[Sherlock_1812]

Hi Philip,

I have been trying to re-write valueFraction for each face of my patch as symm(n*n). I have a very basic doubt.
Is it better to write a new BC (derived from directionMixed (maybe?)) where this definition of valueFraction is changed as symm(n*n) while looping over all faces of the patch? If yes, where do I make the changes? In the 'updateCoeffs' section?

Thanks.

[Sliwa]

Hi,

Originally Posted by hjasak

4) If this is not enough for you (there is another possibility), I have written a newDirectionMixedFvPatchField boundary condition, with 4 components. Unlike the above one, this b.c. allows both the normal and tangential condition to be mixed separately between the fixedValue and fixedGradient b.c. with two blending factors. You need this kind of thing for contact problems with friction and large deformation and similar. In my version, the stuff lives in:
OpenFOAM-1.2/applications/solvers/newStressAnalysis/materialModels/newDirectionM ixed

In my problem, I would like to specify on one of my boundaries:

- a zero gradient for the normal component of the displacement
- a zero displacement in the tangential direction

The newDirectionMixed looked like the perfect solution. However, when I ran it with my solver, I got the following error:

--> FOAM FATAL IO ERROR: 

    Cannot find 'value' entry on patch symr of field U in file "/home/salwa/OpenFOAM/salwa-extend-3.0/run/tutorials/solidMechanics/elasticThermalSolidFoam/flosse_test1/0/U"
    which is required to set the values of the generic patch field.
    (Actual type newDirectionMixed)

    Please add the 'value' entry to the write function of the user-defined boundary-condition
    or link the boundary-condition into libfoamUtil.so

file: /home/salwa/OpenFOAM/salwa-extend-3.0/run/tutorials/solidMechanics/elasticThermalSolidFoam/flosse_test1/0/U::boundaryField::symr from line 64 to line 69.

    From function genericFvPatchField<Type>::genericFvPatchField(const fvPatch&, const Field<Type>&, const dictionary&)
    in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 71.

FOAM exiting

Adding a 'value' entry gave this error:

gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type newDirectionMixed)
    on patch symr of field U in file "/home/salwa/OpenFOAM/salwa-extend-3.0/run/tutorials/solidMechanics/elasticThermalSolidFoam/flosse_test1/0/U"
    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 811.

FOAM exiting

This is my U file:

symr
    {

        type                                newDirectionMixed;
        refValue                           uniform    0;
        refGrad                            uniform    0;
        nHat                               (1 0 0);
        normalValueFraction            0;
        tangentialValueFraction       1;
        value                               uniform (0 0 0);
  }

Does anyone know where the problem might come from? Is there something wrong with my U file?

Thanks,

[bigphil]

Hi Sliwa,

In my problem, I would like to specify on one of my boundaries:
- a zero gradient for the normal component of the displacement
- a zero displacement in the tangential direction

directionMixed can do this: the capabilities of newDirectionMixed have essentially been included in the current directionMixed boundary condition, as valueFraction is a symmTensor now instead of a scalar.

To achieve what you want, use directionMixed like this:

myPatch
{
    type              directionMixed;
    refValue          uniform ( 0 0 0 );
    refGradient       uniform ( 0 0 0 );
    valueFraction     uniform ( 0 0 0 1 0 1 ); // (I - sqr(n))
    value             uniform ( 0 0 0 );

where I have assumed n = ( 1 0 0 ) above.
You can see that to fix the value in the normal direction valueFraction = sqr(n), whereas to fix the value in the tangential directions valueFraction = I - sqr(n).

Best regards,
Philip

[bigphil]

Originally Posted by Sherlock_1812

Hi Philip,

I have been trying to re-write valueFraction for each face of my patch as symm(n*n). I have a very basic doubt.
Is it better to write a new BC (derived from directionMixed (maybe?)) where this definition of valueFraction is changed as symm(n*n) while looping over all faces of the patch? If yes, where do I make the changes? In the 'updateCoeffs' section?

Thanks.

Hi Srivaths,

yes you should derive a new boundary condition from directionMixed and set the valueFraction in the constructor or, if the mesh is moving/changing, in updateCoeffs.

