Hi,

Looking for a way to implement non uniform BC, I found part of the answer here, thanks!

Now, I'm looking for something more specific: I want to implement an inletOutlet condition. With the help provided here, I managed to modify the value argument of my BC. Now I want to modify also the inletValue argument, but I don't know how to write it.

Does anyone can help me? Thank you for your help!

Julien

Hi Julien

There is already implemented an inletOutlet boundary condition. See the User-/Programming-guides.
For the use of these look into "/tutorials/interFoam/damBreak/0".

Best regards,

Niels

Thank you for answering Niels,

but sorry, I wanted to say non uniform inletOutlet boundary condition.
I already used inletOutlet conditions, but only with uniform values at inletValue. I would like to know the syntax to modify the inletValue argument instead of the value one.

Best Regards
Julien

So what you need is to be able to read a list of values in stead of on single value?
If that is the case, I would look into

A_("A", coeffDict_, N_)

where A_ in this case is a scalarField, "A" the name of the valuelist in the dictionary seen by coeffDict_ and N_ is the number of elements. The above is used in a constructor. See also the last constructor in the Doxygen-files:

http://foam.sourceforge.net/doc/Doxy...b6d65dfbddd227

Good luck,

Niels

P.S. I would start with the single-value inletOutlet and modify it where needed.

Hi,
I come back to this topic because I'm using what was explained in the first page, and I want to go further for an industrial use (so I have to create applications that would make my work faster after...)

I want to change the type of boundaryfield with an application, so I'm looking for syntax to do it.
For the moment, after the line

fvPatchScalarField& targetPatch = gamma.boundaryField()[inletPatchID];

when I write

targetPatch.type();

I get

type generic;

and targetPatch is

type fixedValue;
value uniform 0;


and I don't find the way to change type fixedValue.
I want to change from fixedValue to inletOutlet for example, and then implement the arguments of my type (here inletValue and Value). I looked around the declarations of fvPatchField, boundaryField... but I'm a beginner in C++ and didn't find what I wanted.

Can anyone help me please?

Best regards,

Julien

Hi Ravi,

I hope you did not go crazy on the prob :-P , waiting for the answer over one year...but here we go...

I had the exact same problem and I think i came up with an answer.
Since I could not find anything regarding an answer to "our" prob here a post:


the creatfields.h file needs to contain an entry for every variable you want to use (otherwise he complains obout unknown things)

so you need to do:

Info << "Reading field VARIABLE\n" << endl;
vol-insertTYPE-Field VARIABLE
(
IOobject
(
"VARIABLE",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);


regards

Hey There,

I have been trying to create my own nonuniform profile for different variables.

I ran into a prob (suprise, surprise...).

I used the executable that is made once you type "wmake" to change the first boundary patch successfully.
then I was going to add a second patch, which did not work out.
I tried different things and figured that I can only assign the first patch defined in Blockmesh (right ??).

i came up with this theory since I have this code:
....
volVectorField::GeometricBoundaryField& Upatches = U.boundaryField();
volScalarField::GeometricBoundaryField& kpatches = k.boundaryField();
volScalarField::GeometricBoundaryField& epsilonpatches = epsilon.boundaryField();

forAll(Upatches, patchI)
{
if
(
(typeid(Upatches[patchI]) == typeid(fixedValueFvPatchVectorField))
&&
(mesh.boundaryMesh()[patchI].name() == "inlet-air" || "sidewall" ||
"inlet-gas" || "sackgesicht!" )
)
{
fixedValueFvPatchVectorField& Upatch =
refCast<fixedValueFvPatchVectorField>(Upatches[patchI]);

fixedValueFvPatchScalarField& kpatch =
refCast<fixedValueFvPatchScalarField>(kpatches[patchI]);

fixedValueFvPatchScalarField& epsilonpatch =
refCast<fixedValueFvPatchScalarField>(epsilonpatch es[patchI]);

const vectorField& faceCentres =
mesh.Cf().boundaryField()[patchI];


forAll(faceCentres, facei)
{

{
Upatch[facei] = vector (0,0,56789);
kpatch[facei] = 666;
epsilonpatch[facei] = 666;
}


