[ngj]

Hi Luther

The problem is not related to groovyBC but to /system/fvSolution, as stated in the error message. Try to copy e.g. the /system/fvSolution from /tutorials/interFoam/damBreak and see if it does not solve the problem, as it should be working with interFoam.

Best regards,

Niels

[luther]

Originally Posted by ngj

Hi Luther

The problem is not related to groovyBC but to /system/fvSolution, as stated in the error message. Try to copy e.g. the /system/fvSolution from /tutorials/interFoam/damBreak and see if it does not solve the problem, as it should be working with interFoam.

Best regards,

Niels

Hi Niels,

Yes I have changed the two preconditioners it was complaining about in the fvSolution file to preconditioner DIC. And then it worked. Would have to read up on what it entails.

Thank you for the post.

Regards
Luther

[luther]

Hallo Bernard (or anyone else that would be able to help),

First of all, thank you for the help. I have managed to get the groovyBC case working for simulating a wave in a 2D flume.

I have now been trying to apply it to a 3D case. I have made a mesh in gmsh and converted it using gmshToFoam. With the conversion I got a warning message saying it found a number of undefined faces in the mesh and are adding them to the default patch. However, when I look in the constant/polyMesh/boundary file it generated I find:

defaultFaces
{
type patch;
nFaces 0;
.....
}

Would that mean there is 0 default Faces?

If I choose to ignore it and set everything up pretty much the same as in the groovyWaveTank example I find that the simulation crashes near the start. The Courant numbers grow out of control. Here is the massage:

MULES: Solving for gamma
Liquid phase volume fraction = 0.4197596 Min(gamma) = -1.1716894e-19 Max(gamma) = 1.0015516
MULES: Solving for gamma
Liquid phase volume fraction = 0.41975964 Min(gamma) = -4.9807421e-20 Max(gamma) = 1.0000001
MULES: Solving for gamma
Liquid phase volume fraction = 0.41975967 Min(gamma) = -1.271157e-19 Max(gamma) = 1.097679
GAMG: Solving for pd, Initial residual = 0.89005896, Final residual = 0.029750488, No Iterations 3
GAMG: Solving for pd, Initial residual = 0.99557433, Final residual = 0.033653032, No Iterations 3
DICPCG: Solving for pd, Initial residual = 0.99572845, Final residual = 9.8705723e-08, No Iterations 324
time step continuity errors : sum local = 0.0010253293, global = -8.0769936e-07, cumulative = -8.0897217e-07
ExecutionTime = 63.5 s ClockTime = 64 s
Courant Number mean: 5588.1394 max: 64637244
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xb8034400]
#3 Foam::Time::adjustDeltaT() in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::Time::setDeltaT(double) in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 main in "/home/luther/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interFoam"
#6 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#7 Foam::regIOobject::readIfModified() in "/home/luther/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interFoam"
Floating point exception


Then when I have a look at the few results generated it seems like the initial gamma field is set everywere except at the inlet face, where the groovyBC is defined. I use setFields and interFoam. Am I doing something wrong? Anybody with some advice I will really appreciate it. I attach the case I am playing around with if you would like to have a look yourself.

Here is the case file:

http://dip.sun.ac.za/~luther/OF/poles.tar.gz


Kind regards
Luther

[ngj]

Hi Luther

Have you added the libGroovyBC (or what it is called), to the controlDict? If not, then it will not execute the Groovy with setFields, and thus the inlet boundary face will be empty.
Look at the wiki on how to add it.

Niels

[luther]

Originally Posted by ngj

Hi Luther

Have you added the libGroovyBC (or what it is called), to the controlDict? If not, then it will not execute the Groovy with setFields, and thus the inlet boundary face will be empty.
Look at the wiki on how to add it.

Niels

Hi Niels,

Thank you for your reply. I did remember to add the line " libs("libgroovyBC.so"); " to the bottom of controlDict.

Let me know if you think of anything else by any chance.

Kind Regards
Luther

[ngj]

Hi Luther

I have looked at your case file, and several things are off, non of which are related to groovyBC, however let us take it in this tread:

1. You are calculating the surface elevation around z=0 which is also the z-value on one of your boundary patches, even though your setFieldsDict suggest that you want to have the waves averaged around z=2.1.

