CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

Neumann boundary conditions

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   August 11, 2010, 09:35
Default Neumann boundary conditions
  #1
Member
 
Join Date: Aug 2010
Posts: 31
Rep Power: 7
Martin80 is on a distinguished road
Hi,

I want to change my boundary conditions during runtime. For the Dirichlet conditions I have found a way to set up the conditions in the code:

I have choosen fixedValue for the boundary type and I updated it in the code using:
U.boundaryField()[patchI]== mynewScalarField;

I have tried the same with fixedGradient type for a Neumann Condition but it doesn't update the gradient value. (I have reviewed it with .snGrad()).

Maybe someone can give me a useful hint,
thanks, m.
Martin80 is offline   Reply With Quote

Old   August 16, 2010, 07:47
Default
  #2
Senior Member
 
Stefan Herbert
Join Date: Dec 2009
Location: Darmstadt, Germany
Posts: 129
Rep Power: 8
herbert is on a distinguished road
Hi Martin,

you have to do a refCast. Example:
Code:
fixedGradientFvPatchVectorField& gradUPatch=refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchI]);
scalarField& gradUField =  gradUPatch.gradient();
After this you can edit gradient values in gradUField.

Of course you have to include "fixedGradientFvPatchFields.H" in your header.

Regards,
Stefan
herbert is offline   Reply With Quote

Old   August 16, 2010, 08:33
Default
  #3
New Member
 
Join Date: Mar 2010
Posts: 27
Rep Power: 7
astein is on a distinguished road
Hi!
snGrad() has nothing to do with the gradient which you want to impose with your boundary condition, it is some geoemetrical quantity.

The fvPatchField is a field of quantities, which are applied as fixed gradients. Therefore, you have to write the wanted values to the field the same way you do it for the fixedValue stuff.

I hope you get the point...
Cheers, Andreas.
astein is offline   Reply With Quote

Old   August 16, 2010, 13:53
Default
  #4
Member
 
Join Date: Aug 2010
Posts: 31
Rep Power: 7
Martin80 is on a distinguished road
Hi Stefan,
I have already got the same answer from somebody else but thank you very much - this is exactly what I was seeking for. [.gradient() is not a member function of "volVectorField" but of "fixedGradientFvPatchVectorField"].

Hi Andreas,
I don't think u r right, U.boundaryField()[patchI].snGrad() in that case should show me the current boundary condition of the fixedGradient bc object.

B.r.,
Martin.
Martin80 is offline   Reply With Quote

Old   August 16, 2010, 13:59
Default
  #5
New Member
 
Nadeem
Join Date: Mar 2009
Location: München, Bavarian, Deutschland
Posts: 24
Rep Power: 8
ubaid is on a distinguished road
HAve u guys got the solution how to update the value of gradient, I think my problem is also similar to yours.

that is expressed below:

volScalarfield field
(
IOobject(fieldName,runtTime.timeName(),mesh,IOobje ct::NO_READ,IOobject::AUTO_WRITE),
mesh,
dimensionedScalar(fieldName,dimTemperature, 200),
"fixedGradient"
);
forAll(field.BoundaryField(),patchID)
{
field.boundaryField()[patchID]==30;
}

As an output of this code am getting something different.
that is.

boundaryField
{
Inlet
{
type fixedGradient;
gradient uniform 0;
}

and so on;
}

but I am interested to get output as below:

boundaryField
{
inlet
{
type fixedGradient;
gradient uniform 30;

}
}
ubaid is offline   Reply With Quote

Old   August 17, 2010, 03:03
Default
  #6
New Member
 
Join Date: Mar 2010
Posts: 27
Rep Power: 7
astein is on a distinguished road
Martin,
at the end, its the same.

What herbert is proposing is to copy (with the refCast) the reference of the fvPatchField to a new vectorField and editing THAT. Because of the reference, that still modifies the original field.

But you could write to your fixedGradientFvPatchVectorField directly, without giving it a new name. Just try it :-)

And - snGrad is definitely returning some geometrical stuff from the mesh, take a look at doxygen.

As long as it works there is no need to worry...
Have fun,
Andreas.
astein is offline   Reply With Quote

Old   August 17, 2010, 07:31
Default
  #7
New Member
 
Nadeem
Join Date: Mar 2009
Location: München, Bavarian, Deutschland
Posts: 24
Rep Power: 8
ubaid is on a distinguished road
Quote:
Originally Posted by astein View Post
Martin,
at the end, its the same.

What herbert is proposing is to copy (with the refCast) the reference of the fvPatchField to a new vectorField and editing THAT. Because of the reference, that still modifies the original field.

But you could write to your fixedGradientFvPatchVectorField directly, without giving it a new name. Just try it :-)

And - snGrad is definitely returning some geometrical stuff from the mesh, take a look at doxygen.