See for example, fixedDisplacementZeroShear in $FOAM_SRC/solidModels.fvPatchVectorFields in foam extend.

Best regards,
Philip

[Sliwa]

Thank you, Philip! That worked.

[infinity]

Hi Dear Foamers

I'm trying to use no-stress wall boundary condition

and I used:

        type            directionMixed;
        refValue        uniform (0 0 0);
        refGradient     uniform (0 0 0);
        valueFraction   uniform (0 0 0 1 0 0);

and now I'm getting wrong answers

I would appreciate if anyone could help me

[infinity]

any answer guys ?

[bigphil]

I think the slip boundary condition already does what you want.

See here.

Philip

[infinity]

Thanks a lot Philip
It was very Helpful

[STutexas]

Originally Posted by bigphil

Hi Nicolas,

Yes it is possible, using directionMixed, to give every face on a boundary patch a different gradient in the tangential direction. I would do something like this in a header file at the start of a time-step (although it might be possible to use groovyBC but I am not sure):

label patchID = mesh.boundaryMesh().findPatchID("patchOfInterest");
if(patchID == -1)
 {
    Info << "patch not found" << endl;
    return 0;
 }

directionMixedFvPatchVectorField& Upatch =
        refCast<directionMixedFvPatchVectorField>
        (
         U.boundaryField()[patchID]
         );

//- patch face normals      
vectorField n = mesh.boundary()[loadingIndex].nf();
      
//- set value fraction so as to have fixed value in patch normal direction
Upatch.valueFraction() = symm(n*n);

//- set fixed value
Upatch.refValue() = vector (0, 0, 0); //- put what ever vectorField you want here

//- set fixed gradient (as a function of position and time as an example)
const vectorField& patchFaceCentres = mesh.boundaryMesh()[patchID].faceCentre();
Upatch.refGradient() = patchFaceCentres * runTime.value();

By the way, "U" is my solution variable above.

Hope this helps,
Philip

Hi Philip
Interesting explanation for the changing the refGradient in the directionMixed BC. If we include this code in the data can we give any values in directionMixed condition in the 0/U file? Is it possible to set a nonuniform value for the valuefraction in a similar manner using tensor fields.

Thank you.

Saurabh

[STutexas]

Hi Philip

Just another doubt. Can we use funkySetFields with directionMixed BC. I am getting an error when I try to do that. This is the error:

--> FOAM FATAL IO ERROR:
"ill defined primitiveEntry starting at keyword 'valueFraction' on line 29 and ending at line 41"

Thank you.

[nlc]

Yes Saurabh you can do this,

If you want to this you want to define a summetric tensor field as a variable initialize it corectly with all the constructors and add it to the maping function if you want to be able to use it in parallèle.

You can always look at boundary condition source code to give you great exemple, ther is plenty of them.

But valueFraction is alrethy a symmTensorField !?? I'm not shure what is your objectif in creating your new dirrectionMixed boundary condition.

I dont konw about funkysetfield I did not use it yet.

Out of curiosity why do you want to do this ? What are you tring to accomplish ?

Not shur what you mean by including the code in the data ?

Hope this was usfull

[STutexas]

[QUOTE=ubald;576267]Yes Saurabh you can do this,

If you want to this you want to define a summetric tensor field as a variable initialize it corectly with all the constructors and add it to the maping function if you want to be able to use it in parallèle.

You can always look at boundary condition source code to give you great exemple, ther is plenty of them.

But valueFraction is alrethy a symmTensorField !?? I'm not shure what is your objectif in creating your new dirrectionMixed boundary condition.

I dont konw about funkysetfield I did not use it yet.

Out of curiosity why do you want to do this ? What are you tring to accomplish ?

Not shur what you mean by including the code in the data ?

Hi Nicolas

Thank you for replying so quickly. I will take a look the deifnition of the codes and see if I can compile my own BC. I am trying to use openFoam for magnetic decay simulations and my BC doesnot have a symm tensor in value fraction. Please peruse my post:

http://www.cfd-online.com/Forums/ope...groovy-bc.html

This might give you more context to what I am trying to do. Thanks again for the help.

