Meaning of "fvc::div(phi)"

enoch · February 28, 2012, 11:51

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, 05:01

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, 07:01

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, 09:31

Hi Felipre,

Thanks for your prompt reply,

Quote:

Originally Posted by fportela

but from continuity: div(phi) = 0

regarding this, isnt it should be div(u)=0?

Bernhard · July 16, 2013, 09:35

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

sharonyue · July 16, 2013, 09:38

Hi Bernhard,
Could you explain more?

Bernhard · July 16, 2013, 09:39

Can you be more specific?

sharonyue · July 16, 2013, 09:44

Quote:

Originally Posted by Bernhard

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: $\nabla \cdot u=0$ without mentioning whether its cell centre value or the face value. But Im sure I confused about this. So?

Bernhard · July 16, 2013, 09:49

The book are correct, but

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, 09:51

Quote:

Originally Posted by sharonyue

I mean all the books say from continuity we have: $\nabla \cdot u=0$ 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 $\frac{D\rho}{Dt} = \frac{\partial\rho}{\partial t} + \vec{u} \cdot \nabla (\rho) = 0$

Plug this into continuity

$\frac{\partial\rho}{\partial t} + \nabla (\rho \vec{u}) = 0$

And you get

$\nabla \cdot \vec{u} = 0$

sharonyue · July 16, 2013, 10:24

Quote:

Originally Posted by Bernhard

The book are correct, but

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).

$\int\limits_V^{} {\nabla \cdot udV} = \sum\limits_f {{u_f} \cdot {S_f} = 0}$

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

Felipe. Yeah, you are right~

Bernhard · July 16, 2013, 10:27

Quote:

Originally Posted by sharonyue

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, 10:56

$\int\limits_V^{} {\nabla \cdot udV} = \sum\limits_f {{u_f} \cdot {S_f} = 0}$

Regarding this, if div(phi)=0 Do you mean:
$\int\limits_V^{} {u_f \cdot S_fdV} = 0$

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, 11:01

You apply the divergence theorem.
$\int\limits_V^{} {\nabla \cdot udV} = \int\limits_{\partial V}u\cdot\hat{n}dS =\sum\limits_f {{u_f} \cdot {S_f} = 0}$
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, 11:23

Quote:

Originally Posted by Bernhard

You apply the divergence theorem.
$\int\limits_V^{} {\nabla \cdot udV} = \int\limits_{\partial V}u\cdot\hat{n}dS =\sum\limits_f {{u_f} \cdot {S_f} = 0}$
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 18, 2013, 00:52

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, 02:59

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 $\nabla\cdot\vec{u}$ ? 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, 19:46

Quote:

Originally Posted by Bernhard

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 $\nabla\cdot\vec{u}$ ? 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 $\nabla\cdot\vec{u}$ , 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, 05:01

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, 01:08

Quote:

Originally Posted by ARTem

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.

February 28, 2012, 11:51	Meaning of "fvc::div(phi)"	#1
enoch Member Jeong Kim Join Date: Feb 2010 Posts: 42 Rep Power: 16	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? Zhiheng Wang, qwebean and nepomnyi like this.

July 16, 2013, 05:01		#2
sharonyue Senior Member Dongyue Li Join Date: Jun 2012 Location: Beijing, China Posts: 849 Rep Power: 18	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? Zhiheng Wang likes this.

July 16, 2013, 07:01		#3
fportela Member Felipe Alves Portela Join Date: Dec 2012 Location: FR Posts: 70 Rep Power: 14	Isn't phi simply the mass flux rhoUA ? 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 elmo555 likes this.

July 16, 2013, 09:35		#5
Bernhard Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 22	No, because U is the cell centre value, and the divergence is obtained from the face values, i.e. phi. fportela, utkunun, randolph and 1 others like this.

July 16, 2013, 09:38		#6
sharonyue Senior Member Dongyue Li Join Date: Jun 2012 Location: Beijing, China Posts: 849 Rep Power: 18	Hi Bernhard, Could you explain more? Zhiheng Wang likes this.

July 16, 2013, 09:39		#7
Bernhard Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 22	Can you be more specific? Zhiheng Wang likes this.

July 16, 2013, 09:49		#9
Bernhard Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 22	The book are correct, but 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). Kummi, SHUBHAM9595 and fly_light like this.

July 16, 2013, 11:01		#14
Bernhard Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 22	You apply the divergence theorem. $\int\limits_V^{} {\nabla \cdot udV} = \int\limits_{\partial V}u\cdot\hat{n}dS =\sum\limits_f {{u_f} \cdot {S_f} = 0}$ 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. fportela, flowAlways, acs and 1 others like this.

July 18, 2013, 02:59		#17
Bernhard Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 22	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 $\nabla\cdot\vec{u}$ ? 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.

July 22, 2013, 05:01		#19
ARTem Member Artem Shaklein Join Date: Feb 2010 Location: Russia, Izhevsk Posts: 43 Rep Power: 16	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. zjdedongxi, sharonyue, reza2031 and 20 others like this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Cyclic Boundary creation, what's the meaning of "separationVector"	panda60	OpenFOAM	5	April 12, 2023 18:51
What's meaning of UDF FUNCTION	zhaoxinyu	Fluent UDF and Scheme Programming	0	March 31, 2010 09:04
meaning of residual p-mass ?	Dele	CFX	0	March 4, 2008 04:23
want to know meaning	Sangamesh	Siemens	0	May 15, 2007 06:15
What's the meaning of "combustion scalar"and....	cfdbeginner	CFX	0	November 27, 2003 10:02