2. I don't think the mesh resolution is anything near sufficient to resolve the physics you are interested in. Especially because you are having rather large tetrahedrals around the free surface. The scale of which are order of magnitude the wave amplitude.

3. You apply deep water theory, however you are in intermediate waters (0.1 < h/L = 0.4 < (pi or 2 * pi)), thus the applied theory is not correct.

These are the things I have noticed would cause you trouble, however I am almost certain that it is (1) which cause the blow-up.

Best regards,

Niels

[luther]

Originally Posted by ngj

Hi Luther

I have looked at your case file, and several things are off, non of which are related to groovyBC, however let us take it in this tread:

1. You are calculating the surface elevation around z=0 which is also the z-value on one of your boundary patches, even though your setFieldsDict suggest that you want to have the waves averaged around z=2.1.

2. I don't think the mesh resolution is anything near sufficient to resolve the physics you are interested in. Especially because you are having rather large tetrahedrals around the free surface. The scale of which are order of magnitude the wave amplitude.

3. You apply deep water theory, however you are in intermediate waters (0.1 < h/L = 0.4 < (pi or 2 * pi)), thus the applied theory is not correct.

These are the things I have noticed would cause you trouble, however I am almost certain that it is (1) which cause the blow-up.

Best regards,

Niels

Hi Niels,

Thanks.

Regarding (1): I will most certainly try it this evening. I have not been looking out for that and it makes sense that it could be the cause.

Regarding (2) and (3): I was not giving any attention to the wave theory or the mesh resolution itself at this stage. I was merely trying to see if I can apply the groovyBC from groovyWaveTank to a 3D case.

Thank you very much for the effort of looking into it. Hopefully it would not be too long before I can also make useful contributions to the forum.

Regards
Luther

[gautami]

Hello,

I tried to run the groovyBC movingConeDistorted case from the following link:

https://openfoam-extend.svn.sourcefo...roovyBC/Demos/

I did not make any changes to the case,and tried to run it as it is on OpenFOAM 1-5,suse linux 10.3.

But I end up getting this error.

Not Implemented
Trying to construct an genericFvPatchField on patch movingWall of field cellMotionUx#0 Foam::error:rintStack(Foam::Ostream&) in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::genericFvPatchField<double>::genericFvPatchF ield(Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&) in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so"

Can someone please help me.

Thankyou,
Gautami.

[gschaider]

Originally Posted by gautami

Hello,

I tried to run the groovyBC movingConeDistorted case from the following link:

https://openfoam-extend.svn.sourcefo...roovyBC/Demos/

I did not make any changes to the case,and tried to run it as it is on OpenFOAM 1-5,suse linux 10.3.

But I end up getting this error.

Not Implemented
Trying to construct an genericFvPatchField on patch movingWall of field cellMotionUx#0 Foam::error:rintStack(Foam::Ostream&) in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::genericFvPatchField<double>::genericFvPatchF ield(Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&) in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so"

The problem is that the library was not loaded (for whatever reason) and consequently the solver does not know about the boundary condition.

Check the output of the solver further up

Bernhard

[gautami]

Hello Mr Gschaider,

Thank you.
I could run the distortedmovingcone case without any error.
The problem was a small mistake at my end.(sorry)

Thankyou,
Gautami.

[David*]

Hello Foamers,
has somebody dealt with the groovyWaveTank demo? I wonder how the initial condition for gamma on the inlet patch is been set, as my setFields just writes the List<scalar> for the internalField. The result is, that I get a zero initial condition at the inlet. Does somebody know how to do this?
Thanks in advance,
David

[braennstroem]

Hi Bernhard,

I wonder, if your groovyBC is able to connect two boundary conditions!? E.g. is it possible to get the area averaged value of one patch to another one?

Would be great, if this works!

Fabian

[gschaider]

Originally Posted by braennstroem

I wonder, if your groovyBC is able to connect two boundary conditions!? E.g. is it possible to get the area averaged value of one patch to another one?

