[Jiricbeng]

Hi,

I have of 2.3.0 and I installed 1.6ext version. However although I use command of16ext to switch openfoam version I cant make run cases which run under openfoam 2.3.0, such as simpleFoam.. Where is the mistake?

[alexeym]

Hi,

what exactly did you mean by

I cant make run cases

?

There can be lots of things: slightly different dictionary formats, wrong environment variables, etc.

[Jiricbeng]

I mean - I have a simple case I created - a box with velocity inlet and pressure outlet (k - eps model) which worked fine in of 2.3.0. And when I write command to switch from 2.3.0. to 1.6ext and write "simpleFoam" to start calculation, it writes

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM Extend Project: Open source CFD |
| \\ / O peration | Version: 1.6-ext |
| \\ / A nd | Web: www.extend-project.de |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6-ext-064a6e9f332e
Exec : simpleFoam
Date : May 15 2014
Time : 11:33:24
Host : 96GB
PID : 6070
Case : /home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading field p



--> FOAM FATAL IO ERROR:
Cannot open include file "/home/openfoam/OpenFOAM/OpenFOAM-1.6-ext/etc/caseDicts/setConstraintTypes" while reading dictionary "/home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/0/p::boundaryField"

file: /home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/0/p at line 24.

From function functionEntries::includeEntry::includeEntry(dictio nary& parentDict,Istream& is)
in file db/dictionary/functionEntries/includeEntry/includeEntry.C at line 105.

FOAM exiting

....
Have got any idea, what is wrong?

[alexeym]

Can you show your 0/p file? I guess the problem is in the line

#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"

There's no such file in 1.6-ext. As I don't know detail of your case, for the start I'd suggest you to comment out the line.

[Jiricbeng]

I uploaded the case here http://leteckaposta.cz/843824944. You can have a look at the files. I will be really glad for help.

[alexeym]

Well, you need to remove (or comment out) line:

#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"

in 0/U and 0/p files. As in fact you don't need this line even if you're running the case with 2.3.0.

[Jiricbeng]

Thank you,

however I still have the message:

--> FOAM FATAL IO ERROR:
keyword div((nuEff*dev(grad(U).T()))) is undefined in dictionary "/home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/system/fvSchemes::divSchemes"

file: /home/openfoam/JiriV-2.3.0/run/tutorials/incompressible/pokusy/schodek/Merge_schodek/schodek_good_mesh_k-eps/system/fvSchemes::divSchemes

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 396.

FOAM exiting

Although I commented out the div((nuEff*dev(grad(U).T()))) in /fvSchemes (I also tried to comment out other lines in fvSchemes) it still writes the message above (I tried to close and open terminal as well)

[alexeym]

Well, you can't solve everything by just commenting it out

If you go to 1.6 tutorials, you'll find, this line

div((nuEff*dev(T(grad(U))))) Gauss linear;

should be

div((nuEff*dev(grad(U).T()))) Gauss linear;

The reason for it is the implementation of turbulence->divDevReff(U) method. If you look at UEqn.H:

    tmp<fvVectorMatrix> UEqn
    (
        fvm::div(phi, U)
      + turbulence->divDevReff(U)
    );

and then look at kEpsilon.C, in 2.3 divDevReff is:

tmp<fvVectorMatrix> kEpsilon::divDevReff(volVectorField& U) const
{
    return
    (
      - fvm::laplacian(nuEff(), U)
      - fvc::div(nuEff()*dev(T(fvc::grad(U))))
    );
}

while in 1.6 it is

tmp<fvVectorMatrix> kEpsilon::divDevReff(volVectorField& U) const
{
    return
    (
      - fvm::laplacian(nuEff(), U)
      - fvc::div(nuEff()*dev(fvc::grad(U)().T()))
    );
}

That's why you need different lines in your fvSchemes for different versions of OpenFOAM.

[Jiricbeng]

that is true, commenting out is a dull kind of solutin.

Thank you very much indeed mate, I finally used the whole files fvSchemes and controlDict from the 1.6ext tutorial, cause there were other fvSchemes errors.

Anyway, I would like to ask crucial question that I yearn to sort out, that is how could I run MRFSimpleFoam tutorial? There is folder "Make" and files createFields.H and MRFSimpleFoam.C, I do not know how to make it run. Could you give me a clue ?

[alexeym]

If you're talking about tutorials/incompressible/MRFSimpleFoam/mixerVessel2D from 1.6 then there is Allrun script. In the folder tutorials/incompressible/MRFSimpleFoam/MRFSimpleFoam solver itself is located, it's not a case folder.

[Jiricbeng]

Yes, I thought it is two separate folders ( mixerVessel2D and MRFSimpleFoam) I am just working with it (due to Allrun in mixerVessel2D).
Thanks a lot

[Jiricbeng]

I am just going through the mixeVessel2D files. I obviously do not understand, what is actually the logic of MRFSimpleFoam - in this case I cannot see any mixing plane and there is no segment rotating, it is full circle.

I assumed in polymesh/boundary there will be a definition of cyclicGGI or GGI.. but there are just walls for rotor and stator.

Where can I find a case with rotating segmend connected via mixing plane to another segment or to a draft tube?

[Jiricbeng]

Hello,
I uploaded my rotor stator case I wish to simulate by using 1.6ext.

http://leteckaposta.cz/897752382

I d be very happy if you had little time to have a look at the case.

[wyldckat]

Greetings to all!

@Jiri:

Originally Posted by Jiricbeng

Where can I find a case with rotating segmend connected via mixing plane to another segment or to a draft tube?

I was planning on answering here on this thread, but after looking into this topic, I found out that 1.6-ext has the mixing plane feature in another branch and not in the standard one. And that it's preferable to install foam-extend 3.0, as it already has this feature integrated.
For more information, please read my revised post #7 on this thread: http://www.cfd-online.com/Forums/ope...tml#post492711

For future reference, looking for tutorials that have this mixing-plane feature, at least for now, can be done with this command:

find $FOAM_TUTORIALS -iname "*mixingPlane*"

Of course that this requires that you've installed a version of source code that has this feature

Best regards,
Bruno

[Jiricbeng]

Thank you much for your information, I am just struggling with installation of extend -3.0. I am stuck on the step 11 which should last max 30 minutes, I waited nearly two hours and nothing.

[Jiricbeng]

Hi,
I successfully installed extended version 3.0.
I have meshes of stator.msh and rotor.msh which were created in commercial software. In OF 2.3.0 I used fluent3DMeshToFoam to convert meshes .msh to OF format. Then I used mergeMeshes and meshes were merged together.

However, I want to use mixing plane between rotor and stator, using OF3.0. I cant find where to set revolution of the rotor as I cant find it neither in tutorial mixingPlaneAxial nor in mixingPlaneDomADomB.

Moreover when typing simpleFoam a receive the error message:

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Initializing the mixingPlane interpolator between master/shadow patches: outflow/wall-4


--> FOAM FATAL ERROR:
Face zone name outflowZone for mixingPlane patch outflow not found. Please check mixingPlane interface definition.

From function label mixingPlanePolyPatch::zoneIndex() const
in file meshes/polyMesh/polyPatches/constraint/mixingPlane/mixingPlanePolyPatch.C at line 724.

Cause in polymesh/sets I have only folders:
highAspectRatioCells
nonOrthoFaces
region0
region1
wrongOrientedFaces

How shall I get there files with zones, as in tutorial mixingPlaneAxial