CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Specifying nonuniform boundary condition (http://www.cfd-online.com/Forums/openfoam-solving/57782-specifying-nonuniform-boundary-condition.html)

maka September 14, 2005 11:22

What is the format of the file
 
What is the format of the file in which I can specify nonuniform boundary conditions? can any body give a sample?

Thanks,
Maka

chen_jun September 14, 2005 11:26

// Get index of patch lab
 
// Get index of patch
label inletPatchID = mesh.boundaryMesh().findPatchID("topMovingWall");

// Get reference to boundary value
const fvPatchVectorField& faceCentreshub = mesh.Cf().boundaryField()[inletPatchID];
fvPatchVectorField& movingWallU = U.boundaryField()[inletPatchID];

// loop over all hub faces
forAll(movingWallU, faceI)
{
// get coordinate for face centre
const vector& c = faceCentreshub[faceI];
vector p(0.5*(1+Foam::sin(40*M_PI*c[0]-M_PI/2)), 0, 0);
if (c[0]>0.025 &c[0]<0.075)
p = vector(1, 0, 0);

movingWallU[faceI] = p;
}

ami September 14, 2005 12:01

Hi Chen Jun I am interest
 
Hi Chen Jun

I am interested in considering nonuniform boundary conditions in my computations (e.g., a laminar Blasius boundary layer inflow condition along the free stream flow condition). Please can you specify the file name you described and how to use it?

thanks

hani September 15, 2005 03:07

This thread actually belongs i
 
This thread actually belongs in preprocessing. Anyway, Chen actually describes the basics of how to set your boundary conditions. It is however a bit difficult to understand for a beginner. Let me, as a slightly more than beginner try to help you in a more detailed way (there might be other solutions also):

It is unlikely that there is such a boundary condition already implemented and distributed in OpenFoam. You will have to implement it yourself. This goes at least for less common bc's.

A suggestion on how to implement the steady bc (reads 0 and overwrites 0):

Step 1:
Copy the source directory of the particular solver that you want to use to your personal applications directory. For instance:
mkdir ~/OpenFOAM/hani-1.2/applications (if you don't have it)
cp -r OpenFOAM/OpenFOAM-1.2/applications/solvers/incompressible/simpleFoam ~/OpenFOAM/hani-1.2/applications/

Step 2:
Rename your copied directory to something that makes sence, for instance:
mv ~/OpenFOAM/hani-1.2/applications/simpleFoam ~/OpenFOAM/hani-1.2/applications/blasiusBC
Rename the .C-file in your blasiusBC directory to blasiusBC.C
Edit blasiusBC.C: Insert correct descriptions for Application and Description in the header of the file, for clarity. Remove everything in the main function except the include statements in the beginning. You may later on check which ones you actually need by commenting them and try to compile. The compiler error messages will guide you.

Step 3:
Implement your bc's using the directives that Chen gave you. This should be located after the include statements in the main function.
Write out the variables you have changed at the end of the main function:
// Force the write
U.write();
k.write();
epsilon.write();
phi.write();

Info<< "\n ExecutionTime = "
<< runTime.elapsedCpuTime()
<< " s\n" << endl;

Info<< "End" << endl;

return(0);

Step 4:
Edit blasiusBC/Make/files to make sure that the filenames blasiusBC is used instead of the name of the original application.

Step 5:
Compile.
Move to your blasiusBC directory and type
wmake

Step 6:
type:
rehash
to make the executable available.

Step 7:
Set your bc's by typing:
blasiusBC <root> <case>
which will change the files in your <root>/<case>/0 directory to include the bc's you defined in blasiusBC.

Step 8:
Run your case using the solver you need for the application. It will read the 0 directory and get the correct bc's.

Good luck!
Håkan.

maka September 16, 2005 07:37

Thanks all. Many thanks Hakan
 
Thanks all. Many thanks Hakan for the detailed steps. It is very helpful.

Regards,
Maka

ami September 16, 2005 10:08

Thanks Hakan for the detailed
 
Thanks Hakan for the detailed explications.

hilaryspencer October 13, 2005 11:44

Francois I'll have a go at
 
Francois

I'll have a go at answering _some_ of your questions.

> Here are my questions:
>
> * is c[1] is the second component of the vector c on faceI ?

Yes! C and C++ arrays start at zero and (in OpenFOAM) go to size()-1

> * What are the differences between those two objects and two methods
> (C() and Cf()) of the mesh class:

In fvMesh.H it says:
//- Return cell centres as volVectorField
const volVectorField& C() const;

//- Return face centres as surfaceVectorField
const surfaceVectorField& Cf() const;

> * Finaly if I want to read an experimental profile of the x component
> of the velocity Ux=f(y) which is in a file and interpolate those
> values on the mesh to apply them on the x component of my inlet
> boundary velocity field. Is it easy or not ?

