# Meaning of "fvc::div(phi)"

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

 February 28, 2012, 11:51 Meaning of "fvc::div(phi)" #1 Member   Jeong Kim Join Date: Feb 2010 Posts: 42 Rep Power: 8 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?

 July 16, 2013, 04:01 #2 Senior Member   Dongyue Li Join Date: Jun 2012 Location: Torino, Italy Posts: 742 Rep Power: 9 Hi Kim, This problem happens to me in the same time!icoFoam's pressure possion equation. Did you find a solution?

 July 16, 2013, 06:01 #3 Member   Felipe Portela Join Date: Dec 2012 Location: London Posts: 64 Rep Power: 5 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 elmo555 likes this.

July 16, 2013, 08:31
#4
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9
Hi Felipre,

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

 July 16, 2013, 08:35 #5 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 14 No, because U is the cell centre value, and the divergence is obtained from the face values, i.e. phi.

 July 16, 2013, 08:38 #6 Senior Member   Dongyue Li Join Date: Jun 2012 Location: Torino, Italy Posts: 742 Rep Power: 9 Hi Bernhard, Could you explain more?

 July 16, 2013, 08:39 #7 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 14 Can you be more specific?

July 16, 2013, 08:44
#8
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9
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: without mentioning whether its cell centre value or the face value. But Im sure I confused about this. So?

 July 16, 2013, 08:49 #9 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 14 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).

July 16, 2013, 08:51
#10
Member

Felipe Portela
Join Date: Dec 2012
Location: London
Posts: 64
Rep Power: 5
Quote:
 Originally Posted by sharonyue 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

July 16, 2013, 09:24
#11
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9
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).

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

Felipe. Yeah, you are right~

July 16, 2013, 09:27
#12
Senior Member

Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 14
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.

July 16, 2013, 09:56
#13
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9

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?

 July 16, 2013, 10:01 #14 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 14 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. fportela and flowAlways like this.

July 16, 2013, 10:23
#15
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9
Quote:
 Originally Posted by Bernhard 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.

July 17, 2013, 23:52
#16
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9
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?
Attached Images
 1.jpg (11.9 KB, 37 views)

 July 18, 2013, 01:59 #17 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 14 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.

July 18, 2013, 18:46
#18
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9
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 ? 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);

 July 22, 2013, 04:01 #19 Member   Artem Shaklein Join Date: Feb 2010 Location: Russia, Izhevsk Posts: 43 Rep Power: 8 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, shipman and 5 others like this.

August 23, 2013, 00:08
#20
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9
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.

Last edited by sharonyue; August 23, 2013 at 03:35.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post panda60 OpenFOAM 0 June 1, 2010 10:13 zhaoxinyu Fluent UDF and Scheme Programming 0 March 31, 2010 08:04 Dele CFX 0 March 4, 2008 04:23 Sangamesh CD-adapco 0 May 15, 2007 05:15 cfdbeginner CFX 0 November 27, 2003 10:02

All times are GMT -4. The time now is 18:27.