|
[Sponsors] |
Continuity error cannot be removed by adjusting the outflow |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 16, 2015, 22:22 |
Continuity error cannot be removed by adjusting the outflow
|
#1 |
New Member
Luis Felipe Rojas
Join Date: Aug 2015
Posts: 13
Rep Power: 11 |
Good Morning , My name is Luis Rojas . I am trying to process a mesh with a open atmosphere channel . My enviormental configurations are Velocity in movingWall is 37 on the x-axis else 0 in y and z axis; Preassure in movingWall is 0 , Preassure in frontAndBack is 73120 Pascals. I want to process that mesh on the cavity case. So next I paste my configurations for each variable. The problem is .... Anyway I execute the comand ''icoFoam''. OpenFoam show's me that. I will apreciatte too much if you help me to Know what is happening on my simulation for Future Practices publish a Tutorial Solving this trouble.
Code:
$ icoFoam /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.x | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ /* Windows port by CFD support (www.cfdsupport.com) [based on Symscape] *\ \*---------------------------------------------------------------------------*/ Build : 2.3.x-819030ed51bd Exec : C:\OpenFOAM\cygwin64\opt\OpenFOAM\OpenFOAM-2.3.x\platforms\cygwin64mingw-w64DPOpt\bin\icoFoam.exe Date : Dec 16 2015 Time : 03:42:33 Host : "EQUIPO2" PID : 2100 Case : C:/OpenFOAM/cygwin64/opt/OpenFOAM/OpenFOAM-2.3.x/FelipeT/incompressible/icoFoam/SimFelipe/CavityQuebrada/Cavity1 nProcs : 1 fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading transportProperties Reading field p Reading field U Reading/calculating face flux field phi Starting time loop Time = 0.05 Courant Number mean: 0.0595329 max: 121.711 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 6.45652e-006, No Iterations 12 smoothSolver: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0 smoothSolver: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0 --> FOAM FATAL ERROR: Continuity error cannot be removed by adjusting the outflow. Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow. Total flux : 368.881 Specified mass inflow : 10.4802 Specified mass outflow : 0 Adjustable mass outflow : 0 From function adjustPhi(surfaceScalarField&, const volVectorField&,volScalarField&) in file cfdTools/general/adjustPhi/adjustPhi.C at line 122. FOAM exiting For the Velocity i have this Code:
/*--------------------------------*- 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 (0 0 0); boundaryField { movingWall { type fixedValue; value uniform (37 0 0); } fixedWalls { type fixedValue; value uniform (0 0 0); } frontAndBack { type fixedValue; value uniform (0 0 0); } } // ************************************************** *********************** // Code:
/*--------------------------------*- 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 { movingWall { type zeroGradient; } fixedWalls { type zeroGradient; } frontAndBack { type fixedFluxPressure; value uniform 73120; } } // ************************************************** *********************** // https://drive.google.com/file/d/0B1P...I2R2pMZTg/view https://drive.google.com/file/d/0B1P...V6SFp6clU/view https://drive.google.com/file/d/0B1P...E0YU5IMzA/view https://drive.google.com/file/d/0B1P...VJaFVydTg/view https://drive.google.com/file/d/0B1P...FKdFNMVFk/view Last edited by wyldckat; December 19, 2015 at 15:59. Reason: Added [CODE][/CODE] markers |
|
December 19, 2015, 16:12 |
|
#2 | ||
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,982
Blog Entries: 45
Rep Power: 128 |
Greetings Luis Rojas,
There are two problems that I can see. The first one: Quote:
Remember seeing that in the OpenFOAM User Guide, the tutorial for the cavity case tells us that it's using pseudo-2D, by defining the front and back patches as type "empty"? This was also defined in the "blockMeshDict", which consequently means that the same will happen to the resulting file "constant/polyMesh/boundary". More details in subsection "5.2.1 Specification of patch types in OpenFOAM" of the User Guide: http://cfd.direct/openfoam/user-guide/boundaries/ The second issue is this: Quote:
For example, if you want the fluid to exit through the patch "frontAndBack", you need to define the boundary condition like this in the file "U": Code:
frontAndBack { type zeroGradient; } Bruno
__________________
|
|||
Tags |
cavity problem, continuity equation, continuity error, icofoam problem |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Continuity error cannot be removed by adjusting the outflow. Please check the velocit | range_rover | OpenFOAM Running, Solving & CFD | 7 | August 17, 2016 02:12 |
potentialFoam doesnt start?! | Sway | OpenFOAM Running, Solving & CFD | 0 | July 2, 2015 08:48 |
Continuity error cannot be removed by adjusting the outflow | fontania | OpenFOAM Running, Solving & CFD | 1 | October 9, 2012 11:36 |
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 | bookie56 | OpenFOAM Installation | 8 | August 13, 2011 05:03 |
Could anybody help me see this error and give help | liugx212 | OpenFOAM Running, Solving & CFD | 3 | January 4, 2006 19:07 |