# IcoFoam continuity error in 2D transient simulation

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

 October 27, 2005, 12:09 I am running a basic test case #1 New Member   Craig Finch Join Date: Mar 2009 Location: Orlando, FL, USA Posts: 4 Rep Power: 8 I am running a basic test case using icoFoam. I defined a 2D channel with two walls, an inlet, and an outlet. The walls have a no-slip boundary condition U=uniform(0 0 0). The inlet has a boundary condition of U=uniform(1 0 0) which causes flow into the channel with a uniform velocity profile. The outlet BC is of type zeroGradient for U. All pressure boundaries are of type zeroGradient. This setup produces the following error: Reading/calculating face flux field phi Starting time loop Time = 0.001 Mean and max Courant Numbers = 0 0.1 BICCG: Solving for Ux, Initial residual = 1, Final residual = 9.49086e-09, No Iterations 1 --> 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. From function adjustPhi(surfaceScalarField& phi, const volVectorField& U,const volScalarField& p in file adjustPhi/adjustPhi.C at line 108. FOAM exiting If I set one wall b.c. OR the internalField to U=uniform(0.00001 0 0) then the expected parabolic velocity profile develops. Reducing the time step does not help. Can someone please explain why this is happening, and how to set it up correctly?

 October 27, 2005, 12:30 Have a look at your boundary c #2 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,763 Rep Power: 21 Have a look at your boundary conditions on the velocity. In FOAM, we typically use fixed value U and zero gradient pressure at the inlet and fixed pressure and zero gradient U at the outlet. There is an option of using zero gradient on both p and U at the outlet, but then the code needs to adjust the outlet velocities in order to achieve global continuity. The message says it cannot do that for some reason. Enjoy, Hrv kid and Pirlu like this. __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 October 27, 2005, 23:49 Oops. I thought I had set the #3 New Member   Craig Finch Join Date: Mar 2009 Location: Orlando, FL, USA Posts: 4 Rep Power: 8 Oops. I thought I had set the output pressure to zero instead of zeroGradient, but after checking I realize that it was in fact zeroGradient. No wonder it wasn't working. Thanks for the tip. I'll post my results as a tutorial sometime. chqingyuan likes this.

 March 27, 2012, 01:42 Thank You #4 Senior Member   cfdkid Join Date: Mar 2009 Posts: 133 Rep Power: 8 Hello Hrv, Your comments helped a lot. regards, cfdkid

 September 24, 2013, 17:11 #5 New Member   Join Date: Feb 2011 Posts: 7 Rep Power: 6 great help. Also valid for SimpleFoam!!! thanks a lot!!!

November 16, 2014, 00:06
Continuity error in sloshingtank2d
#6
Senior Member

Join Date: Mar 2009
Posts: 307
Rep Power: 9
Quote:
 Originally Posted by hjasak Have a look at your boundary conditions on the velocity. In FOAM, we typically use fixed value U and zero gradient pressure at the inlet and fixed pressure and zero gradient U at the outlet. There is an option of using zero gradient on both p and U at the outlet, but then the code needs to adjust the outlet velocities in order to achieve global continuity. The message says it cannot do that for some reason. Enjoy, Hrv
Dear all:

I am running sloshingTank2D in interDYMFoam. Tank dimensions in the y direction (horizontal) is 11 meters; vertical 7 meters. Water depth is 4.4 meters. There is no inflow or outflow. However I get a error message as follows:
[5] --> FOAM FATAL ERROR:
[5] 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 : 4.06534e-16
Specified mass inflow : 5.66242e-19
Specified mass outflow : 8.26281e-19
[5]
[5]
[5] From function adjustPhi(surfaceScalarField& phi, const volVectorField& U,const volScalarField& p
[5]
FOAM parallel run exiting
[5]
[4]
[4]
[4] --> FOAM FATAL ERROR:
[4] 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 : 4.06534e-16
Specified mass inflow : 5.66242e-19
Specified mass outflow : 8.26281e-19

Can any tell me why I am getting this error? Thankyou.

 February 20, 2015, 03:22 #7 Member   Raitis Lebdevs Join Date: Feb 2015 Location: Latvia Posts: 37 Rep Power: 2 Your error says that your inflow and your outflow is not the same. Look at your BC, they need to deal with the same amount of flux comming in and out.

February 20, 2015, 09:09
#8
Senior Member

Join Date: Mar 2009
Posts: 307
Rep Power: 9
Quote:
 Originally Posted by rietis Your error says that your inflow and your outflow is not the same. Look at your BC, they need to deal with the same amount of flux comming in and out.
Thankyou for your response. I am simulating a tank in sloshingtank2d. What is realized is that this error was given due to a run time error. It is one of those cases where a run time error creates other cascading errors.

