[Linse]

Hello all!

According to some standard books (Patankar, Versteeg, etc.), the common way of solving CFD-problems (abbreviatedly) consists of getting the equations into a form of aX + bX + cX = D, which is put into a matrix A of coefficients a, b and c and two vectors of X and D, basically giving a system [A] X = D.
Several steps are needed for solving this equation system, among others
- getting a, b and c into a form that makes [A] consisting of one diagonal of values instead of three (use of recurrence relations)
- calculating the actual value for X based on the results of the recurrence calculations

My question now is:
In which parts of the code are these steps done?
And how could these steps be manipulated?
Ideally I would like to access the equations/matrices on a cell-level and change/control them cell-wise...

I guess I will have to manipulate the matrices themselves, but how is that done? Any information/pointing to information would be highly welcome!

Thank you all in advance!

[andyru]

Hi,

if you look into the solver ico-Foam for example, the main coefficients of the matrix are calculated with function A():

volScalarField rUA = 1.0/UEqn.A();

Here you can acces them an manipulate them.

forAll(rUA,celli)
{
...
}

So, this depends, what you want to do?

I'm facing almost the same problem and I need to manipulate the source term grad(vsf) (Manipulating source fvc::grad(vsf1+vsf2))

What is your physical application?


Greetings

Andy

[santiagomarquezd]

Originally Posted by Linse

Hello all!

According to some standard books (Patankar, Versteeg, etc.), the common way of solving CFD-problems (abbreviatedly) consists of getting the equations into a form of aX + bX + cX = D, which is put into a matrix A of coefficients a, b and c and two vectors of X and D, basically giving a system [A] X = D.
Several steps are needed for solving this equation system, among others
- getting a, b and c into a form that makes [A] consisting of one diagonal of values instead of three (use of recurrence relations)
- calculating the actual value for X based on the results of the recurrence calculations

My question now is:
In which parts of the code are these steps done?
And how could these steps be manipulated?
Ideally I would like to access the equations/matrices on a cell-level and change/control them cell-wise...

I guess I will have to manipulate the matrices themselves, but how is that done? Any information/pointing to information would be highly welcome!

Thank you all in advance!

The questions are not so clear. I could help but I can't understand the problem.

Regards.

[j-avdeev]

Propably, I have same problem.
I want to save matrices A to separate file (A from AX=D).

http://openfoamwiki.net/index.php/Op...x_coefficients

OpenFOAM stores:

• diagonal coefficients as a scalar field, indexed by cell volume; and
• off-diagonal coefficients as two scalar fields, indexed by face centres.

lduAddressing is used to related the two indexing methods.

but how to write it in separate file?

[elvis]

I guess they want to do something similar that
Santiago Marquez Damian described in his post Can someone tell me more about vulashaka

[santiagomarquezd]

Maybe you need http://openfoamwiki.net/index.php/Contrib_gdbOF, it has an specific tool to do that.

Regards

[j-avdeev]

Santiago, yes, GdbOF looks like what I want.
I've read GdbOF-Manual.pdf - it has a lot of, but very general examples like

Example 3 "View Boundary Field values with gdbOF"

$ (gdb) ppatchvalues vSF 0

and not written exactly when, from which directory I have to type this command.
Maybe it's very simple for describing - but I need at least one step-by-step example.

I like example from (gdb)+OF

go to cavity tutorial directory
$cd cavity
run icoFoam in debug
$gdb icoFoam
create breakpoint
$b icoFoam.C:77

$run
There are two ways of stepping in the file:

$n (next) will step to the next line in the current file, but will not go into functions and
included files.
$s (step) will go to the next line, also in functions and included files.

- I want similar, but for GdbOF (with pfvmatrixfull or pfvmatrixsparse commands).

Can someone describe sequence of commands for describing? Or correct me, if I do something wrong.

[santiagomarquezd]

Well, it suppose some basic knowledge about gdb as a pre-requisite, tell us which solver do you want to debug and what system within it.

Regards

[j-avdeev]

Solver - let it be simpleFoam.
Which solver to use - not matter for me (at least I think so now).

What system within solver... == what algoritm of solver?

About simpleFoam exist article here The_SIMPLE_algorithm_in_OpenFOAM
but equations of solver far from Ax=b (it would be cool for me to know this moment, where equation like

fvm::div(phi, U) - laplacian(nu, U)

become single matrix like A or I wrong?)

Also if needs case for example of debugging - it could be
$FOAM_TUTORIALS/incompressible/simpleFoam/pitzDaily

Thanks.

[santiagomarquezd]

Well,

Originally Posted by j-avdeev

it would be cool for me to know this moment, where equation like

fvm::div(phi, U) - laplacian(nu, U)

become single matrix like A or I wrong?)

it's a long story about FVM discretization and C++ implementation, but in order to be helpful, suppose you're solving a tutorial for scalarTransportFoam and you want to see the equation for following lines in scalarTransportFoam.C (the scalar advection diffusion equation without sources)

00058             solve
00059             (
00060                 fvm::ddt(T)
00061               + fvm::div(phi, T)
00062               - fvm::laplacian(DT, T)
00063             );

then go the case directory, for eample $FOAM_TUTORIALS/basic/scalarTransportFoam/pitzDaily and start gdb

$ gdb scalarTransportFoam

once you you're within gdb:

$ start
$ b fvMatrixSolve.C:140
$ continue
$ pfvmatrixfull this AdvDiff.dat
$ shell cat AdvDiff.dat

these lines will show you the matrix for this system. You also can read the AdvDiff.dat in octave or Matlab as a matrix.

Regards.