[praveensrikanth91]

Hello,

I am trying to use the conjugate heat transfer solver to compute phase change at a liquid-vapor interface. I have implemented the phase change models into the solver with just a normal velocity at the interface for the phase change. However, I have vapor flow over the interface which would create a viscous shear on the surface of the liquid. The boundary condition for the problem is essentially equal tangential velocities on either side of the interface and equal tangential shear stresses. Added to this is the fixed value in the normal direction. I was thinking that this would be possible to be implemented using the directionMixed boundary condition. However I am not sure how the value fraction would look for such a scenario.

Is it possible to use directionMixed for such a BC? I am hoping someone with some experience would be able to direct me in the right direction. As far as I know there does not seem to be any similar boundary conditions in OF.

Thanks so much for your time

Praveen

[behzad-cfd]

Hi,

I don't know i'm in right thread or not by the way I want to solve equation and obtain B that is defined like .
I've implemented the equation in my base solver. Now i want to test functionality of the new solver but i have some boundary condition problem before testing.
For example if i want to get in boundaries i need to set and .

Can i use directionMixed BC for this?
How can i implement this BCs?

Thanks in advance,
Behzad

[nlc]

Hi Behzad,

OpenFOAM is 3D by défaut 1D and 2D case are achieve by setting special BC. The equations you share seem to be 2D. You need first to specify your equations in 3D then figure ought what type of BC you need. Fixed, gradient, mixed !! Then you'll know what to look for.

It seems to me that you should start a new thread. Wright the hole set of equations for your problem with detail on the boundary condition you want to use. Or a link in an article relevant to your case.

It is better to use vector notation then component details as OF use vector and tensor notation. Add me on your new tread please as it seems interesting.

NLC

[behzad-cfd]

Originally Posted by nlc

Hi Behzad,

OpenFOAM je 3D n'y défaut 1D and 2D case are achieve by setting special BC. The equation you share seem to be 2D. You need first to specify your equation on 3D then figure ought what type of BC you need. Fixed, gradient, mixed !! Then you'll know what to look for.

It seems to me that you should start a new thread. Wright the hole set of equations for your problem with detail on the boundary condition you want to use. Or a link in an article relevant to your case.

It is better to use vector notation then component details as OF use vector and tensor notation. Add me on your new tread please as it seems interesting.

NLC

Hi Nicolas,

Thanks for kind reply. as you mentioned OF operates in 3D my case is 2D and I'll set front and back plane as empty and that's not the problem. I showed component details for clarifying the variable relations and boundary conditions. any way I'll open new thread and add you there.

Kind regards,
Behzad

[behzad-cfd]

Originally Posted by behzad-cfd

Hi Nicolas,

Thanks for kind reply. as you mentioned OF operates in 3D my case is 2D and I'll set front and back plane as empty and that's not the problem. I showed component details for clarifying the variable relations and boundary conditions. any way I'll open new thread and add you there.

Kind regards,
Behzad

Hi Nicolas,

This is the link of new thread.
https://www.cfd-online.com/Forums/op...tml#post671506

[neilk]

Hello,

I have a doubt regarding mixed boundary condition. The available mixedFvPatchField I have to specify fixed Value and a normal gradient. I want to apply a mixed BC to a wall to simulate mass diffusion across it. Thus boundary condition to vary along the wall for varying mass fraction gradients and mass fraction values in cells neighboring the wall. Is there a boundary condition that provides this facility? I have attached the boundary condition equation below where Cmucus is the mass concentration which undergoes convection-diffusion and the coefficients of Cmucus are constants.

Capture.PNG

Thank you

[Pavithra]

Hello Everyone

I am unable to understand the mixed boundary condition clearly.

I have a vertical wall and I want to set the x-component of velocity to be u = 0 and y-component of velocity to be set as dv/dx = 0.

In order to achieve this, I have implemented the following

sideWall
{
type directionMixed;
refValue uniform (0 0 0);
refGradient uniform (0 0 0);
valueFraction uniform (0 0 0 0 0 1);
}

but, when I plot I see non-zero values for the x-component.

Kindly, please help me.

With Thanks & Regards,
Pavithra.