CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   Meaning of "fvc::div(phi)" (https://www.cfd-online.com/Forums/openfoam-programming-development/97922-meaning-fvc-div-phi.html)

 enoch February 28, 2012 11:51

Meaning of "fvc::div(phi)"

Hi Foamers,

When I look at pEqn.C in the "twoPhaseEulerFoam" solver, I don't really understand the following codes.

.......
for(int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++)
{
fvScalarMatrix pEqn
(
fvm::laplacian(Dp, p) == fvc::div(phi)
);
.....

Speaking of div(phi), divergence of any scalar is zero mathematically.

Divergence reduce the order rank of maxtrix.
For an example, let's say, velcotiy vector u=(ux, uy)

div(u)=ux/dx + uy/dy ---> scalar quantity

But, scalar phi=phi(x,y)
div(phi)=0

So what is the meaning of div(phi) and what's a mathematical formulation for the term in openfoam?

 sharonyue July 16, 2013 04:01

Hi Kim,

This problem happens to me in the same time!http://www.cfd-online.com/Forums/ope...-equation.html Did you find a solution?

 fportela July 16, 2013 06:01

Isn't phi simply the mass flux rho*U*A ? check this
HTML Code:

http://openfoamwiki.net/index.php/Uguide_table_of_fields
and this
HTML Code:

http://openfoamwiki.net/index.php/Main_FAQ#What_is_the_field_phi_that_the_solver_is_writing
I have not used this particular solver, so I'm not sure what's going on, but from continuity: div(phi) = 0 implies that ddt(rho) is zero, if this is not the case, then div(phi) is not zero.

Cheers,
Felipe

 sharonyue July 16, 2013 08:31

Hi Felipre,

Quote:
 Originally Posted by fportela (Post 440008) but from continuity: div(phi) = 0
regarding this, isnt it should be div(u)=0?

 Bernhard July 16, 2013 08:35

No, because U is the cell centre value, and the divergence is obtained from the face values, i.e. phi.

 sharonyue July 16, 2013 08:38

Hi Bernhard,
Could you explain more?

 Bernhard July 16, 2013 08:39

Can you be more specific?

 sharonyue July 16, 2013 08:44

Quote:
 Originally Posted by Bernhard (Post 440031) No, because U is the cell centre value, and the divergence is obtained from the face values, i.e. phi.
I mean all the books say from continuity we have: without mentioning whether its cell centre value or the face value. But Im sure I confused about this. So?

 Bernhard July 16, 2013 08:49

The book are correct, but http://www.cfd-online.com/Forums/vbL...5ac33fb3-1.gif is valid without a mesh. If you integrate this equation over a control volume, this converts to a summation over the faces of the velocity times the area ( http://en.wikipedia.org/wiki/Divergence_theorem ). phi is nothing less then the velocity at the face (times the density and the face area).

 fportela July 16, 2013 08:51

Quote:
 Originally Posted by sharonyue (Post 440034) I mean all the books say from continuity we have: without mentioning weather its cell centre value or the face value. But Im sure I confused about this. So?
This is only true for incompressible flow.

For incompressible flow, you have

Plug this into continuity

And you get

 sharonyue July 16, 2013 09:24

Quote:
 Originally Posted by Bernhard (Post 440037) The book are correct, but http://www.cfd-online.com/Forums/vbL...5ac33fb3-1.gif is valid without a mesh. If you integrate this equation over a control volume, this converts to a summation over the faces of the velocity times the area ( http://en.wikipedia.org/wiki/Divergence_theorem ). phi is nothing less then the velocity at the face (times the density and the face area).

I know this, but phi is a scalar, what is div(scalar).....

Felipe. Yeah, you are right~

 Bernhard July 16, 2013 09:27

Quote:
 Originally Posted by sharonyue (Post 440049) I know this, but phi is a scalar, what is div(scalar).....
Be careful here. phi is a surfaceScalarField, so there is always a direction vector defined by the face area vector.

 sharonyue July 16, 2013 09:56

Regarding this, if div(phi)=0 Do you mean:

Quote:
 phi is a surfaceScalarField, so there is always a direction vector defined by the face area vector
Is there any difference between "surfaceScalarField" and "volScaklaField" expect where they are stored?

 Bernhard July 16, 2013 10:01

You apply the divergence theorem.

You can't integrate face values over a volume as you are posting.

The difference between a volScalarField and a surfaceScalarField, is that for a volScalarField, there is a value stored per control volume or cell. For a surfaceScalarField there is a value stored per face.

You can of course interpolate from the one to the other, but this is only accurate to some order.

 sharonyue July 16, 2013 10:23

Quote:
 Originally Posted by Bernhard (Post 440063) You apply the divergence theorem. You can't integrate face values over a volume as you are posting. The difference between a volScalarField and a surfaceScalarField, is that for a volScalarField, there is a value stored per control volume or cell. For a surfaceScalarField there is a value stored per face. You can of course interpolate from the one to the other, but this is only accurate to some order.
Bernhard, Thanks very very much for your consistent help, But I still cannot understand this "div(u)=0" turns into "div(phi)=0" in OpenFOAM, even mathematicly div(vector) works but div(scalar) not.
Does it mean fvc::div(phi)=0 equals to sum(phi)=0 in OpenFOAM? Why doesnt it use sum(phi)=0 instead.
At last,I think I need to clear my head. Thanks for you patience. Really thankful.:)

 sharonyue July 17, 2013 23:52

1 Attachment(s)
Im still confused!!!!!!

div(u)=0 I know its meaning.

