resolve my problem...Example:
I start first simulation in OpenFoam, it converges after 47 time step and simulation stops, so I have 0 and 47 time directory. I star new simulation it starts from 47, and it converges at 56 time step, but in my case directory I don't have only 0 and 56 time directory but 0 47 and 56. 

October 24, 2010, 06:21 

#13 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108 
Greetings to all!
@Niels: there is a small typo in your command in post #8; it should have an asterisk for the ls: Code:
ls d [09]* Code:
simpleFoam rm rf 0 mv `ls d [09]*  sort g  tail 1  tr d ''\n''` 0 Code:
unix('rm rf 0; mv `ls d [09]*  sort g  tail 1  tr d ''\n''` 0') Bruno
__________________
Last edited by wyldckat; October 24, 2010 at 06:37. Reason: Ooops, typo in Daniele's name... 

October 24, 2010, 06:25 

#14 
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 9 
Thanks you a lot Bruno, now it is clear! You are very useful!
Daniele 

March 19, 2016, 18:38 

#15 
Member
Ram
Join Date: Oct 2015
Posts: 35
Rep Power: 3 
Hey,
I've already run some iterations using a custom solver. After some time (approximately 100 iterations), the Courant number starts to blow up and the simulation terminates. (At least I believe it's the Co blowing up which is causing it to terminate). Now, to ensure that the Co remains less than 1 , I want to reduce deltaT in the controlDict file. But doing so does not change the deltaT when I resume the simulation. How do I change the deltaT while ensuring that the simulation starts from the point it has stopped with the updated deltaT Here's the error Courant Number mean: 0.0778162 max: 1.38578 smoothSolver: Solving for Ux, Initial residual = 0.00297599, Final residual = 7.76143e006, No Iterations 8 smoothSolver: Solving for Uy, Initial residual = 0.00559096, Final residual = 7.71217e006, No Iterations 4 DICPCG: Solving for p, Initial residual = 0.0466867, Final residual = 9.81585e007, No Iterations 754 DICPCG: Solving for p, Initial residual = 0.000445843, Final residual = 9.98038e007, No Iterations 100 DICPCG: Solving for p, Initial residual = 0.000181184, Final residual = 9.64879e007, No Iterations 53 time step continuity errors : sum local = 5.26678e010, global = 2.18292e015, cumulative = 3.17868e012 DICPCG: Solving for p, Initial residual = 0.0119082, Final residual = 9.30373e007, No Iterations 739 DICPCG: Solving for p, Initial residual = 5.90821e005, Final residual = 9.27508e007, No Iterations 26 DICPCG: Solving for p, Initial residual = 3.38914e005, Final residual = 9.32952e007, No Iterations 21 time step continuity errors : sum local = 5.04431e010, global = 2.64054e015, cumulative = 3.17604e012 DILUPBiCG: Solving for T, Initial residual = 0.0122802, Final residual = 2.62996e009, No Iterations 5 ExecutionTime = 173.687 s ClockTime = 173 s Time = 12.1485 Courant Number mean: 0.0780047 max: 1.6609 smoothSolver: Solving for Ux, Initial residual = 0.00329476, Final residual = 4.90866e+227, No Iterations 1000 smoothSolver: Solving for Uy, Initial residual = 0.00622384, Final residual = 1.32554e+227, No Iterations 1000 DICPCG: Solving for p, Initial residual = 1, Final residual = nan, No Iterations 1001 DICPCG: Solving for p, Initial residual = nan, Final residual = nan, No Iterations 1001 > FOAM FATAL IO ERROR: wrong token type  expected Scalar, found on line 0 the word 'nan' file: C:/OpenFOAM/cygwin64/opt/OpenFOAM/OpenFOAM2.3.x/tutorials/incompressible/icoFoam/laminar_pipe U=2/system/data.solverPerformance.p at line 0. From function operator>>(Istream&, Scalar&) in file lnInclude/Scalar.C at line 93. FOAM exiting And here's my controlDict file /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application my_icoFoam; startFrom latestTime; startTime 0; stopAt endTime; endTime 25; deltaT 0.0005; writeControl timeStep; writeInterval 200; purgeWrite 0; writeFormat binary; writePrecision 6; writeCompression off; timeFormat general; maxCo 0.6; adjustTimeStep yes; timePrecision 6; runTimeModifiable true; // ************************************************** *********************** // Thanks!! Ram 