}
};

Info<< "Writing nonsence\n" << endl;
U.write();
k.write();
epsilon.write();

Info<< "End\n" << endl;

return 0;


}

}

and he writes only new entrys for the first patch defined by blockmesh.
I changed patch-orders in Blockmesh.
When I changed first and second patch he assigned values to the new first patch.
When I tried having the patch originally assigned third on first place, i ended up with error messages->:confused: .

so what the bleeep is going on and how can I assigne non-uniform values to several patches at once??
-----------
One veery noobish question:
I was forced to copy the executable, which is created by typing wmake, to the case-folder and execute it using ./filename..
Since rehash seems not to work on suse 11.
How can I rehash easy, so that I can use it like the other tools (such as setHotRoom, or paraFoam) just by typing its name??
-----------



thx&regards

That was not what you wanted to write. You wanted something like
Maybe there are other problems, but this was the most obvious one

Bernhard

Hi Bernhard,

thanks for your answer!

But I am afraid it has to be something else...

when I do:

volVectorField::GeometricBoundaryField& Upatches = U.boundaryField();
volScalarField::GeometricBoundaryField& kpatches = k.boundaryField();
volScalarField::GeometricBoundaryField& epsilonpatches = epsilon.boundaryField();

forAll(Upatches, patchI)
{
if
(
(typeid(Upatches[patchI]) == typeid(fixedValueFvPatchVectorField))
&&
(mesh.boundaryMesh()[patchI].name() == "inlet-air" )
)

{
fixedValueFvPatchVectorField& Upatch =
refCast<fixedValueFvPatchVectorField>(Upatches[patchI]);

fixedValueFvPatchScalarField& kpatch =
refCast<fixedValueFvPatchScalarField>(kpatches[patchI]);

fixedValueFvPatchScalarField& epsilonpatch =
refCast<fixedValueFvPatchScalarField>(epsilonpatch es[patchI]);

const vectorField& faceCentres =
mesh.Cf().boundaryField()[patchI];

forAll(faceCentres, facei)
{

{
Upatch[facei] = vector (0,0,777);
kpatch[facei] = 666;
epsilonpatch[facei] = 666;
}




}
};
Info<< "Writing nonsence\n" << endl;
U.write();
k.write();
epsilon.write();
Info<< "End\n" << endl;
return 0;
}

It only writes new values when I change the patch-entry in blockmesh to first position, otherwise it seems not to be doing anything ...

any further Ideas?

regards!

p.s. can anyone also give me a hint how to quickly rehash on suse 11. ?

nonuniform internal Field
 

Hi All,

if I want to have a nonuniform InternalField and I would like to have a similar code like postet above for the inlet...what do I have to change?
Can anyone give me a hint?

I have been trying stuff like this, but it does not work...

fvPatchField::internalField& Upatches = U.internalField();
GeometricField::internalField& Upatches = U.internalField();

I have also been trying to find a hint how to do it in the doxygen-"documentation"...but without success...has anyone a hint how to takle the problem, when I have a file setting the boundary (like postet before) and I want to rewrite it to set a nonuniform INternalfield ??

Thx&Regards !

The best strategy is usually "which utility does something like this and can inspire me". Have a look at the code of the engineSwirl-utility (found in $FOAM_UTILITIES/preprocessing). Basically a cell value for U can be accessed via U[cellI].

Bernhard

Hi Bernhard,

thx for your answer..
It is kind of inspiring, but I am lacking the knowledge to do anything with this inspiration...

For example:

I have the lines:

const vectorField& faceCentres =
mesh.Cf().boundaryField()[patchI];

and

scalar test = cellCentres.y() /R;

For the boundary-profile.
I suppose the first line assigns the position-information to the variable "face centers".
The secont line uses part of this info.

Since i want to fit it to my cause (the internal-field) i have been trying things like this:

const vectorField& position =
mesh.Cf().internalField()[cellI];

scalar test = position.y() /R;

which obviously causes the compiler (and i guess also you) to do: :rolleyes: !

I could not find a axample in files (like funkysetfields, setfields...) which i was able to transfer.