This may not be the easiest or most accurate solution -
you could create a 1d mesh with cell centres at the locations of your experimental profile. The Ux data could then be the experimental data

you could then create another case with a 1d mesh the same as your boundary of your (2d?) case
you could then use mapFields to interpolate from the first mesh to the second

then copy the interpolated data to the boundary condition of your 2d case (assuming the mesh is numbered in the same way for both - you'll have to make sure of this when you generate the 1d mesh)

> PS: more a C++ question, please don't laugh !!!
> Why is there sometimes an & (like after VectorField) and sometimes
> not (like scalarField)

Now this is a REALLY good question. One it took me AGES to understand
when there is an & after a name of a class it means that you are not creating a new one, you are just referring to one that all ready exists. It is therefore a reference

Example
int i = 0;
int& j = i; // j refers to i. No new data is created
j = 2; // actually sets i = 2 also

francois October 13, 2005 11:58

Tanks Hilary for your help wit
 
Tanks Hilary for your help with OpenFOAM and C++ !

I will study this problem carefully ... it's like an adventure for me ...

Have a nice day.
Francois

aurelia December 13, 2005 15:28

Hello! I'm trying to implemen
 
Hello!
I'm trying to implement non uniform bc at the inlet, following the step by step method of Håkan (thank you, by the way )
i compile with wmake, it seems to work
then the command rehash doesn't exist
and finaly, when i do step7, it doesn't change the values in the 0 directory
i suppose it's due to many mistake in c++
so i will be happy if one of you could take time to help me and check it

here is what i wrote in the main of the .c file, after all the include

/ Get index of patch
label inletPatchID = mesh.boundaryMesh().findPatchID("inlet");

// Get reference to boundary value
fvPatchVectorField& inletU = U.boundaryField()[inletPatchID];

// get coordinate for cell centre
const fvPatchVectorField& centre = mesh.C().boundaryField()[inletPatchID];
scalarField y = centre.component(vector::Y);
scalarField x = centre.component(vector::X);

// calculate inlet velocity
inletU = y*0.75/0.0051*vector (1,0,0)+x*0.75/0.0051*vector(0,1,0)+7.5*vector(0,0,1);

U.write();

Info<< "ExecutionTime = "
<< runTime.elapsedCpuTime()
<< " s\n\n" << endl;


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

return(0);
}


thanks
aurelia

hjasak December 14, 2005 05:22

In the statements: // calcu
 
In the statements:

// calculate inlet velocity
inletU = y*0.75/0.0051*vector (1,0,0)+x*0.75/0.0051*vector(0,1,0)+7.5*vector(0,0,1);

try doing

inletU == ...; (the rest is the same).

I suspect your boundary condition for this patch is fixedValue.

Hrv

unoder December 17, 2005 14:59

Can we get a tutorial out of t
 
Can we get a tutorial out of this? I'm also new to both Foam and C++ and interested in learning...

braennstroem January 4, 2006 10:52

Hi, I tried to implement th
 
Hi,

I tried to implement the version from aurelia. The compilation went fine, but applying the profile to an existing case in turbFoam I get:

...
Reading field U



--> FOAM FATAL IO ERROR : size 3 is not equal to the given value of 2438

file: turbFoam/smc/0/U::INLET from line 36 to line 42.

From function Field<type>::Field(const word& keyword, const dictionary& dict , const label s)
in file /home/fab/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude/Field.C at li ne 225.

FOAM exiting



I adjusted 'inletPatchID' to the existing 'INLET' in my case. Would be nice, if anybody has an idea!

Greetings!
Fabian

markc May 3, 2008 10:31

Some time ago already, however
 
Some time ago already, however I am experiencing the same problem. The error from Fabian is however caused by the fact that (probably) the 0/U file has non-uniform and three lines of vectors in it already, while the field is supposed to have 2438 faces and thus 2438 entries.
I think you have to include initContinuityErrs.H
However, even after this I am still not able to get things work. Changes are made to the internalFieldValues but not to boundary patches.

Any comments?
Once I succeed I will return with results.

Brgds,

Mark

markc May 3, 2008 13:18

Ok, I finally get it working.
 
Ok, I finally get it working. A small utility that is able to set nonuniform boundary conditions. For my case it is programmed to set gamma at 1 if Z coordinate is <0>0. However, users will be able to modify themselve.
The code is based on snippets found on this forum and very much resembles snippets in this thread. however 1 to 1 copying failed in my case. So here the full directory. hope it is useful for others.

attach{setBoundarygamma}

Brgds,

Mark

markc May 3, 2008 13:19

Lets try WITH attachment this
 
Lets try WITH attachment this time
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif setBoundarygamma.zip

rres October 11, 2008 08:45

Hi guys, I'm trying to crea
 
Hi guys,

I'm trying to create a custom bc as told here, but I'm stuck. I want to set the values of U, k and epsilon at the inlet, but when I try to compile, it throws the folowing errors:
Quote:


'k' was not declared in this scope
'epsilon' was not declared in this scope
'faceCentreshub' was not declared in this scope

I don't know what libraries are required. I've searched the manuals, internet, forums and nothing. For God's sake, someone help me! It's driving me crazy!!! http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Ravi

rres October 11, 2008 09:12

Hi, The kEpsilon.H has the
 
Hi,

The kEpsilon.H has the following declarations:

//- Return the turbulence kinetic energy
tmp<volscalarfield> k() const
//- Return the turbulence kinetic energy dissipation rate
tmp<volscalarfield> epsilon() const


But it seems that refers to cell volume values. I need the face values. Searching in the files (solvers) I found something like that: fvVectorMatrix divR = turbulence->divDevReff(U);
and I think that what I'm looking for is something like this.

