CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Continuity error cannot be removed by adjusting the outflow

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 16, 2015, 21:22
Exclamation Continuity error cannot be removed by adjusting the outflow
  #1
New Member
 
Luis Felipe Rojas
Join Date: Aug 2015
Posts: 13
Rep Power: 8
luisfeliperojas95 is on a distinguished road
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
I dont Know why OpenFOAM is showing me an error with the outlet and inlet.

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);
}
}

// ************************************************** *********************** //
For Preassure 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 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;
}
}

// ************************************************** *********************** //
Next I attached the Mesh Images.

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 14:59. Reason: Added [CODE][/CODE] markers
luisfeliperojas95 is offline   Reply With Quote

Old   December 19, 2015, 15:12
Default
  #2
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 125
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings Luis Rojas,

There are two problems that I can see. The first one:
Quote:
Originally Posted by luisfeliperojas95 View Post
Code:
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
This means that the Y and Z directions are of type "empty" and were not solved.
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:
Originally Posted by luisfeliperojas95 View Post
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);
}
}

// ************************************************** *********************** //
It looks like the fluid is being injected on one end of the geometry, namely through the one named "movingWall". This means that you are asking icoFoam to compress the fluid inside the mesh, because there is no exit defined in any of the other patches. But icoFoam cannot compress fluid, because it's only able to deal with incompressible fluids.

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;
}
Best regards,
Bruno
luisfeliperojas95 likes this.
__________________
wyldckat is offline   Reply With Quote

Reply

Tags
cavity problem, continuity equation, continuity error, icofoam problem

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 01:12
potentialFoam doesnt start?! Sway OpenFOAM Running, Solving & CFD 0 July 2, 2015 07:48
Continuity error cannot be removed by adjusting the outflow fontania OpenFOAM Running, Solving & CFD 1 October 9, 2012 10:36
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 bookie56 OpenFOAM Installation 8 August 13, 2011 04:03
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 18:07


All times are GMT -4. The time now is 19:40.