So I started looking in the doxygen-files..I think they are hiding the answer somewhere...

So my question:

----------How do I start looking for the answer (in this case of bottom to top engineering) ??



I have been trying to find the syntax in the classes that regard my prob.. For example in :

src » finiteVolume » fields » fvPatchFields » fvPatchField

But the source code contains no information about finding a position in the field.

Or I have been staring at:
Foam::globalMeshData

I can see with which variables the classes exchange data...but i cant find a solution for my prob(or any service of the class i can call and which classes i have to include for him to work)..


I know that this is quite a "large" question, but I think the only way to really "learn" how to deal with Openfoam is to understand how I get information about the structure (otherwise i keep on guessing ).

regards&thx ( again) !

Yes. Have a look at Table 2.1 in the Programmer's guide for the meaning of Cf(). What you'll also find is the method C() for cell centers which you'll propably need for non-uniform internal fields

Hi Bernhard,

thx a lot, was quite usefull..

have a nice weekend!

regards

nonuniform internalField, Volumeprofile, profile, Volume
 

Hi Folks,

since I was not able to find something like this and I just finished it (and it is working :D ) here a post for the archive:
(This file is writing a non uniform internal-field for k, epsilon, velocity)

#include "fvCFD.H"
#include "OSspecific.H"
#include "fixedValueFvPatchFields.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{

# include "setRootCase.H"

# include "createTime.H"
# include "createMesh.H"
# include "createFields.H"


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

volVectorField::InternalField& Upatches = U.internalField();
volScalarField::InternalField& kpatches = k.internalField();
volScalarField::InternalField& epspatches = epsilon.internalField();


forAll(Upatches, cellI)
{
scalar R = 0.0026;
//for 3d geometries only!?
/*scalar rR = sqr(faceCentres[facei].y *faceCentres[facei].y() +
faceCentres[facei].x() *faceCentres[facei].x() )/R; */

scalar test = mesh.Cf().internalField()[cellI].y() /R;


if
(
(test > 0) &&
(test < 1.00)
)

{
scalar MEAN_vel1 = 53;
scalar FACT1 = 0.03;


scalar VEL1 = MEAN_vel1 * (1.1758 + 0.27651 * test - 4.034 * pow(test,2) +
21.211*pow(test,3) - 50.888 * pow(test,4) + 57.595 * pow(test,5) - 25.343 * pow(test,6));

scalar k_1 = (3*VEL1*VEL1*FACT1*FACT1)/2;
scalar sucker_1 = VEL1*VEL1*VEL1;
scalar eps_1 = ( (Foam::sqrt(sucker_1>0 ? sucker_1 : -sucker_1) ) / (0.1 * 2*
0.0026));



Upatches[cellI] = vector (0,0,VEL1);
kpatches[cellI] =k_1 ;
epspatches[cellI]= eps_1;

}


if
(
(test > 1.00) &&
(test < 5)

)
{
scalar MEAN_vel2 = 9.2;
scalar FACT2 = -0.60736 + 1.2393 * test - 0.82277 * pow(test,2) + 0.2596 * pow(test,3) - 0.042878 * pow(test,4) + 0.0035864 *pow(test,5) -
0.00012003 * pow(test,6);
scalar VEL2 = MEAN_vel2 * ( -8.5665 + 19.253 * test - 16.531 *pow(test,2)
+ 7.6006* pow(test,3) - 2.0045 * pow(test,4) + 0.30352 * pow(test,5) - 0.024522 * pow(test,6) + 0.00081898 * pow(test,7) ) ;


scalar k_2 = (3*FACT2*FACT2*VEL2*VEL2)/2);

scalar eps_2 = ( (Foam::sqrt(VEL2*VEL2*VEL2) ) / (0.1 * 2* 0.0026));


Upatches[cellI] = vector (0,0,VEL2);
kpatches[cellI] = k_2;
epspatches[cellI]= eps_2;
}



if
(
(test > 5) &&
(test < 6.5)

