[Reptider]

Hello!
I have created the body with blockMesh. I suggest that there are cells within the body.
My problem is to create own solver by which I fill each cell by certain value, for example, temperature = 5.
I have created initial conditions for T in the "0" file and created the "createFields.H" file, where defined values of field are read, it looks like:

volScalarField T
(
    IOobject
    (
        "T",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

So then I would like to use "forAll" for changing already defined values in each cells like that:

forAll(T, i)
{
	...
}

How can I do that?
What should I do for see these values (fields) in paraview?

[geth03]

why don't you just use setFieldsDict?
it would be more flexible.

[Reptider]

Originally Posted by geth03

why don't you just use setFieldsDict?
it would be more flexible.

I need to understand how to work with "forAll", because after that I must use "topoSet" to define zones of my body and go through the cells of each zones and assign special values for them.

[geth03]

i see.

after defining your zone in topoSet you need to access the cells:

word myZone = "nameGivenInTopoSetDict";
label zoneID = mesh.cellZones().findZoneID(myZone);
const labelList& cells = mesh.cellZones()[zoneID];
forAll(cells, i)
{
const label cell = cells[i];
T[cell] = yourValue; //keep in mind that you need to match Unit also!
}

//repeat for other zones!

[Reptider]

Originally Posted by geth03

i see.

after defining your zone in topoSet you need to access the cells:

word myZone = "nameGivenInTopoSetDict";
label zoneID = mesh.cellZones().findZoneID(myZone);
const labelList& cells = mesh.cellZones()[zoneID];
forAll(cells, i)
{
const label cell = cells[i];
T[cell] = yourValue; //keep in mind that you need to match Unit also!
}

//repeat for other zones!

Thank you!
Could you give me another advice what should I write in the solver that is responsible for sending cells to paraview? (Create "Cell Arrays" under "Mesh regions").
ParaView doesn't see new partial temperatures ( "T(partial)" ), but see created cellZones. They're represented by different colours. I can choose old T(partial) only which shows zero values at each cells (when "internalMesh" is chosen"). I have attached paraView interface: https://ibb.co/DrNqG8V.
In addition to this, I've noticed that new time has appeared (1 sec). How can I avoid this?

[geth03]

look at this T-object:

volScalarField T
(
IOobject
(
"T",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

if you create a volScalarField as IOobject it means it is an input-output object, which means the solver can read and/or write data, so paraview can find it in the time-directories. if you write AUTO_WRITE it will create a T-file in every output directory that you can open with paraview, the files will be updated when your solver calls the function runTime.write().

you decide in controlDict under writeInterval when runtime.write() should be called. if you change your T-field in the solver manually with cellZones and later on let the solver update the field by solving an equation you will see the field which is provided by the result of the equation for T.

if you initialize your T-field in the 0-directory with 0-entries for the internal mesh it is normal that in the old timestep which is time=0 sec that paraview shows only 0 Kelvin.

[Reptider]

Originally Posted by geth03

look at this T-object:

volScalarField T
(
IOobject
(
"T",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

if you create a volScalarField as IOobject it means it is an input-output object, which means the solver can read and/or write data, so paraview can find it in the time-directories. if you write AUTO_WRITE it will create a T-file in every output directory that you can open with paraview, the files will be updated when your solver calls the function runTime.write().

you decide in controlDict under writeInterval when runtime.write() should be called. if you change your T-field in the solver manually with cellZones and later on let the solver update the field by solving an equation you will see the field which is provided by the result of the equation for T.

if you initialize your T-field in the 0-directory with 0-entries for the internal mesh it is normal that in the old timestep which is time=0 sec that paraview shows only 0 Kelvin.

Yeah! I appreciate your help!
I've got that code:

word one_sec = "1";
    while (runTime.loop())
    { 
          Info<< "Time = " << runTime.timeName() << endl;
          if ( runTime.timeName() == one_sec )
          {
          	Info<< "\nSet up certain values for cellZones\n" << endl;
                word myZone1 = "cs1";
    		label zoneID1 = mesh.cellZones().findZoneID(myZone1);
    		const labelList& cells1 = mesh.cellZones()[zoneID1];
    		forAll(cells1, i)
    		{
    		const label cell = cells1[i];
    		T[cell] = 5;
    		}
    
    		word myZone2 = "cs2";
    		label zoneID2 = mesh.cellZones().findZoneID(myZone2);
    		const labelList& cells2 = mesh.cellZones()[zoneID2];
    		forAll(cells2, j)
    		{
    		const label cell = cells2[j];
    		T[cell] = 25;
    		}
    
    		word myZone3 = "cs3";
    		label zoneID3 = mesh.cellZones().findZoneID(myZone3);
    		const labelList& cells3 = mesh.cellZones()[zoneID3];
    		forAll(cells3, k)
    		{
    		const label cell = cells3[k];
    		T[cell] = 100;
    		}
    		
    		runTime.write(); 		
          }
     }

It creates the new file "1" at the directory of programm. Now I can see changed T field in paraview at 1 sec.