1) If via continuity, we have div(phi)=0, then we make an intergration on this equation like this:

[LaTeX Error: Syntax error]

Is this weird?

 Bernhard July 18, 2013 01:59

Yes, this is extremely weird. phi only lives in the discretized domain on faces of cells. The is no way you can do a volume integral over such a variable.

Do you know how to derive the equation ? You can do this using a mass-micro-balanse. This has not yet anything to do with a mesh, but if you understand this, it is easily translated.

 sharonyue July 18, 2013 18:46

Quote:
 Originally Posted by Bernhard (Post 440449) Yes, this is extremely weird. phi only lives in the discretized domain on faces of cells. The is no way you can do a volume integral over such a variable. Do you know how to derive the equation ? You can do this using a mass-micro-balanse. This has not yet anything to do with a mesh, but if you understand this, it is easily translated.
Yeah, Im very clear about this , and I know after intergral it can be a sum. I dont know whether you know what I dont know.
Code:

fvScalarMatrix pEqn                 (                     fvm::laplacian(rAU, p) == SUM(phiHbyA)//If there existed "SUM"                 );
Even I can understand this. But I cannot understand fvc::div(phiHbyA).
Anyway thanks bro.

BTW, the unit of fvc::div(u) and fvc::div(phi) is the same:
Code:

fvc::div(HbyA):dimensions      [0 0 -1 0 0 0 0]; internalField  nonuniform List<scalar> 9(0.157469 -0.0674757 -0.487085 -0.960691 0.789192 0.715649 30.1762 0.258981 -30.5822); fvc::div(phiHbyA):dimensions      [0 0 -1 0 0 0 0]; internalField  nonuniform List<scalar> 9(-0.435688 -0.0982547 0.152804 -0.0448476 0.720155 -0.152663 28.2072 0.236062 -28.5848);

 ARTem July 22, 2013 04:01

Take into account that mathematical and OpenFOAM's languages are different.
Originally, mathematical divergence is vector operation that gives you source or sink at a point. When you use finite volume method to discretize differential equation, you get linear form of diff. equation and volumes to store discrete variables. That's why in order to get divergence you should firstly compute fluxes at volume faces.
In OF there are two ways to compute divergence:
1) take fvc::div( of volVectorField ). You can see in sources, it calls for fvc::surfaceIntegrate ( volVectorField & mesh.Sf() ).
2) make first step manually (i.e. phi = U&mesh.Sf()) and call for fvc::div( surfaceScalarField phi ). Again, OF will make fvc::surfaceIntegrate ( surfaceScalarField ).
Mathematically div(scalar phi) has no sense. Because you think of variables as continuous fields, but in OF variables are discrete fields.

You are partially right, there is no "SUM", but "surfaceIntegrate" called by OF to compute div.

And again, phi = U & mesh.Sf(). div(phi) = div(U) = div(U&mesh.Sf()). That's why you get same dimensions.

 sharonyue August 23, 2013 00:08

Quote:
 Originally Posted by ARTem (Post 441149) Take into account that mathematical and OpenFOAM's languages are different. Originally, mathematical divergence is vector operation that gives you source or sink at a point. When you use finite volume method to discretize differential equation, you get linear form of diff. equation and volumes to store discrete variables. That's why in order to get divergence you should firstly compute fluxes at volume faces. In OF there are two ways to compute divergence: 1) take fvc::div( of volVectorField ). You can see in sources, it calls for fvc::surfaceIntegrate ( volVectorField & mesh.Sf() ). 2) make first step manually (i.e. phi = U&mesh.Sf()) and call for fvc::div( surfaceScalarField phi ). Again, OF will make fvc::surfaceIntegrate ( surfaceScalarField ). Mathematically div(scalar phi) has no sense. Because you think of variables as continuous fields, but in OF variables are discrete fields. You are partially right, there is no "SUM", but "surfaceIntegrate" called by OF to compute div. And again, phi = U & mesh.Sf(). div(phi) = div(U) = div(U&mesh.Sf()). That's why you get same dimensions.
U make it very very clear, Thanks very much. So I just make it a example.:

1. volVectorField U;
fvc::div(U);

2. volVectorField U;
phi = U & mesh.Sf();
fvc::div(phi);

So these two functions are the same rite? fvc::div(u)=fvc::div(phi).

Looks like div() has been overloaded.

I make a testify:

Code:

fvc::div(HbyA)dimensions      [0 0 -1 0 0 0 0]; internalField  nonuniform List<scalar> 9(0.000569046 -8.589e-06 -0.000648869 -0.00128281 0.000183935 0.00124553 0.00416702 3.71583e-06 -0.00422898); fvc::div(phiHbyA):dimensions      [0 0 -1 0 0 0 0]; internalField  nonuniform List<scalar> 9(0.000569046 -8.589e-06 -0.000648869 -0.00128281 0.000183935 0.00124553 0.00416702 3.71583e-06 -0.00422898);
Its total the same. Good job.

All times are GMT -4. The time now is 02:05.