)
{
scalar MEAN_vel3 = 9.2;
scalar FACT3 = -2.2207 + 1.4684 * test - 0.3617 * pow(test,2) + 0.039378 * pow(test,3) - 0.0016 * pow(test,4);
scalar VEL3 = MEAN_vel3 * 1 ;
scalar k_3 = (3*( pow(FACT3, 2) * pow(VEL3,2) )/2;

scalar eps_3 = ((Foam::sqrt(pow(VEL3,3))) / (0.1 * 2* R));


Upatches[cellI] = vector (0,0, VEL3);
kpatches[cellI] = k_3;
epspatches[cellI]= eps_3;
}


if
(
(test > 6.5)
)
{
scalar MEAN_vel4 = 9.2;
scalar FACT4 = 0.001;
scalar VEL4 = MEAN_vel4 * 1 ;
scalar k_4 = (3 * (pow(FACT4, 2) * pow(VEL4,2))/2;
scalar eps_4 = ((Foam::sqrt(pow(VEL4,3))) / (0.1 * 2* R));

Upatches[cellI] = vector (0,0, VEL4);
kpatches[cellI] = k_4;
epspatches[cellI]= eps_4;
}
}
Info<< "Writing stuff\n" << endl;
U.write();
k.write();
epsilon.write();

Info<< "End\n" << endl;

return 0;
}


regards!

nonuniform profile with library
 

Hi There,

i have managed to make an executable (by using wmake) that patches the folder "0" with the desired non-uniform Values (see postings before if interested) ...

So I tried to do the same using the library I can create out of my BC-files by using "wmake libso"..

So I do:
"wmake libso" and he says : "'libNULL.so' is up to date."

I added the library entry to controldict
( like shown here: http://openfoamwiki.net/index.php/Si...ry_/_Tutorials )
libs ("setProfiles_oneInlet.so");I also added an entry to the k or U or epsilon file in 0 :
Like for using groovyBC...

inlet
{
type setProfiles_oneInlet;
value uniform 0.000138;
}



when i start the calculation he says:

gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type setProfiles_oneInlet)
on patch inlet of field k in file "/home/itvns/OpenFOAM/OpenFOAM-1.6/!!_OWN/sandia_nonpremixed_turb_jetflame/V5_profiles_byLIB/0/k"
You are probably trying to solve for a field with a generic boundary condition.

From function genericFvPatchField<Type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 782.


so what did I miss, how do I use the boundary-conditionst this way (or is it not possible??)

thx in advance!

regards!

Hi All,

i thougth I managed to create a profile for the BC and the internal-field..unfortunatelly I failed for reasons I dont understand.

The Profiles (for U, epsilon, k, CH4 and O2) should be independent of Z-direction, BUT they are NOT !

I attached pictures of CH4 over y (for different heights (Z)).
And also a graph for the z-velocity over y (for different heights (Z)).
Those were made for time 0 after patching the profile.
CH4 is the easyest example of the profile i am trying to use.
It should be 1 for 0<y<0.0026& 0<z<2 and 0 elsewhere.

(I am also assigning values to U,eps, k, CH4, O2, thats why i dont use setFields)


:confused: So 2 PRROBS :confused: :

1. why is the distribution depending on z, eventhough it should not be?
2. The patched file "0/CH4" has the values 0 and 1 ONLY (i checked on that ;)
), the values I get out of "sample-utility" and the picture from
paraFoam show values unequal to 0 or 1 ...similar things happen to U_z(see picture "vel_distribution.."):confused: ???

So why is the distribution depending on z and why does he alter my (peak) values ???

thx in advance&regards!!

More Info:
I have an INLET along the y-axes(CH4 entering for y< 0.0026, O2 for y>0.0026), x-Direction is"empty" since i am doing 2d..Direction of flow is along z-axis.

The Complete code for patching the BC and internal field is attached, parts of it can be seen further down...
(here i deleted eveything not necessary for CH4, to keep it simple)


sampleDict:

HI Folks,

i updated the last post to make the prob clearer..

regards& a nice weekend!!

OK. Now I get it. You're mixing cells with faces. What you'll want is
But your code gives the more interesting (not completely random) patterns

Thank you so much, again!! :o