View Issue Details

Jump to NotesJump to History
IDProjectCategoryView StatusDate SubmittedLast Update
0000663OpenFOAMBugpublic2012-10-15 09:232022-05-18 11:08
Reporteruser525Assigned Towill  
PriorityurgentSeveritymajorReproducibilityalways
Status resolvedResolutionfixed 
PlatformLinuxOSUbuntuOS Version12.04.01 64 bit
Fixed in Versiondev 
Summary0000663: AMI corrupts passive scalar
DescriptionThe passive scalar are NOT correctly calculated when using AMI.

Using a simple tutorial case (mixerVesselAMI2D) with fixedvalue uniform T (as example), immediately are shown cells with higher and lower temperature close to one wing (interesting, not all wings....) .
 
Starting form a uniform field, the problem seems related to a Phi divergence that is not null in those cells, increasing or decreasing the total T (passive scalar) in those cells.

The non 0 divergence, may cause of course other issues not yet discovered...
Steps To Reproduceusing tutorial example mixerVesselAMI2D, add passive scalar (e.g Temperature) as described for icoFoam in http://openfoamwiki.net/index.php/How_to_add_temperature_to_icoFoam , acting on mixerVesselAMI2D tutorial.
The same result can be obtained for any passive scalar.


Modify
transportProperties
my_icoFoam.C and createField.H
fvSchemes and fvSolution


In "0" directory, set the boundaryField for stator and rotor in new the T file with fixed uniform temperature, so that *no changes should occur* in temperature when mixer rotating
{
        type fixedValue;
        value uniform 100;
    }


Run the solver.
Open paraFoam, and discover that exist cluster of cells that shows higher themperature and cluster of cells that show lower temp. than 100°C.

See image.

TagsAMI

Activities

user525

2012-10-15 09:23

 

Schermata del 2012-10-15 09:59:26.png (118,105 bytes)   
Schermata del 2012-10-15 09:59:26.png (118,105 bytes)   

user525

2012-10-15 17:55

  ~0001730

The cells concerned with the problem, are the ones close/around to pRefCell.
Changing the pRefCell Value, makes the problem appear around that new pRefCell.

PIMPLE
{
....
    pRefCell 0;
    pRefValue 100;
}

user525

2012-10-15 18:05

  ~0001731

Commenting out the divergence operator in the passive scalar solver, makes error disappear.
Things seems to show that the problem is concerned with divergence error caused in the very first cell calculated.


        fvScalarMatrix TEqn
        (
            fvm::ddt(T)
            //+ fvm::div(phi, T) < commented out ============
            - fvm::laplacian(DT, T)
        );

        TEqn.solve();
        T.correctBoundaryConditions();

user525

2012-10-15 21:45

  ~0001732

More info...
Before passive scalar solver, dumped out divergence values;

It shows clearly the FIRST Cells have a very HUGE DIVERGENCE,
very different from the other cells

dump and code follow:
--------------------------------------------------
time step continuity errors : sum local = 8.08573e-09, global = -1.18856e-09, cumulative = -1.18467e-09
GAMG: Solving for p, Initial residual = 0.0747711, Final residual = 0.000343049, No Iterations 6
GAMG: Solving for p, Initial residual = 0.000336345, Final residual = 1.99852e-06, No Iterations 6
GAMG: Solving for p, Initial residual = 1.9989e-06, Final residual = 5.45285e-07, No Iterations 2
time step continuity errors : sum local = 3.22009e-09, global = -2.85251e-10, cumulative = -1.46992e-09
Divergence:

3072
(
-0.00377731 <============ here
6.81498e-05
-0.000131197 <============ here
1.04748e-05
-8.13186e-05
9.22288e-06
-2.76134e-05
.....
.....
----------------------------------------------------------------
                turbulence->correct();
            }
        }
Info << "Divergence:" << endl;
Info << scalarField(fvc::div(phi)) << endl;

        fvScalarMatrix TEqn
        (
            fvm::ddt(T)
            + fvm::div(phi, T)
            - fvm::laplacian(DT, T)
        );
--------------------------------------------------

user525

2012-10-16 21:30

  ~0001736

Tutorial case + passive scalar tested also on OF 2.1.x

But with the same result:
-----------------------------------------------------------------------
time step continuity errors : sum local = 8.08573e-09, global = -1.18856e-09, cumulative = -1.18467e-09
GAMG: Solving for p, Initial residual = 0.0747711, Final residual = 0.000343049, No Iterations 6
GAMG: Solving for p, Initial residual = 0.000336345, Final residual = 1.99852e-06, No Iterations 6
GAMG: Solving for p, Initial residual = 1.9989e-06, Final residual = 5.45285e-07, No Iterations 2
time step continuity errors : sum local = 3.22009e-09, global = -2.85251e-10, cumulative = -1.46992e-09
Divergence with OpenFoam 2.1.x:

3072
(
-0.00377731
6.81498e-05
-0.000131197
1.04748e-05
-8.13186e-05

user270

2012-11-20 13:48

  ~0001783

I was experiencing similar issues to the ones described here.
After reproducing mentioned test case, I run into similar results.
Running the test case on 64bit Ubuntu 10.04, OF-2.1.1

will

2022-05-18 11:08

manager   ~0012586

Numerical issues with AMI-based patch couplings have been resolved by the new Non-Conformal Coupled (NCC) development. See the following commit for explanation, and instructions for how to use NCC and convert cases from AMI.

https://github.com/OpenFOAM/OpenFOAM-dev/commit/569fa31d09f98e29d1aaf84d40bb16043f104ec6

Issue History

Date Modified Username Field Change
2012-10-15 09:23 user525 New Issue
2012-10-15 09:23 user525 File Added: Schermata del 2012-10-15 09:59:26.png
2012-10-15 17:55 user525 Note Added: 0001730
2012-10-15 18:05 user525 Note Added: 0001731
2012-10-15 21:45 user525 Note Added: 0001732
2012-10-16 21:30 user525 Note Added: 0001736
2012-11-20 13:48 user270 Note Added: 0001783
2014-12-29 18:42 wyldckat Tag Attached: AMI
2022-05-18 11:08 will Assigned To => will
2022-05-18 11:08 will Status new => resolved
2022-05-18 11:08 will Resolution open => fixed
2022-05-18 11:08 will Fixed in Version => dev
2022-05-18 11:08 will Note Added: 0012586