Ravi

dmoroian October 14, 2008 01:58

Hi Ravi, If you'll attach the
 
Hi Ravi,
If you'll attach the sources to your post, maybe someone will have a look at it, otherwise we can at most speculate the source of your error.

Dragos

schoeller November 13, 2008 07:43

dear all, I have a simple g
 
dear all,

I have a simple geometry, which I model as a 2-phase liquid flow with interFoam solver. So far I have set boundary conditions manually using a text editor but it's just easier to have a function via command line at hand in order to do so.

Thus I followed the thread by on setBoundaryGamma and worked myself through it:

1. Using the instructions by Håkan Nilsson I copied the interFoam directory, renamed the files and applied my changes
2. Everything compiles with wmake
3. While executing setBoundaryGamma <patchname> from the project directory I receive the following error:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/home/schoeller/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/schoeller/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xb809b400]
#3 std::basic_string<char,>, std::allocator<char> >::basic_string(std::string const&) in "/home/schoeller/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libstdc++.so. 6"
#4 main in "/home/schoeller/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/setBoundar yGamma"
#5 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#6 _start in "/home/schoeller/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/setBoundar yGamma"
Segmentation fault

Does anybody have an idea why this could be?

* interFoam as a solver works fine with the case
* 'which gcc' tells me that it is using the compiler version from ThirdParty directory

The source code I used is as follows:

\*---------------------------------------------------------------------------*/
#include "fvCFD.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main(int argc, char *argv[])
{
argList::validArgs.append("patchName");
# include "setRootCase.H"
word patchName(args.args()[3]);
# include "createTime.H"
# include "createMesh.H"
# include "createFields.H"
# include "initContinuityErrs.H"

Info<< "This utility initializes gamma values for boundary patches based on" <<endl;
Info<<>=0 ==>gamma=0, z<o>gamma=1." <<endl;
Info<< "These settings are presently only changeable by modifying the source code." <<endl;
Info<< "Source code to be found in: OF/user/applications." <<endl;
Info<< "Change code (.C file) according your needs and in that directory run wmake." <<endl;
Info<< "\nStarting time loop\n" << endl;

// Get index of patch
label inletPatchID = mesh.boundaryMesh().findPatchID(patchName);
// Get reference to boundary value
//const fvPatchVectorField& centre = mesh.C().boundaryField()[inletPatchID];
const fvPatchVectorField& faceCentreshub = mesh.C().boundaryField()[inletPatchID];
//const fvPatchVectorField& faceCentreshub = mesh.Cf().boundaryField()[inletPatchID];
//Uncomment the line for your case: U for velocity cases, gamma for gamma cases
//fvPatchVectorField& Inlet = U.boundaryField()[inletPatchID];
fvPatchScalarField& targetPatch = gamma.boundaryField()[inletPatchID];
// loop over all hub faces
forAll(targetPatch, faceI)
{
// get coordinate for face centre
//const vector& c = centre[faceI];
const vector& c = faceCentreshub[faceI];
//vector p(0.5*(1+Foam::sin(40*M_PI*c[0]-M_PI/2)), 0, 0);
// c[0] is X coordinate, c[1] is Y coordinate, c[2] is Z coordinate
// Apply boundary condition based in one coordinate (X, Y, or Z).
if (c[1] < 0.3)
//if true: below watersurface
// loop over all hub faces
forAll(targetPatch, faceI)
{
// get coordinate for face centre
//const vector& c = centre[faceI];
const vector& c = faceCentreshub[faceI];
//vector p(0.5*(1+Foam::sin(40*M_PI*c[0]-M_PI/2)), 0, 0);
// c[0] is X coordinate, c[1] is Y coordinate, c[2] is Z coordinate
// Apply boundary condition based in one coordinate (X, Y, or Z).
if (c[1] < 0.3)
//if true: below watersurface
{
targetPatch[faceI] = scalar (1);
//Inlet[faceI] = vector (1, 0, 0);
}
//if false: at or above watersurface
else
{
targetPatch[faceI] = scalar (0);
//Inlet[faceI] = vector (10 ,0 ,0);
}
}
// Force the write
gamma.write();
//U.write();

Info<< "\n ExecutionTime = "
<< runTime.elapsedCpuTime()
<< " s\n" << endl;
Info<< "End" << endl;

return(0);
}
\*---------------------------------------------------------------------------*/

I would be very happy for any input.

Best wishes

Sebastian

markc November 14, 2008 13:54

Hi Sebastian, I have the ex
 
Hi Sebastian,

I have the experience that similar error messages can be due to very stupid small writing errors, either in filenames or e.g. patch names, or files being in the wrong place. Maybe it's something like this... Though it can be something completly else as well.

Brgds,

Mark


All times are GMT -4. The time now is 06:09.