March 20, 2016, 05:38 

#16 
Senior Member
Join Date: Aug 2014
Location: N/A
Posts: 139
Rep Power: 4 
Hi,
adjustTimeStep is not implemented in icoFoam natively, so you can maybe try to implement it in your custom icoFoam solver for convenience. (i think i saw threads on this topic in the forum) If you want to restart your simulation from the latest time with adjusted time step size, you simply check the latest saved time folder (in your cases possibly 12.1 or something) open your controDict file and change the startTime to this last saved time step, where your simulation converged. Don't forget to adjust the time step also. But as i mentioned adjustable run time is the more convinient way to cope with increasing courant numbers. Have fun. 

March 21, 2016, 12:47 

#17 
Member
Ram
Join Date: Oct 2015
Posts: 35
Rep Power: 3 
Hey BlnPhoenix,
I tried doing what you'd suggested but its not working...This is what I tried. This is my custom solver. And I used setDeltaT in the hope that it will read the deltaT from the controlDict file. #include "fvCFD.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { #include "setRootCase.H" #include "createTime.H" #include "createMesh.H" #include "createFields.H" #include "initContinuityErrs.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nStarting time loop\n" << endl; while (runTime.run()) { Info<< "Time = " << runTime.timeName() << nl << endl; #include "readPISOControls.H" #include "readTimeControls.H" #include "CourantNo.H" #include "setDeltaT.H" runTime() ++; fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U) ); solve(UEqn == fvc::grad(p)); //  PISO loop for (int corr=0; corr<nCorr; corr++) { volScalarField rAU(1.0/UEqn.A()); volVectorField HbyA("HbyA", U); HbyA = rAU*UEqn.H(); surfaceScalarField phiHbyA ( "phiHbyA", (fvc::interpolate(HbyA) & mesh.Sf()) + fvc::interpolate(rAU)*fvc::ddtCorr(U, phi) ); adjustPhi(phiHbyA, U, p); for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++) { fvScalarMatrix pEqn ( fvm::laplacian(rAU, p) == fvc::div(phiHbyA) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (nonOrth == nNonOrthCorr) { phi = phiHbyA  pEqn.flux(); } } #include "continuityErrs.H" U = HbyA  rAU*fvc::grad(p); U.correctBoundaryConditions(); } fvScalarMatrix TEqn ( fvm::ddt(T) + fvm::div(phi, T)  fvm::laplacian(DT, T) ); TEqn.solve(); runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; } Info<< "End\n" << endl; return 0; } // ************************************************** *********************** // Now here's what I get when I run the solver for my case Time = 12.15578 Courant Number mean: 0.0111567 max: 0.511585 deltaT = 6.45436e005 smoothSolver: Solving for Ux, Initial residual = 0.00180382, Final residual = 6.162e007, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.00295248, Final residual = 2.7079e007, No Iterations 2 DICPCG: Solving for p, Initial residual = 0.0164652, Final residual = 9.7402e007, No Iterations 732 DICPCG: Solving for p, Initial residual = 4.28776e005, Final residual = 8.91207e007, No Iterations 12 DICPCG: Solving for p, Initial residual = 1.30543e005, Final residual = 8.37702e007, No Iterations 5 time step continuity errors : sum local = 5.25956e011, global = 1.0707e015, cumulative = 6.64415e011 DICPCG: Solving for p, Initial residual = 0.000841824, Final residual = 9.98842e007, No Iterations 450 DICPCG: Solving for p, Initial residual = 4.01403e006, Final residual = 9.26023e007, No Iterations 10 DICPCG: Solving for p, Initial residual = 2.30103e006, Final residual = 8.52151e007, No Iterations 2 time step continuity errors : sum local = 5.35375e011, global = 3.18539e012, cumulative = 6.32561e011 DILUPBiCG: Solving for T, Initial residual = 0.00547638, Final residual = 1.73926e009, No Iterations 3 ExecutionTime = 839.743 s ClockTime = 840 s Time = 12.15584 Courant Number mean: 0.0109212 max: 0.510881 deltaT = 6.3169e005 smoothSolver: Solving for Ux, Initial residual = 0.00179596, Final residual = 5.92427e007, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.00296089, Final residual = 2.65592e007, No Iterations 2 DICPCG: Solving for p, Initial residual = 0.0179838, Final residual = 9.62282e007, No Iterations 731 DICPCG: Solving for p, Initial residual = 3.90246e005, Final residual = 8.9584e007, No Iterations 12 DICPCG: Solving for p, Initial residual = 1.18486e005, Final residual = 8.32487e007, No Iterations 5 time step continuity errors : sum local = 5.14033e011, global = 3.29354e015, cumulative = 6.32529e011 The Co is no longer blowing up. But the time is not advancing by the step given in the controlDict. If I let the solver solve for some more time, the significant digits in the time reach an absurdly large 810 (for example the time shown in the command terminal becomes 12.16543879...). I want the time to advance by the deltaT mentioned in the controlDict. Any help is greatly appreciated. Thanks!! Ram 

