[linch]

Originally Posted by gschaider

A dimensionedScalar defined in the program? No. There are some ways around (the IOreferencer described below is one of them). But to say which is the best it would be helpful if you described the problem you want to solve

I use a moving reference frame. It is sufficient to describe the reference frame velocity with a single vector, this velocity is needed for BCs. That's it, actually.

Best regards,
Illya

[akidess]

Done

Originally Posted by gschaider

I wasn't aware of this. That's why it was not represented in the grammar.

That would be a simple fix to the grammar.

You don't have to ask to file a bug report. If I don't like them I will turn them down Yes. Please

[gschaider]

Originally Posted by linch

I use a moving reference frame. It is sufficient to describe the reference frame velocity with a single vector, this velocity is needed for BCs. That's it, actually.

It was discussed elsewhere: it is not possible to access a variable in the solver code if it is not registered with the mesh.

The possibilities with swak are (I assume that the reference frame velocity is specified in a file):
- use a global variable that is used in all boundary conditions. That wy you have to specify the velocity twice (and consistent): once in the original file, the other time in the controlDict with a global-variable functionObject
- with the pythonIntegration (or the swakCoded if you prefer C++) functionObject: the FO reads the value from the file and injects it into the global namespace

Note: with option 1 you have a possibility to keep it consistent: add a dictionary file with an entry

referenceVelocity (1 1 42);

include that using the include directive into both files where the vel is used and write $referenceVelocity instead of the velocity.

[Mohamad(AUT)]

Hi bernhard
thank you for your works i appreciate you for these
if you notice that the sourcefourge svn for downloading groovy bc lib is down can you mail it for me?
thank you for your help...

Best Regards Mohamad

[ngj]

Hi Mohamad,

The SVN is still down and has been for a while. Temporary download instructions can be found here:

http://openfoamwiki.net/index.php/Co...am#Downloading

Note that swak4Foam combines groovyBC and funkySetField functionalities, and I believe that the individual devlopment of these two tools have come to a stop along with the introduction of swak4Foam.

Kind regards

Niels

[Sherlock_1812]

Hi all,

I would like to have a gradient BC for velocity at the boundary that is calculated from updated values of the temperature field. Is this possible using groovyBC?

Thanks in advance,

[gschaider]

Originally Posted by Sherlock_1812

Hi all,

I would like to have a gradient BC for velocity at the boundary that is calculated from updated values of the temperature field. Is this possible using groovyBC?

Thanks in advance,

Yes, it is. Use gradientExpression and set fractionExpression to "0"

[Sherlock_1812]

Hi Bernhard,

Thank you for the reply.

So if I have to write gradient(U) = (1/mu)*(dSigma/dT)*gradient(T) where T is the temperature on the particular patch, it has to be like

surface
{
type groovyBC;
variables "mu= ... ;dSigma/dT= ...;";
fractionExpression "0";
gradientExpression "(1/mu)*(dSigma/dT)*T"; ---> how to make sure T is temperature of the patch 'surface' here?
}

[gschaider]

Originally Posted by Sherlock_1812

Hi Bernhard,

Thank you for the reply.

So if I have to write gradient(U) = (1/mu)*(dSigma/dT)*gradient(T) where T is the temperature on the particular patch, it has to be like

surface
{
type groovyBC;
variables "mu= ... ;dSigma/dT= ...;";
fractionExpression "0";
gradientExpression "(1/mu)*(dSigma/dT)*T"; ---> how to make sure T is temperature of the patch 'surface' here?
}

T IS the current temperature on the patch. Everything else would be a bit complicated (and make groovyBC unusable). If you want things to be more complicated internalField(T) gives you the values on the cells next to the patch (sometimes, especially when dealing with gradients this value can help)

Some remarks:
- use the list-syntax for the variables. It makes things more readable
- if your U is a vector then the gradientExpression must be a vector too (it is the gradient of the field in the direction of the face normal).

[Sherlock_1812]

Originally Posted by gschaider

T IS the current temperature on the patch. Everything else would be a bit complicated (and make groovyBC unusable). If you want things to be more complicated internalField(T) gives you the values on the cells next to the patch (sometimes, especially when dealing with gradients this value can help)

Some remarks:
- use the list-syntax for the variables. It makes things more readable
- if your U is a vector then the gradientExpression must be a vector too (it is the gradient of the field in the direction of the face normal).

Thank you for the reply and your remarks Bernhard. This will be of help.

[haze_1986]

Hi, I am not sure why groovyBC does not work with my 1.6ext installation but works with 2.1.1. I am currently using the multiple installation iso from here. http://www.tfd.chalmers.se/~hani/kur...fromUSBiso.htm

Works fine for 2.1.1 but in 1.6ext

--> FOAM Warning : 
    From function dlLibraryTable::open(const fileName& functionLibName)
    in file db/dlLibraryTable/dlLibraryTable.C at line 86
    could not load libgroovyBC.so: cannot open shared object file: No such file or directory
Create mesh for time = 0


Reading gravitationalProperties
Reading field h

Reading field h0 if present

Reading field U

Creating field hU



--> FOAM FATAL ERROR: 
Not Implemented
    Trying to construct an genericFvPatchField on patch inlet of field hU

    From function genericFvPatchField<Type>::genericFvPatchField(const fvPatch& p, const DimensionedField<Type, volMesh>& iF)
    in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 45.