As long as it works there is no need to worry...
Have fun,
Andreas.


Thanks, surely it works, I read this thread little bit late thoroughly and atlast i did it.
ubaid is offline   Reply With Quote

Old   September 6, 2010, 05:37
Default Help Neumann boundary condition in fluent
  #8
cfm
New Member
 
Join Date: Sep 2010
Posts: 1
Rep Power: 0
cfm is on a distinguished road
Hi!!
I need to define an output Neumann boundary condition using fluent. the condition is dc/dn=0, where c is the concentration of a certain species and n is the normal versor to the output face.
How can I do this? Thanks!
cfm is offline   Reply With Quote

Old   October 14, 2010, 09:28
Default
  #9
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 230
Rep Power: 9
Cyp is on a distinguished road
Quote:
Originally Posted by herbert View Post
Hi Martin,

you have to do a refCast. Example:
Code:
fixedGradientFvPatchVectorField& gradUPatch=refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchI]);
scalarField& gradUField =  gradUPatch.gradient();
After this you can edit gradient values in gradUField.

Of course you have to include "fixedGradientFvPatchFields.H" in your header.

Regards,
Stefan

Hi Stefan and everybody,

I trying to implement neumann BC with your method but I had a fail during the compilation. I have merely copy your piece of code in my main.C file and I included "fixedGradientFvPatchFields.H" in my header.

I get the following error :

Code:
applications/twoDarcyF> wmake
Making dependency list for source file twoDarcyF.C
SOURCE=twoDarcyF.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-40 -I/gemp/csoulain/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude -IlnInclude -I. -I/gemp/csoulain/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude -I/gemp/csoulain/OpenFOAM/OpenFOAM-1.7.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/twoDarcyF.o
twoDarcyF.C: In function int main(int, char**):
twoDarcyF.C:74: error: invalid initialization of reference of type Foam::scalarField& from expression of type Foam::Field<Foam::Vector<double> >
make: *** [Make/linux64GccDPOpt/twoDarcyF.o] Erreur 1

Do you have any idea where I am wrong ?

Regards,
Cyp
Cyp is offline   Reply With Quote

Old   October 14, 2010, 09:44
Default
  #10
Member
 
Join Date: Aug 2010
Posts: 31
Rep Power: 7
Martin80 is on a distinguished road
It should be:


vectorField& gradUField = gradUPatch.gradient();

(in case U is a volVectorField)

M.
Martin80 is offline   Reply With Quote

Old   October 14, 2010, 10:26
Default
  #11
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 230
Rep Power: 9
Cyp is on a distinguished road
Ok. Thank you very much. It compiles now.


But in case U is a volScalarField (a pressure field for example)? The code of Hebert should works, shouldn't it ?
Cyp is offline   Reply With Quote

Old   October 14, 2010, 10:51
Default
  #12
Member
 
Join Date: Aug 2010
Posts: 31
Rep Power: 7
Martin80 is on a distinguished road
No, i think in that case (for a volScalarField) you have to modify the first expression of Stefan's code in an appropriate way.
M.
Martin80 is offline   Reply With Quote

Old   October 14, 2010, 12:33
Default
  #13
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 230
Rep Power: 9
Cyp is on a distinguished road
I have a problem of understanding: the gradient of a scalar should be a vector. So the following snippet should work:

Code:
label patchID = mesh.boundaryMesh().findPatchID("inlet"); 

fixedGradientFvPatchVectorField& gradUPatch=refCast<fixedGradientFvPatchVectorField>(p.boundaryField()[patchID]);
scalarField& gradUField =  gradUPatch.gradient();

gradUField = -(inv(M)&U)+rho*g;
where M is a tensor, U the velocity field (vector), rho a volScalarField, and g the vector acceleration.

In fact, it compiles but fails while running:

Code:
Time = 0.1


--> FOAM FATAL ERROR: 
Attempt to cast type fixedValue to type fixedGradient

    From function refCast<To>(From&)
    in file /opt/openfoam171/src/OpenFOAM/lnInclude/typeInfo.H at line 114.

FOAM aborting
I can't see my mistake..
Cyp is offline   Reply With Quote

Old   October 14, 2010, 12:49
Default
  #14
Member
 
Join Date: Aug 2010
Posts: 31
Rep Power: 7
Martin80 is on a distinguished road
You define the outer normal gradient (grad p * n) [n is the surface outer normal direction]

let p be a scalarF and V a vectorF then:

grad(p) is a vectorF -> (grad(p)) *n is a scalarF
grad(V) is a tensorF -> (grad(V)) *n is a vectorF

I hope it helps, M.
Martin80 is offline   Reply With Quote

Old   October 14, 2010, 13:14
Default
  #15
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 230
Rep Power: 9
Cyp is on a distinguished road
Thank you very much Martin. It helps me much in the understanding !