March 21, 2016, 13:03 

#18 
Senior Member
Join Date: Aug 2014
Location: N/A
Posts: 139
Rep Power: 4 
Hi,
so the time in the terminal 12.16543879 would mean that your time step size gets smaller and smaller i suppose. This on the other hand would mean that you have implentend an adjustable time step into the solver. Unfortunatly i have no experience with custom solvers so i cannot say whether the error may be in the implementation into your custom icoFoam solver or in the problem itself (boundary conditions etc.) ( So yea, can you please check that you have set your controlDict to adjustTimeStep no; and writeControl timeStep; if u want a fixed time step for your simulation?! Maybe someone else can be of more help. Good luck. 

March 21, 2016, 17:17 

#19 
Member
Ram
Join Date: Oct 2015
Posts: 35
Rep Power: 3 
Hey BlnPhoenix,
Thanks for your reply. I changed the write control to timeStep and tried again. Now the solver is giving a warning regarding timePrecision. This is what it says Time = 12.1401 Courant Number mean: 0.00768437 max: 0.0709925 > FOAM Warning : From function Time:perator++() in file db/Time/Time.C at line 1055 Increased the timePrecision from 6 to 18 to distinguish between timeNames at time 12.1401 smoothSolver: Solving for Ux, Initial residual = 0.000179277, Final residual = 9.51591e009, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 0.000461942, Final residual = 1.47774e008, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.0460253, Final residual = 9.43666e007, No Iterations 734 DICPCG: Solving for p, Initial residual = 0.00357939, Final residual = 9.96147e007, No Iterations 315 DICPCG: Solving for p, Initial residual = 0.00136696, Final residual = 9.94625e007, No Iterations 131 time step continuity errors : sum local = 1.01988e011, global = 1.34098e013, cumulative = 1.31505e013 DICPCG: Solving for p, Initial residual = 0.000789953, Final residual = 9.43314e007, No Iterations 312 DICPCG: Solving for p, Initial residual = 0.000349991, Final residual = 9.73125e007, No Iterations 57 DICPCG: Solving for p, Initial residual = 0.000195612, Final residual = 9.82302e007, No Iterations 76 time step continuity errors : sum local = 1.00649e011, global = 1.88417e013, cumulative = 3.19922e013 DILUPBiCG: Solving for T, Initial residual = 0.000736939, Final residual = 1.67772e008, No Iterations 1 ExecutionTime = 30.088 s ClockTime = 30 s Time = 12.1401000000000003 Courant Number mean: 0.00768449 max: 0.0717468 smoothSolver: Solving for Ux, Initial residual = 0.000172211, Final residual = 8.9619e009, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 0.000430594, Final residual = 1.20743e008, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.0289387, Final residual = 9.32201e007, No Iterations 725 It proceeds but the time precision is now 18!! I'm attaching my solver code and Boundary conditions file as well. The case is a simple laminar flow through a pipe. If someone can figure out why this is happening it'll be of great help! Solver: myicoFoam.C /**\ =========  \\ / F ield  OpenFOAM: The Open Source CFD Toolbox \\ / O peration  \\ / A nd  Copyright (C) 20112013 OpenFOAM Foundation \\/ M anipulation   License This file is part of OpenFOAM. OpenFOAM is free software: you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any later version. OpenFOAM is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details. You should have received a copy of the GNU General Public License along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>. Application icoFoam Description Transient solver for incompressible, laminar flow of Newtonian fluids. \**/ #include "fvCFD.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { #include "setRootCase.H" #include "readTimeControls.H" #include "createTime.H" #include "createMesh.H" #include "createFields.H" #include "initContinuityErrs.