FOAM aborting

[gschaider]

Originally Posted by haze_1986

Hi, I am not sure why groovyBC does not work with my 1.6ext installation but works with 2.1.1. I am currently using the multiple installation iso from here. http://www.tfd.chalmers.se/~hani/kur...fromUSBiso.htm

Works fine for 2.1.1 but in 1.6ext

--> FOAM Warning : 
    From function dlLibraryTable::open(const fileName& functionLibName)
    in file db/dlLibraryTable/dlLibraryTable.C at line 86
    could not load libgroovyBC.so: cannot open shared object file: No such file or directory
Create mesh for time = 0


Reading gravitationalProperties
Reading field h

Reading field h0 if present

Reading field U

Creating field hU



--> FOAM FATAL ERROR: 
Not Implemented
    Trying to construct an genericFvPatchField on patch inlet of field hU

    From function genericFvPatchField<Type>::genericFvPatchField(const fvPatch& p, const DimensionedField<Type, volMesh>& iF)
    in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 45.

FOAM aborting

For technical reasons every OF-installation has to have its own installation of swak/groovyBC. Seems that this 1.6-ext has none. From what I see in the link the ISO is from last years workshop. I was not involved in the creation of that ISO so I can't vouch that there was a swak for 1.6-ext on it.

I guess you'll have to get the sources from the latest release and compile them

[haze_1986]

Originally Posted by gschaider

For technical reasons every OF-installation has to have its own installation of swak/groovyBC. Seems that this 1.6-ext has none. From what I see in the link the ISO is from last years workshop. I was not involved in the creation of that ISO so I can't vouch that there was a swak for 1.6-ext on it.

I guess you'll have to get the sources from the latest release and compile them

I intend to get the tarball from
http://openfoamwiki.net/images/e/e6/...e_0.2.3.tar.gz

and wmake all from the OF1.6ext terminal.

Would that be a sensible procedure?

[gschaider]

Originally Posted by haze_1986

I intend to get the tarball from
http://openfoamwiki.net/images/e/e6/...e_0.2.3.tar.gz

and wmake all from the OF1.6ext terminal.

Would that be a sensible procedure?

Yep. 0.2.3 is not the latest version but more up-to-date than what is on the stick anyway.

There is a problem with 1.6-dev that there are two slightly different version around. If you experience problems during compilation (something about symmTensors in the Parsers) go to Libraries/swak4FoamParsers/include/swak.H and comment (or uncomment) the line with #define FOAM_SYMMTENSOR_WORKAROUND

[haze_1986]

Originally Posted by gschaider

Yep. 0.2.3 is not the latest version but more up-to-date than what is on the stick anyway.

There is a problem with 1.6-dev that there are two slightly different version around. If you experience problems during compilation (something about symmTensors in the Parsers) go to Libraries/swak4FoamParsers/include/swak.H and comment (or uncomment) the line with #define FOAM_SYMMTENSOR_WORKAROUND

Works very well, thank you very much.

[Tushar@cfd]

Dear Bernhard,

I wish to apply inlet boundary for the tensor using groovy BC. Suppose, the boundary is "mu*(du/dy)" along xx-direction (i.e., Txx). How would I progress?

Thanks in Advance

[gschaider]

Originally Posted by Tushar@cfd

Dear Bernhard,

I wish to apply inlet boundary for the tensor using groovy BC. Suppose, the boundary is "mu*(du/dy)" along xx-direction (i.e., Txx). How would I progress?

Thanks in Advance

One way is to build the tensor from components with a function "tensor(Txx,...)" (there are of course 9 components.
Also all the operators (inner/outer product etc) described in table 1.2 of the OF Programmers Guide are supported

For details see:
http://sourceforge.net/p/openfoam-ex...amReference.md

[Tushar@cfd]

Thank you for the info.

I will try to figure out..

[zandi]

Originally Posted by RitaFC

Sorry because I forget to report that the problem is solved.
I thank you for the answer.
In fact the file was already with "bash". But with a lot of patience and installations and verifing the text files in "swakconfiguration" and "the Files" the problem is solved and swak4Foam is working pretty well.
Thanks for that also.

Note: However the messages 9 not found and so on still appeared.

Hi RitaFC,
would you please tell me how do you fix it?
I need it really!
Thank you

[zandi]

Originally Posted by RitaFC

Hi

No 'swakConfiguration'. Python etc won't work
Checking swak4Foam-version and generating file
./Allwmake: line 32: wmake: command not found

I meant this error
I have the same problem