 February 20, 2015, 09:20 #9 Member   Raitis Lebdevs Join Date: Feb 2015 Location: Latvia Posts: 37 Rep Power: 2 Dear, musahossein, do you have expirience in snappyHexMesh? If you have and are willing to look on a problem I would appriciate. here is a link: Refining mesh at the walls cheers Raitis.

February 20, 2015, 10:30
#10
Senior Member

Join Date: Mar 2009
Posts: 307
Rep Power: 9
Quote:
 Originally Posted by rietis Dear, musahossein, do you have expirience in snappyHexMesh? If you have and are willing to look on a problem I would appriciate. here is a link: Refining mesh at the walls cheers Raitis.
Unfortunately, I do not. Another way you can refine the mesh at the walls is to subdivide our domaing into smaller blocks. By doing so you can refine the mesh in the block of your choice. However this requires that you redefine your model with more nodes as the blocks must be defined with nodes. One drawback of this method is that the mesh must be the same in at least one direction as the mesh in adjacent blocks must match. Sorry I could not help you more.

 February 20, 2015, 10:59 #11 Member   Raitis Lebdevs Join Date: Feb 2015 Location: Latvia Posts: 37 Rep Power: 2 No worries. Yes I undarstand that it is a way, but this time I need to do with this method.

May 5, 2015, 11:43
#12
New Member

Chen Linya
Join Date: Oct 2014
Posts: 4
Rep Power: 2
Quote:
 Originally Posted by musahossein Dear all: I am running sloshingTank2D in interDYMFoam. Tank dimensions in the y direction (horizontal) is 11 meters; vertical 7 meters. Water depth is 4.4 meters. There is no inflow or outflow. However I get a error message as follows: [5] --> FOAM FATAL ERROR: [5] 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 : 4.06534e-16 Specified mass inflow : 5.66242e-19 Specified mass outflow : 8.26281e-19 Adjustable mass outflow : 0 [5] [5] [5] From function adjustPhi(surfaceScalarField& phi, const volVectorField& U,const volScalarField& p [5] in file cfdTools/general/adjustPhi/adjustPhi.C at line 118. [5] FOAM parallel run exiting [5] [4] [4] [4] --> FOAM FATAL ERROR: [4] 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 : 4.06534e-16 Specified mass inflow : 5.66242e-19 Specified mass outflow : 8.26281e-19 Adjustable mass outflow : 0 Can any tell me why I am getting this error? Thankyou.
Dear, musahossein
I am expirienceing this problem,can you tell me the details about the run time error?

May 5, 2015, 13:48
#13
Senior Member

Join Date: Mar 2009
Posts: 307
Rep Power: 9
Quote:
 Originally Posted by Chen Linya Dear, musahossein I am expirienceing this problem,can you tell me the details about the run time error?
In my case the run time error was due to other errors during run time. The applied displacement was so large that essentially the tank was dispalcement by more than half its length. So I would suggest that you look at your data and then the results of your run using ParaFOAM upto the point where the error occurs. May be you will discover some error in modeling or input which, if taken care of will not generate this type of error message.

Also, are you running the latest version of OpenFOAM? From what I hear, it is more robust and handles these types of errors better.

May 6, 2015, 01:25
#14
New Member

Chen Linya
Join Date: Oct 2014
Posts: 4
Rep Power: 2
Quote:
 Originally Posted by musahossein In my case the run time error was due to other errors during run time. The applied displacement was so large that essentially the tank was dispalcement by more than half its length. So I would suggest that you look at your data and then the results of your run using ParaFOAM upto the point where the error occurs. May be you will discover some error in modeling or input which, if taken care of will not generate this type of error message. Also, are you running the latest version of OpenFOAM? From what I hear, it is more robust and handles these types of errors better.
I use the foam-extend-3.1,i want to combine the icoFsiFoam and interFoam to a interFsiFoam to couple with multiphase fluid-struction interaction problem(dambreak with a elastic baffle),and the error occured in first interation(and i guess) due to the fluid mesh moving.the dynamicMeshDict as follow:
dynamicFvMesh dynamicMotionSolverFvMesh;
twoDMotion yes;
solver laplace;
frozenDiffusion on;
distancePatches(consoleFluid);

 May 7, 2015, 10:04 #15 Senior Member   musaddeque hossein Join Date: Mar 2009 Posts: 307 Rep Power: 9 I would suggest that you check your mesh, Start with checkmesh or (CheckMesh?) command once you have run blockMesh, to make sure OpenFOAM is ok with your aspect ratio. Once you have established that it is not a aspect ratio problem, it is more likely how you are communicating the input data to OpenFOAM, or how you have set up the problem. Check those in a systematic manner.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post agrewal OpenFOAM Running, Solving & CFD 3 February 9, 2008 18:12 Li CFX 0 July 25, 2007 11:27 sree CFX 0 November 2, 2005 11:03 Korsh Mik CFX 1 November 2, 2005 10:08 guru FLUENT 2 February 7, 2005 10:33

All times are GMT -4. The time now is 18:42.