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nStarting time loop\n" << endl; while (runTime.run()) { #include "readPISOControls.H" #include "CourantNo.H" #include "setDeltaT.H" Info<< "Time = " << runTime.timeName() << nl << endl; fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U) ); solve(UEqn == fvc::grad(p)); //  PISO loop for (int corr=0; corr<nCorr; corr++) { volScalarField rAU(1.0/UEqn.A()); volVectorField HbyA("HbyA", U); HbyA = rAU*UEqn.H(); surfaceScalarField phiHbyA ( "phiHbyA", (fvc::interpolate(HbyA) & mesh.Sf()) + fvc::interpolate(rAU)*fvc::ddtCorr(U, phi) ); adjustPhi(phiHbyA, U, p); for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++) { fvScalarMatrix pEqn ( fvm::laplacian(rAU, p) == fvc::div(phiHbyA) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (nonOrth == nNonOrthCorr) { phi = phiHbyA  pEqn.flux(); } } #include "continuityErrs.H" U = HbyA  rAU*fvc::grad(p); U.correctBoundaryConditions(); } fvScalarMatrix TEqn ( fvm::ddt(T) + fvm::div(phi, T)  fvm::laplacian(DT, T) ); TEqn.solve(); runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; } Info<< "End\n" << endl; return 0; } // ************************************************** *********************** // controlDict: /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application myicoFoam; startFrom latestTime; startTime 0; stopAt endTime; endTime 25; deltaT 0.00005; writeControl timeStep; writeInterval 200; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; maxCo 0.6; adjustTimeStep no; timePrecision 6; runTimeModifiable true; // ************************************************** *********************** // O folder P: /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 2 0 0 0 0]; internalField uniform 0; boundaryField { INLET { type zeroGradient; } OUTLET { type fixedValue; value uniform 0; } TOP_WALL_STRAIGHT { type zeroGradient; } BOTTOM_WALL_STRAIGHT { type zeroGradient; } BOTTOM_WALL_WAVY { type zeroGradient; } TOP_WALL_WAVY { type zeroGradient; } frontAndBackPlanes { type empty; } } // ************************************************** *********************** // T: /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; object T; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 1 0 0 0]; internalField uniform 300; boundaryField { INLET { type fixedValue; value uniform 300; } OUTLET { type zeroGradient; } TOP_WALL_STRAIGHT { type fixedValue; value uniform 330; } BOTTOM_WALL_STRAIGHT { type fixedValue; value uniform 330; } BOTTOM_WALL_WAVY { type fixedValue; value uniform 330; } TOP_WALL_WAVY { type fixedValue; value uniform 330; } frontAndBackPlanes { type empty; } } // ************************************************** *********************** // U: /** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 1 0 0 0 0]; internalField uniform (2 0 0); boundaryField { INLET { type fixedValue; value uniform (2 0 0); } OUTLET { type zeroGradient; } TOP_WALL_STRAIGHT { type fixedValue; value uniform (0 0 0); } BOTTOM_WALL_STRAIGHT { type fixedValue; value uniform (0 0 0); } BOTTOM_WALL_WAVY { type fixedValue; value uniform (0 0 0); } TOP_WALL_WAVY { type fixedValue; value uniform (0 0 0); } frontAndBackPlanes { type empty; } } // ************************************************** *********************** // 

March 21, 2016, 17:23 

#20 
Member
Ram
Join Date: Oct 2015
Posts: 35
Rep Power: 3 
I tried removing timePrecision and maxCo from the controlDict file but still its changing the precision to 18 and proceeding. Thought this might help...


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
refineWallLayer Error  Yuby  OpenFOAM Meshing & Mesh Conversion  1  May 19, 2017 10:13 
High Courant Number @ icoFoam  Artex85  OpenFOAM Running, Solving & CFD  11  February 16, 2017 14:40 
Help for the small implementation in turbulence model  shipman  OpenFOAM Programming & Development  25  March 19, 2014 11:08 
AMI speed performance  danny123  OpenFOAM  19  October 24, 2012 07:44 
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3  bookie56  OpenFOAM Installation  8  August 13, 2011 04:03 