[bigphil]

Nicolas,

I am not too familiar with writing a boundary condition but I think you can call the mother constructor to set gradients etc (see $FOAM_SOLVERS/newStressAnalysis/materialModels/fvPatchFields/tractionDisplacement/tractionDisplacementFvPatchVectorField.C in OpenFOAM-1.6-ext which is derived from fixedGradient).

Philip

[nlc]

Great example Tanks

[AlmostSurelyRob]

I would like to implement Newton's law of cooling. This is a type of Robin boundary condition, which is specified by

\frac{\partial T}{\partial n} = -(h A/k) (T_w - T_{ref})

where h, A, k are problem constants, n is the normal to the boundary and T is the temperature. The subscript w, means wall temperature and ref is the reference ambient temperature.

I would be happy to implement and test this, but I would need to understand the code a little bit more. Can mixed boundary condition simulate that kind of behaviour?

Essentially I would like to have a basic BC that allows to specify a b and g as described here:
http://en.wikipedia.org/wiki/Robin_boundary_condition

I would be obliged for any hints.

[AlmostSurelyRob]

Right... I think I've answered my questions now, although as a "home-grown" user and programmer of OF I will always appreciate any help and comments.

After analysis of the code in fixedGradient, fixedValue and mixed, I came to a conclusion that for my BC I need to express the functions snGrad and evaluate. One way to do it, is

1. express the T_w in snGrad as T_p + \frac{\partial T}{\partial n} and do a bit of juggling with terms.
2. express T_w in evaluate as T_p + approximation of gradient from neighbouring cells.

T_p is the internal value.


Is there anything else I should keep in mind? I don't quite understand what's the purpose of XCoeffs functions. Do I need to make alterations there as well?

Is it off-topic? Should I post in developers forum?

[makaveli_lcf]

Hi Robert,

an explanation how to use modified mixed BC for your equation see
the post http://www.cfd-online.com/Forums/ope...tml#post295694

[AlmostSurelyRob]

Thank you very much for the reply. Yes, I was actually thinking of expressing the equations in terms of the blending coefficient, but for some reason I thought it will not be possible. Clearly, I was wrong.

Incidentally, I've written my version of robinBC which evaluates the face value in exactly the same way. It calculates the gradient in a similar manner. It is a 1st order approximation. However, I have not touched XCoeff functions as I am still not sure what they do and my robinBC is not tested. The only positive is that it doesn't diverge when I run it with my case.

Now I could test it against this setting of mixed BC.

Many thanks.

[makaveli_lcf]

The XCoeff (nice name:-)) functions update your diagonal elements of the linear system which you solve after all based on the BC type. And it uses either your value representation at the boundary for let's say convectional terms or gradient treatment for your diffusion terms.

[AlmostSurelyRob]

Thanks again. The main advantage of my implementation, if it proves to work, should be an easier definition of the transfer coefficient. The mixed BC "hack" requires to specify delta which is the first cell centroid wall distance. I would like to get rid of that!

[moun139]

how about mixed boundary condition in FLUENT code ,please ?

thank you

[ziemowitzima]

Dear Bigphil

I tried your method to customize directionMixed BC but I could not compile my code.
I got following errors:

error: ‘directionMixedFvPatchVectorField’ was not declared in this scope
error: ‘loadingIndex’ was not declared in this scope
error: ‘const class Foam:olyPatch’ has no member named ‘faceCentre’

Do you know maybe what can be reason for that ?
Currently I am using 2.1.0 OpenFOAM.

Do you know maybe if it is possible to use groovyBC it this case ?

Best and thank you
ZM

[ziemowitzima]

Dear Bigphil

I tried your method to customize directionMixed BC but I could not compile my code.
I got following errors:

error: ‘directionMixedFvPatchVectorField’ was not declared in this scope
error: ‘loadingIndex’ was not declared in this scope
error: ‘const class FoamolyPatch’ has no member named ‘faceCentre’

Do you know maybe what can be reason for that ?
Currently I am using 2.1.0 OpenFOAM.

Do you know maybe if it is possible to use groovyBC it this case ?

Best and thank you
ZM

[bigphil]

Hi ZM,

Actually there is a small mistake in my previous code snippet:
this line:

vectorField n = mesh.boundary()[loadingIndex].nf();

should be

vectorField n = mesh.boundary()[patchID].nf();

and

const vectorField& patchFaceCentres = mesh.boundaryMesh()[patchID].faceCentre();

should be

const vectorField& patchFaceCentres = mesh.boundaryMesh()[patchID].faceCentres();

And also, you need to tell your solver about the directionMixed class, so add the following line under #include "fvCFD.H":

#include "directionMixedFvPatchFields.H"

Philip

[ziemowitzima]

Hi Philip
Thanks a lot !
There is one more error:
error: ‘Foam::directionMixedFvPatchVectorField’ has no member named ‘refGradient’

but I corrected it:
instead:
Upatch.refGradient() = patchFaceCentres * runTime.value();

should be:

Upatch.refGrad() = patchFaceCentres * runTime.value();
Thanks again
-ZM

[bigphil]

Great,

hopefully it'll do what you want.

In answer to your earlier question, I would say that groovy/swak4Foam can more than likely do what you want also, but I have never used it.

Philip

[Sherlock_1812]

Greetings.

I have got a fairly clear idea about directionMixed Bc from this thread. Thank you!

I have one question though (may be trivial, but still).

What are the three components of the vector given as input to refGradient in cartesian notations? Example, if refGradient is (-1 0 0) is dv1/dx= -1 or dv1/dz?

How does one assign partial du/dy and/or partial dv/dx alone using this bc?

[bigphil]

Originally Posted by Sherlock_1812

Greetings.

I have got a fairly clear idea about directionMixed Bc from this thread. Thank you!

I have one question though (may be trivial, but still).

What are the three components of the vector given as input to refGradient in cartesian notations? Example, if refGradient is (-1 0 0) is dv1/dx= -1 or dv1/dz?

How does one assign partial du/dy and/or partial dv/dx alone using this bc?

Hi,

refGradient is (-1 0 0) means:
dvx/dn = -1
dvy/dn = 0
dvz/dn = 0
where vx, vy, vz are the cartesian components of vector field v (e.g. velocity) and n is the patch normal direction.

Keep in mind, the valueFraction will control the fraction of the refValue used and the fraction of the refGradient used.

Philip

[Sherlock_1812]

Thank you Philip!

[Sherlock_1812]

Originally Posted by bigphil

If your patch faces have all different normals then you will have to set the patch valueFraction in the solver (using refCast etc.) to be symm(n*n).

Hi Philip,

I'm not able to understand what changes are to be made to valueFraction in the above case (using refCast?). I have a curved patch where face normals are different for different faces, so I see that I should do what you've said. My C++ isn't that good. Can you elaborate?

If two faces in a patch have different normals n1 and n2, then the valueFraction is given by symm(n1*n2)? Is this right?

Thanks in advance,

[bigphil]

Originally Posted by Sherlock_1812

Hi Philip,
If two faces in a patch have different normals n1 and n2, then the valueFraction is given by symm(n1*n2)? Is this right?

It depends on what condition you want to impose;
in the case where you would like the normal component to be fixedValue and the tangential components to be fixedGradient then you fix the face valueFraction to be symm(n*n) where n is the face normal.

e.g.
if you have a list of faces (f1, f2, f3, …) with face normals (n1, n2, n3, …) then you would set the valueFractions to be symm(n1*n1), symm(n2*n2), symm(n3*n3), …

Philip

[Sherlock_1812]

Thank you for your quick reply Philip