Currently not. Shouldn't be too hard (I thought about it once) but I'll have to have a look who to do it concretly

Bernhard

[chiven]

Hi, dear friends, I am trying to update the dambreak case of interPhaseChangeFoam for OF-1.5 to OF-1.6, and just meet the same problem like #40.
The alpha1 setting is

    alpha1
    {
        MULESImplicit
        {
        maxIter 1000;
        nLimiterIter 10;
        maxUnboundedness 1;
        CoCoeff 0.2;
        solver
        {
        solver          PBiCG;
        preconditioner   DILU;
        tolerance        1e-10;
        relTol           0;
        }
        }
    }

The case and the terminal prompt are attached. Any suggestions are appreciated.

Have a good day!
chiven

------------------------------------------------------------------------------------------------------------------------
Starting time loop
Courant Number mean: 0 max: 0
deltaT = 2.4e-05
Time = 2.4e-05

Attempt to return dictionary entry as a primitive
file: /work/g2/e090012/dambreak/system/fvSolution::solver from line 58 to line 60.
From function ITstream& primitiveEntry::stream() const
in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 83.
FOAM aborting
#0 _ZN4Foam5error10printStackERNS_7OstreamE-0x1466af0
in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so"
#1 _ZN4Foam7IOerror5abortEv-0x1989560
in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so"
#2 _ZNK4Foam15dictionaryEntry6streamEv-0x1921900
in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so"
#3 _ZNK4Foam10dictionary6lookupERKNS_4wordEbb-0x19476e0
in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so"
#4 void Foam::MULES::implicitSolve<Foam:neField, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam:neField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, double, double) in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxIA64GccDPOpt/interPhaseChangeFoam"
#5 main in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxIA64GccDPOpt/interPhaseChangeFoam"
#6 __libc_start_main-0x1060880
in "/lib/tls/libc.so.6.1"
#7 _start in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxIA64GccDPOpt/interPhaseChangeFoam"
Abort

[gschaider]

Originally Posted by chiven

Hi, dear friends, I am trying to update the dambreak case of interPhaseChangeFoam for OF-1.5 to OF-1.6, and just meet the same problem like #40.
The alpha1 setting is

I fail to get the significance of this for this thread. Especially if you look at #41 and #42 where a solution strategy for this was discussed

[chiven]

Originally Posted by gschaider

I fail to get the significance of this for this thread. Especially if you look at #41 and #42 where a solution strategy for this was discussed

hi, bernhard, thanks a lot for your reply.
I have tried what #41 and #42 said, but faild. These days I am struggling with this problem. And some other friends in this forums also meet the same problems. Any suggestiohs are precious for us.
Best regards,
Chiven

[gautami]

Hello,

I am trying to simulate a wave tank case in interDyMFoam.
I have set the inlet as groovyBC.
I want to set the expression for the inlet in pointMotionUx dictionary as follows:

if (time>1 and time<=2 expression-1) if (time>2 and time<3 expression-2) else zero.

I am trying to do it a follows,but I get an error.

valueExpression "toPoint((time()>1 && time()<=2) ? A*w*cos(w*time()) (time()>2 && time()<3) ? B*v*cos(w*time()) : 0 )";

How do I input such expression?
ThankYou.


Regards,
Gautami.

[braennstroem]

Hi Bernhard,

thanks for the info! Shouldn't be so hard sounds good ...

Fabian

[Arnoldinho]

Hi, did anybody successfully test and use the groovyBC with OpenFOAM 1.6?
From the errors I get, I guess that a few things have to be changed due to differences in calling of constants etc. between 1.5 and 1.6...

Arne

[gschaider]

Originally Posted by Arnoldinho

Hi, did anybody successfully test and use the groovyBC with OpenFOAM 1.6?
From the errors I get, I guess that a few things have to be changed due to differences in calling of constants etc. between 1.5 and 1.6...

The has been a separate versioon that compiles with 1.6 for some months, but obviously I never updated
http://openfoamwiki.net/index.php/Co...ovyBC#Download
(nevertheless, the 1.6 URL could have been easily guessed from the 1.5-URL)

Bernhard