So I changed the code as :

Code:
label patchID = mesh.boundaryMesh().findPatchID("inlet");  
fixedGradientFvPatchScalarField& gradUPatch=refCast<fixedGradientFvPatchScalarField>(p.boundaryField()[patchID]); 
scalarField& gradUField =  gradUPatch.gradient();
Now, according to your definition, if I understand correctly, I need to get the projection of my field -(inv(M)&U)+rho*g on the patch : (-(inv(M)&U)+rho*g ) *n. Is it possible to do such a thing ?
Cyp is offline   Reply With Quote

Old   October 14, 2010, 13:41
Default
  #16
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 230
Rep Power: 9
Cyp is on a distinguished road
I think it could work with :

Code:
gradUField = linearInterpolate(-(inv(M)&U)+rho*g) & mesh.Sf();
Cyp is offline   Reply With Quote

Old   October 14, 2010, 14:14
Default
  #17
Member
 
Join Date: Aug 2010
Posts: 31
Rep Power: 7
Martin80 is on a distinguished road
The normal surface vector field on the boundarypart patchID is:
vectorField n = mesh.Sf().boundaryField()[patchID]


Take care that the left part of your calculation is finally also a vectorField on the appropriate domain (boundaryField()[patchID]).
M.
Martin80 is offline   Reply With Quote

Old   October 18, 2010, 11:53
Default
  #18
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 230
Rep Power: 9
Cyp is on a distinguished road
Hi Martin!

Thank you very much for your answer. I am not sure to understand very well...

I tried:

Code:
label patchID = mesh.boundaryMesh().findPatchID("inlet");
fixedGradientFvPatchScalarField& gradUPatch=refCast<fixedGradientFvPatchScalarField>(p.boundaryField()[patchID]);
scalarField& gradUField =  gradUPatch.gradient();

vectorField n = mesh.Sf().boundaryField()[patchID];
and either
Code:
gradUField = (-(inv(M)&U)+rho*g)&n
or
Code:
gradUField = (-(inv(M)&U)+rho*g)*n
or
Code:
gradUField = linearInterpolate(-(inv(M)&U)+rho*g)&n
but it does not compile... Do you see my mistake ??

Last edited by Cyp; October 18, 2010 at 12:46.
Cyp is offline   Reply With Quote

Old   October 25, 2010, 10:28
Default
  #19
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 230
Rep Power: 9
Cyp is on a distinguished road
Hi!


I succed in the compilation using this piece of code :

Code:
        label patchID = mesh.boundaryMesh().findPatchID("inlet");

        fixedGradientFvPatchScalarField& gradUPatch=refCast<fixedGradientFvPatchScalarField>(p.boundaryField()[patchID]);
        scalarField& gradUField = gradUPatch.gradient();
        
        vectorField n = mesh.Sf().boundaryField()[patchID];

        vectorField UU_beta = U_beta.boundaryField()[patchID];

        tensorField MM_beta = M_beta.boundaryField()[patchID];

        tensorField invMM_beta=inv(MM_beta);

        gradUField = -((invMM_beta&UU_beta)&n)+(rho_beta.boundaryField()[patchID]*(g.value())&n);

I set up a fixedValue at the inlet for my U_beta field but when I plot the results, the U_beta value is different that the one I chose...

Did I miss something ??

Regards,
Cyp
Cyp is offline   Reply With Quote

Old   October 26, 2010, 05:00
Default
  #20
Senior Member
 
Stefan Herbert
Join Date: Dec 2009
Location: Darmstadt, Germany
Posts: 129
Rep Power: 8
herbert is on a distinguished road
Please realize that you are editing the BC for p with your code
Quote:
Originally Posted by Cyp View Post
Code:
        fixedGradientFvPatchScalarField& gradUPatch=refCast<fixedGradientFvPatchScalarField>(p.boundaryField()[patchID]);
If you want to edit BC for U, you have to change it in the following way
Code:
       fixedGradientFvPatchScalarField& gradUPatch=refCast<fixedGradientFvPatchScalarField>(U.boundaryField()[patchID]);
Regards,
Stefan
herbert is offline   Reply With Quote

Reply

Tags
boundary conditions, fixedgradient, neumann

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Impinging Jet Boundary Conditions Anindya Main CFD Forum 24 January 11, 2012 14:40
mesh file for flow over a circular cylinder Ardalan Main CFD Forum 6 April 17, 2010 23:40
Concentric tube heat exchanger (Air-Water) Young CFX 5 October 6, 2008 23:17
Pressure boundary conditions Lionel S. Main CFD Forum 1 August 24, 2007 18:03
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 01:24.